This is just one of some 80 files about machining and metalworking and useful workshop subjects that can be read at: http://www.janellestudio.com/metal/index.html ------------------------------------------------------------------ Here find many users' tips on milling procedures, using a milling machine or using a milling attachment on a metal lathe. Milling tips here are generic for the most part. If the conversation is about a specific brand of mill, it is likely that you can adapt the procedure or tip here to your particular model and needs. There is another file here called Atlas Lathe Milling, which will provide lots of tips about milling procedures using an Atlas or other metal lathe. Another text file here called Cutters, Bits, and Arbors has useful discussions including milling cutters -- types and use and sharpening. There are many situations where a SHAPER may be a viable alternative to a MILL. Certainly the ability to easily create and sharpen bits at home for the shaper, whereas mill cutters are always expensive to buy, is something to consider. (A whole shaper can be bought for the price of a handful of larger mill cutters.) But one case, a blind ended T-slot, is probably better handled by a mill cutter. There is a conversation to this effect in the Shaping Tips file. See messages there starting: 27 Jan 2004 From: n8as1x~xxaol.com Subject: Re: Re: what's going on in your shop? Why not read all the shaper files? Can't hurt to learn something new :-) If you got to this file directly from my HOME PAGE, return there by using your browser's back button. BUT if you came to this file as the result of a web search engine, see many additional files on my home page Machining and Metalworking at Home http://www.janellestudio.com/metal/index.html SAFETY WARNING BEWARE: DO NOT ASSUME that any subject matter or procedure or process is safe or correct or appropriate just because it was mentioned in a news/user group or was included in these files or on this site or on any other web site or was published in a magazine or book or video. Working with metals and machinery and chemicals and electrical equipment is inherently dangerous. Wear safety devices and clothing as appropriate. Remove watches, rings, and jewellery -- and secure or remove loose clothing -- before operating any machine. Read, understand and follow the latest operating procedures and safety instructions provided by the manufacturer of your machine or tool or product. If you do not have those most recent official instructions, acquire a copy through the manufacturer before operating or using their product. Where the company no longer exists, use the appropriate news or user group to locate an official copy. Be careful -- original instructions may not meet current safety standards. Updated safety information and operating instructions may also be available through a local club, a local professional in the trade, a local business, or an appropriate government agency. In every case, use your common sense before beginning or taking the next step; and do not proceed if you have any questions or doubts about any procedure, or the safety of any procedure. Follow all laws and codes, and employ certified or licenced professionals as required by those laws or codes. Hazardous tasks beyond your competence or expertise should also be contracted to professionals. Let's be really careful out there. (c) Copyright 2003 - 2016 Machining and Metalworking at Home The form of the collected work in this text file (including editing, additions, and notes) is copyrighted and this file is not to be reproduced by any means, including electronic, without written permission except for strictly personal use. ========================================================================= From: Gregory Gagarin Date: Sun Jan 2, 2000 9:22pm Subject: Re: Sherline Mill Tramming/Tooling Plate Yury, I use a Sherline 5400 mill which is now 1 1/2 years old and get very good high precision (0.001" or better)results. I do have 2-3 thousands spongyness in the column/headstock relative to the table, as you described, but this rarely causes problems if you make sensible cuts and finish with a light cut and a sharp tool at high RPM (don't lean on the column or motor while moving the Z-axis handwheel). I think this is normal (you have a lot of leverage there on relatively small structures) but it returns to a stable alignment and I've never seen mine "knocked" out of alignment in normal use. The bigger concern is the Z axis stick and release tendancy which has been addressed many times in this group (see previous posts). In reading your post, I see several possible sources of error: 1. Cheap surface plate -- not a player. Cheap angle plate -- probably not a problem as you can shim to square. Cheap square -- big problem. Your square is your primary reference in setting up the mill for which I am aware of no work-around. Woodworking squares are totally useless and good machine shop squares are expensive. I use the relatively "inexpensive" Mitutoyo grade B (made in England) squares -- I have 3 different sizes which is convienient. They are not the best but are within about 0.0006" of square end-to-end. This is a good place to spend your money and something to take good care of. I assume you have a good working procedure for squaring the mill that ends in a spindle sweep of a flat table surface. For my mill, the table surface is not flat on the X-Y plane -- it is 0.0015" low at the back (x-axis) edge -- so I have to shim my square for all subsequent alignment steps and put a 0.0015 shim under the back edge of all setups on the mill table. 2. I find the use of a Dial Indicator (DI) very awkward for squaring the mill. I have a B&S DI(0.001") which I rarely use. I have 2 Dial TEST Indicators (DTI) (B&S Bestest and Mitutoyo #513-112 -- both 0.0005") which I use all of the time. The "touch" of a DTI is very light compared to a DI. I can set my square on the mill table and sweep the edge of the square with a DTI in the spindle without moving the free-standing square. I particularly like the Mitutoyo DTI since it is a "barrel" type with a .375" stem which can be held in the .375" end mill holder on the spindle and, with its 1.5" long tip, can sweep almost a 3" diameter circle without other holding attachments. This is particularly useful for checking square prior to flycutting as it covers approximately the same area. 3. Machining large flat surfaces with multiple setups is fraught with difficulty -- this is where large mills and surface grinders reign supreme. Insure that you use the same reference surfaces for all setups -- this may require an externally held DTI setup (such as a magnetic base indicator holder) in order to reach the reference surfaces when you move the stock for subsequent cuts. An alternative to simplify your task may be to machine two or three smaller pads for the finished plate to rest on vice the whole surface -- this is how the head attaches to the lathe bed and mill saddle (note that the center protion of the surfaces is milled out to limit contact to the outer surfaces simplifying the milling). 4. Metals warp. When you machine away surfaces on, or drill/bore large holes in, metal plates you may relieve internal stresses resulting in warpage -- this can be significant and varies with metal type, forming process and heat treatment. I always try to reserve my finishing cuts on precision critical surfaces until the bulk of metal removal is complete and the stock has been allowed a day or so to "cure". There are others in this group who can tell you a lot more about this -- I'm certainly no expert. 5. Fly cutting. You will normally get a slight cut on the back side of the circle due to flexing during a heavy cut but this should almost disappear in very light finishing cuts -- leaves a nice flat irridescent surface of crisscrossing circles. The back cut should never completely disappear since it is cutting across the "grain" of the leading cuts where there are always ridges in the cuts that should be in contact if your equipment is square. You can see the intersecting edges between cuts but should not be able to feel them on the surface with your fingernail -- a DTI sweep across these edges should show less than 0.0005". It sounds like you may not have the mill spindle square and perpendicular to the surface -- check it with a large DTI circular spindle sweep. Also, make sure your spindle and flycutter MT1 surfaces are clean and that the flycutter is properly seated. Lock the Z-axis firmly prior to each cut initiation. Hope you find this helpful -- don't scrap your mill yet as it should serve you well within the limits of its design. Greg ------- From: Gregory Gagarin Date: Tue Jan 4, 2000 2:15pm Subject: Re: Sherline Mill Tramming/Tooling Plate Yury, when I said that my table was low on the back side by 0.0015", what I meant was that the entire "table assembly" (everything above the X-Y plane of motion) was "thiner" at the back than at the front. The table plane is not parallel to the X-Y plane. I measured this by fixing a DTI "in space" above the table (attached to the column, head, or even an external mounting) with the tip resting on the table measuring in the Z direction. You then move the table in X and Y under the DTI tip -- the Z reading should stay the same -- the inclination of the X-Y plane makes no difference and thus this has nothing to do with column alignment. Mine remained virtually the same for all X but varied by 0.0015 in Y (higher at the front of the table than the back) for all locations (X) on the table. You CANNOT correct this condition by shimming the column -- you want the column (Z motion axis) perpendicular to the X-Y motion plane not perpendicular to the table if it happens to be a slight wedge like mine. The only way (I know) to proceed from here (without modifying the table) is to place a shim (0.0015) on the back edge of the table and rest the base of your square across the shim and the front edge of the table (the top surface of the base of the square will now pass the above test in Y and the vertical edge of the square is a good reference for alignment of the column axis in the front-to-back Z-Y plane). If the Y axis of your table is good, remove the shim when you rotate the square 90 degrees to align the column axis in the Z-X plane. You complete the alignment this way and when you finally sweep the table from the spindle you will see that it is 0.0015" lower on the back side. Everything you mount on the table will now need to be shimmed on the back to compensate for this KNOWN error in the table but your mill will be square. An alternative to the above is to "modify the table" by covering it with a mill plate. Here you check the top surface of the mill plate (as in the first step above) and shim it as necessary until it is "level". This then becomes your new table and is used for all subsequent alignment with no need for further correction. The disadvantages in this approach are that you need a near perfectly flat mill plate with good attachment points, you shorten the Z axis and you give up the subsequent use of the T-slots. In the alignments of my equipment, I find it helpful to frequently remind myself that I am aligning motion axes -- not surfaces. The surfaces are shimmed as necessary to get the X,Y & Z axes mutually perpendicular and to align the spindle axis relative to these axes (normally parallel to the z axis). All of these measurements ar dynamic ("sweeping") measurements (not simply placing a square between mill surfaces as used for rough alignment). On the Sherline there are no provisions for varying the alignment of X to Y and the table is assumed to lie in the X-Y plane (hense the above problem). ------- From: Ross Heitt Date: Tue Feb 22, 2000 12:42pm Subject: Flat Bottom Holes When a flat bottom is required I always drill the depth with an ordinary drill and then finish the bottom with another bit with the tip ground off flat. This is easy to do and works fine for me. :) Ross ------- From: tim deagan Date: Thu May 4, 2000 9:59am Subject: Re: Stiff X axis on mill (new clue) In sherlinex~xxegroups.com, "tim deagan" wrote: > Hello you helpful people ;-) > I was making my own t-bolts out of 1/4" machine screws (the kind with > the low dome head on top of the 4 square sides) by machining the head > flat and machining two sides down to the proper width. I was taking > pretty light cuts (.003") with the bolt held in the vise (by the lip > of the head so that the 'square' edge at the top of the screw was on > the top edge of the vise jaws. > Everything was going fine for 10 or 15 cuts when all of a sudden.. ! > WHAM! ..the mill grabs hard on the screw edge. The screw jumps out > of the vise, the vise shifts out of true, the entire mill jumps hard. > I turn the power off. I stand back. Impressed. Grateful the > spinning edge mill jumped _away_ from me. > > I assess the damage. Seemingly nothing is harmed. An ugly cut on > the screw, but that's a small price. I use a Starret Last Word to > indicate in the X-axis travel and it's as good as the day I bought > it. However, I notice that the X-axis wheel is very stiff while > moving the x-axis right to left. Not stiff at all moving left to > right. Only stiff on about the middle third of the right to left > travel. I clean, I lube. No change. > Last night I got brave and decided to tear down the X-axis to see > what I can see (hey, I bought the thing to learn :-) I clean out the > lead screw and nut, I fix up the backlash adjustment. I clean, I > lube. I put it all back together. I did not determine how to do > much of anything to the saddle nut. > The stiffness is better, but not gone. Still present only in one > direction of travel for a small section. Any ideas? Thanks, --Tim All, I spent a good deal of time last night with my dial indicators trying to determine if I had wonked up the travel, luckily I can't seem to find any problems. I tried a couple of different setups with my vise and rotation (not rotary) table. Then I started indicating with nothing setup on the table. The stiffness almost completely went away. Apparently the clamps on the vise or the t-nuts on the rotation table are causing the stiffness. I had thought I was being careful not to overtighten, but perhaps I am bearing down too much. Anything less than what I have been doing barely seems adequate to keep parts in place during milling. Not that I have a torque hex wrench, but any ideas about what appropriate torque would be? I could set up a standard torque wrench setup and practice till I have the feel down. I suspect that climb milling may well be the source of my grief. I get a little confused on figuring out whether I'm doing climb or conventional milling when face milling (in my ignorance it seems like I must be doing both.) It's much easier to determine when edge milling. As a novice with no access to anyone with any experience (best I can do around here is find someone who can kinda recognize a drill press 'cause their Dad had one :-( I am incredibly grateful for this forum and the help I have received. Tim ------- From: Marcus & Eva Date: Thu May 4, 2000 1:21pm Subject: Re: Re: Stiff X axis on mill (new clue) Something is not right! You should be able to snug a flat part or a flat vise down pretty good on the Sherline table. The stiff spot may be a hump in the table; check it for flatness with a straight rule and blueing, or on a surface plate. Check the leadscrew by rotating it in a vee block with an indicator. Check the vise for flatness with a rule and blueing as you did with the table. ------- From: Marcus & Eva Date: Fri May 5, 2000 11:31pm Subject: Re: Thanks for suggestions(Drilling small holes in cop per clad board) Don't do it Dave. Get yourself a couple of circuit board drills; they are solid carbide with a 1/8" dia shank and can be held easily in a 1/8 collet. Run them as fast as the mill will go. They cost about $10.00 CDN apiece from KBC (at least that was their price last time I bought some.) They are stiffer than High speed drills. If you still have a wandering problem, make up a spotting point from a 1/8 bit of high speed steel. Grind on 3 flats at 120 degrees to get a triangular point. Make the included angle about 60 degrees. To get the point dead nuts in the center, whip the lathe headstock off the lathe and mount it on the mill table at a 30 degree angle. Get a mounted grinding point (Dremel is ok) and chuck it in the mill spindle. Rough out the point freehand on the bench grinder, and then chuck it in the lathe headstock. You can eyeball the 120 degree increment using the chuck jaws; you don't care about the accuracy of this indexing anyway. All you want is the point in the center. Touch up the point with the grinding wheel , and you're in business. Good luck Dave Marcus. ------- From: "Rich D." Date: Thu Jul 27, 2000 7:16 pm Subject: Re: [sherline] End mill instead of fly cutter? > Hello, I'm new to the group and to machining. I did not buy the fly > cutter and now need to square a piece of steel. Is it OK to use an end > mill? Would the surface look as good as if it was done with a fly > cutter? Thanks! Rogerio Rogerio, Endmills will do fine. If you use the 'end' rather than the side, try to use one that is bigger in diameter than the stock. The results will be the same assuming the edges are sharp.Be safe. Rich D. ------- From: "Flosi Gudmundsson" Date: Thu Jul 27, 2000 7:39 pm Subject: Re: End mill instead of fly cutter? >>From: "Keith Yundt" Date: Fri Jan 21, 2000 1:04 pm Subject: [sherline] Tool making tip Happy New Year! I thought I would share an idea I had while making myself a flycutter for my lathe: Rather than have to make a #1 morse taper, I use the #1 morse taper adaptor that came with my 3/8" drill chuck. That way I didn't need to make the taper, and I already had the drawbar too. So I made the flycutter (which looks like the Sherline version holding a 1/4" bit) and thread the morse taper adaptor into it. The best part about it was that once the flycutter part was drilled and tapped, the piece could be threaded onto the adaptor and put in the lathe, making sure it would turn out true and also made it easy to machine. A future benefit is that I can make other pieces to thread onto the adaptor in a similar way such as a gear cutter arbor, end mill holder etc. Anyway, you get the idea, hope it helps someone! Keith. << You can easily make your own flycutter as Keith Yundt described in Sherline message no. 995. I did and it works great. I also made a circular saw arbour. One of the grat things about lathe and mill is that they can be used to make other tools. Flosi ------- From: "Rich D." Date: Thu Jul 27, 2000 7:43 pm Subject: Re: [sherline] Re: End mill instead of fly cutter? Rogerio, "try it any way". Yes. Draw file it if you want a better finish. OK,OK! WHAT'S A DRAWFILE! Hold a flat file in both hands like it was a stick with both thumbs pointing together, sorta. Pull or push the flat file surface (file at right angles to the work) against the work. Use oil for best finish. Harder to describe than do. Gives a straight brush finish depending on the file's finish grade. Always use a single cut file, smooth or smooth bastard. Alternatively, tape a sheet of 'emery' paper to a hard, flat surface and stroke the metal on that. Back to my widgit maker. Rich D. ------- From: wanliker... Date: Fri Jul 28, 2000 12:50 am Subject: Re: [sherline] End mill instead of fly cutter? << Would the surface look as good as if it was done with a fly cutter?>> No, there will be a series of swirls across the plate where you make each pass with the mill, the flycutter will leave a series of grooves where it cuts, With either the mill head needs to be accurately trammed with the table or the surface will be concave. If the job will permit it, use either, then sand the surface on a flat plate. Make your own flycutter, it is a good project to learn on. bill ------- From: Ron Ginger Date: Fri Jul 28, 2000 8:27 am Subject: Re: [sherline] Re: End mill instead of fly cutter? videos... wrote: > The stock is 1/2" and the biggest end mill I have is 3/8", it will > take 2 passes, should I try it any way? Sure, this is very often done. Even with a fly cutter some work is so wide that one pass doesn't cover it. Take a look at any of Rudy Kouhoupt's articles in HOME SHOP MACHINIST, he almost makes a 'trademark' on his projects of the mill passes. He does them very neatly, and very uniform and the projects have a nice look -- almost like 'engine turning' on old work. I asked him about that finish and he very consciously figures out the pattern across each part so the mill lines come out uniformly spaced. He does not sand the finished surface. You must of course have the machine lined up very well or else the mill marks will be grooves and that is bad. ron ------- From: Marshall Pharoah Date: Tue Aug 1, 2000 10:52am Subject: Re: How do I machine a radius? Rich, you can make a short post which will fit in the t-slot of the table on your mill and fit through the hole of your stock. By holding your stock with your hands, you can manually revolve it into the cutter to create the radius. Take real light cuts, and maybe even make an adjustable clutch with flat/lock washers. Scribe it and use a hacksaw and file to get it close first. You can get a little more control by making a longer handle. This is something I've done on a larger mill. The key is to take real light cuts so that you maintain control of the piece and don't let the cutter grab it. You could always make a simple rotary table if you're going to do a lot of this, but for a few, you can feed it by hand. Marshall ------- From: Ron Ginger Date: Thu Aug 24, 2000 4:16pm Subject: Re: My 1/4" collet and end mill are stuck in the headstock! I think your only choice is to hit it harder! Make sure the headstock is supported so the force goes completely into the collet- I would unmount the headstock and place it on a firm benchtop in a way that when you hit the drawbar you are driving the whole headstock into the bench, that should put all the force on the collet. Hitting it while mounted on the mill column will mostly shake the column I would use the drawbar, not a brass rod to do the hitting. Be sure the drawbar is well screwed into the collet so you load as many threads as possible- if its only a turn or two in you will likely ruin the thread in the collet, the drawbard or both. Using a rod, even brass, will place all the load on the top thread, possibly ruining the collet. I assume there is a mill in the collet. Maybe a thin rod, through the collet, to hit the top of just the mill will push the mill out. Since its a 1/4" collect this would require a rod slightly under 1/4", and the length of a drawbar. Thats going to be so long and skinny it likely will just bow, but maybe worth a try. There was a discussion here a few weeks ago about how hard to tighten the drawbar. You have shown it's possible to make it too tight! ron ------- From: Dave Martindale Date: Thu Aug 24, 2000 4:48pm Subject: Re: My 1/4" collet and end mill are stuck in the headstock! If you're going to hit the drawbar (or a rod that replaces the drawbar) very hard, it would be a good idea to support the headstock so that the *spindle* end takes the force, not the headstock base. If the base is what takes the load, the impact is transmitted from the spindle to the base through the headstock bearings, and enough impact will damage the bearings. Another thought: use something like a large C-clamp or woodworker's pipe clamp to provide pressure without impact. The headstock bearings should take a lot of steady pressure (without impact) before being damaged. Dave ------- From: Bill Miller Date: Thu Aug 24, 2000 8:14pm Subject: Re: My 1/4" collet and end mill are stuck in the headstock! Dan, I just did the same thing yesterday with my fly cutter. Fortunately, I have a brass rod that I use for squib rounds in my pistols that just fits through the spindle ID. Two good taps with a hammer had it out. I think the draw bolt was flexing too much and absorbing the impact on it. Bill ------- From: Charlie Lear Date: Thu Aug 24, 2000 8:34pm Subject: Re: My 1/4" collet and end mill are stuck in the headstock! On Thu, 24 Aug 2000, Dan Gustafson wrote: >> Great. I managed to have gotten my 1/4" collet and end mill stuck in the headstock of my mill. I tried cooling the entire thing in my freezer hoping the metal would change size enough for me to tap it out but I still cannot get it out. I have tapped good and hard on the big long screw that pulls the collet into the taper but it aint movin. What do you guys do in this situation? Is there any way to prevent this from happening? Happens to the best of us, more often than people care to admit! As you have seen, on shallow tapers there isn't a big difference between not quite tight enough and too tight. On my bigger lathes (3MT and 6MT) it is easy to slide a heavy bar up the spindle hole and cleanly knock it out without much drama. On a Sherline, you aren't going to get much mass in a 3/8" bar, so the method doesn't apply. DO NOT hit the end of the drawbolt with anything metal or heavy. (You won't damage the drawbolt or collet threads unless you're way too angry or have the drawbolt way too slack.) You'll get away with it a few times but sooner or later you will damage the headstock bearings. The same applies for poking a bar of anything down the spindle and whacking the end of the bar. What needs to be done is to support the nose of the spindle, while applying force to the end of the drawbolt. What I do - and this is by no means the only way of doing it, or a "correct" way of doing it - is to get a 2" piece of 3/4" OD steel tube, slip it over the milling cutter and collet, and butt it up against the spindle. My offcut is small enough to not interfere with the spindle threads. Slacken off the drawbolt by 1/8", put the solid end of an 8" G-clamp against the tube, and tighten the clamp screw against the end of the drawbolt. A couple of turns and she'll pop out with no drama at all, and no stress on the headstock. I've only used this method with collets, as I haven't (yet) got a flycutter or boring head jammed up the spout. When I do, I'll have to figure a way of applying force to the end of the spindle past the tool. Probably a piece of aluminium plate shaped like a C and butting up against the flat part of the spindle register will do the trick. In ordinary use (eg 99% of the time, when I haven't been too heavy-handed in the screwing-it-up-tight department) I just slacken the drawbolt two turns and tap the end with a plastic-faced hammer. For the next question: how do you stop the mill spindle from turning when you have a spanner on the end of the drawbolt? 8-) Hope this helps, Charlie ------- From: Ron Ginger Date: Fri Aug 25, 2000 9:25am Subject: Tramming the head (tutorial) "Rich D." wrote: > Bill, > The spindle is not at 90 degrees to the table. Fix a dti in the > spindle and sweep the table/make adjustments. I think this is a topic that could use some more explanation for the new guys. This operation is called 'tramming the head' and is required on all vertical milling machines, even the biggest of them. Sherline is no exception if you are looking for the most accurate work. The idea is to be sure the spindle axis is exactly perpendicular to the table. It can be off for several reasons. 1) the mount of the headstock is designed to swivel. In the lathe position this is used to trun tapers, in the mill position it really is not a usefull adjustment. A key is fitted to the head to hold it in a straight position, but its likely this is not 'perfect' 2) the vertical column is bolted to a mounting block with 4 screws. There is no pin to align this, so its possible it can be slightly off. If you have the optional swivel plate here it can be way off. 3) The base block that mounts the column to the base could be milled slightly off, or could have a chip under it that makes the head lean off 'true north' So, there are several places that can cause the head to lean. You determine the lean by putting a DTI into the spindle at an angle then use it to sweep as large a circle on the table as possible. If the head is perfectly vertical the reading will be the same for the entire sweep. If there is error it will show as the indicator being 'long' on one side and 'short' on the opposite side. Your job is to 'simply' adjust something until the reading is the same all the way around the circle. Easier said than done, if you want it real close. If the reading shows a lean to the left or right the headstock mounting can be swiveled, just as for turning taper. I read somewhere about a fine adjustment block for this that would also be a great addition in lathe mode. Essentially a plate with 2 tapped holes arranged to push on either end of the headstock body to make fine adjustments. If the column is leaning forward or aft the only adjustment is to shim or file under the base block. Anytime I want to make very accurate parts I do a quick sweep of the head first. It does not take a big hit to knock it off true. ron ------- From: Marshall Pharoah Date: Fri Aug 25, 2000 10:03am Subject: Re: Tramming the head (tutorial) Very good. You can also shim between the vertical column and the base block. This might actually be a good spot for a permanent fine adjustment? Marshall ------- From: Date: Fri Aug 25, 2000 10:56am Subject: Re: Tramming the head (tutorial) Make sure that the front to back table error is caused by the column and not the table before you go too far. With an indicator touching the table surface, run the table forward and back. On my 5400 mill, this showed a difference of about 1 thou. With a mill tooling plate in place, I got the same results. I chose to mount the tooling plate with a shim under one edge to correct this. Final tramming of the head then required only getting the headstock parrellel to the vertical axis in the left to right directions. This required TWO checks. First, make sure the column is truly vertical to the table by mounting an indicator in the spindle and without turning the spindle run the headstock up and down while indicating on a known good square resting on the table. Adjust by loosening slightly the four mounting screws and tapping into alignment. After the column is truly vertical, adjust the headstock angle (the one used for taper turning on the lathe) using the tradition sweep method. -Brian ------- From: Rich D. Date: Sun Sep 10, 2000 11:33am Subject: Re: cutting t-slots for a new sherline milling table Jason Spangle wrote: > Hello Everyone, I'm making a tooling plate for my sherline 2000 mill. I've purchased some 3/4" thick 4-1/2" wide 6065 aluminum, and once I have the length cut down, I'll have a slightly larger/longer table. I'll be using some old mill that's big enough to handle fly-cutting this piece, I'm waiting on the fly-cutting until I have all holes drilled. But then I thought about putting two or three T-slots down the length. Now how do I go about machining T-slots? Is the size measured on the smaller cut or larger (bottom) cut? Do I first run an end-mill down the length so that the T-slot cutter will have room to throw chips out? I think I'll have enough room to have three slots machined (to standard Sherline spacing of each) and then I'll fly-cut both sides since I'm sure there will be a slight warping from heat right? thanks everyone, Jason < Jason, cutting T slots is a two step process. The vertical slot is done first with an end mill or a radial cutter in a horiz miller and then a T-slot cutter is run down the center of the slot to cut the head of the T. The 'Size' is usually given as the T bolt shank diameter, so the slot may be wider. The Sherline T slot is a small special size. A cutter will have to be made from drill rod or you could step up to the smallest commercial size: for 1/4" bolts. Fly cutting your alum. slab may warp, but only because you cut away stressed material on one side. I understand that Sherline will not supply a longer table because of this. Rich D. ------- From: Kevin P. Martin Date: Mon Sep 11, 2000 10:53am Subject: RE: cutting t-slots for a new sherline milling table The Sherline T slot is a small special size. A cutter will have to be made from drill rod or you could step up to the smallest commercial size for 1/4" bolts. I seem to recall that I found a "keyseat cutter" that, although not identical to the Sherline T-slot size, would be able to cut an acceptable T-slot once the main slot had been milled out. The only problem is that it has a 1/2" shank (whice necks down near the cutter). I was planning on buying another 3/8" end-mill holder and boring the hole out to 1/2" but I never got around to it, and still haven't used the cutter! Kevin Martin ------- From: Date: Sun Sep 24, 2000 1:38am Subject: Lathe ops on a mill Is it possible to do lathe operations on a mill? I currently own a Sherline mill, and was thinking about doing lathe operations by holding stock in the spindle and the tool in the mill vise. I know finding centre would be a pain, but is it possible? Keith ------- From: Marcus & Eva Date: Sun Sep 24, 2000 9:39am Subject: Re: Lathe ops on a mill Hi Keith: Sure it is!! I've done it often, when I've had a setup in the lathe that I didn't want to disturb, and just needed a quick cut on something else. I've also done CNC turning on a Sherline mill equipped with Flashcut and the horizontal milling base. Worked like a charm on a bunch of plastic parts that I had to make. The only thing that you can't do easily, is tailstock operations. Cheers Marcus ------- From: Date: Mon Sep 25, 2000 8:30pm Subject: Re: Lathe ops on a mill Okay, now that I know it can be done, do the four jaw and three jaw chucks mount up to the mill's spindle? Thanks for the replies, it is greatly appreciated. I'm really glad I found this e-group. Now I can share my hobby with others that actually share the same interest. Keith ------- Date: Fri, 5 Jan 2001 18:41:52 -0800 From: "Yasmiin Davis" Subject: RE: Advice for novice >> I've got some ground stainless steel shaft 1/4" diameter by 6" long. I need to drill a 1/16" hole through it for a dowel pin, thread the end of the rod about 3/4" (1/4-20) and cut 2" off the other end (I need 4" shafts and this came in 6" increments from the Small Parts catalog). Anyway, I've got the Sherline lathe & mill, carbide/TiN drills, and a standard bench grinder, cutoff saw and drill press. So far I've only worked with aluminum, so if there's any advice people on this list would care to throw my way before I hurt myself I'd appreciate it ;-] Thanks in advance, Eric Solberg << You need to make a jig. Take a piece of whatever and mill a 45 degree V ( 90 degrees total) into it about 3/4 of an inch deep. Then drill a 1/16 hole into the bottom of the V and out the other side. Then clamp you rod to the V with the flat side of the jig on top and perpendicular to the plane of the drill. Center punch the rod through the 1/16 hole with a 1/16 transfer punch. Then drill the hole going slowly till the hole in the rod is well started. If you really want to get fancy you could make a drill bushing and drill a bigger hole into the bottom of the V. Then make a drill bushing that will reach down and touch the rod. This will cause the drill to have less of a tendency to wander. There are ways of sharpening a drill that will tend to prevent this but that's really going a bit over the top for a 1/16 th drill. I am sure you will get some other methods that will work as well or better than mine but then that how we all learn. Yasmiin ------- Date: Sat, 06 Jan 2001 03:50:13 -0000 From: "Flosi Gudmundsson" Subject: Re: Advice for novice The simplest way of drilling a hole on cener of a round stock is to mill as small a flat on it as possible and then use eyesight to senter a center drill over it. After some practice this is rather eazy. A general advise regarding machining is to use sharp HSS tools, good cutting fluid and don't get tangled in the steel wool while it is forming. It can easyly cut off fingers. SS is probably not the easiest stuff to machine, but I know nothing that gives better finish. Flosi ------- Date: Wed, 10 Jan 2001 02:55:35 -0000 From: "Robin " Subject: Turning on mill... No, not powering up a mill, but rather using a mill as a lathe :) Tonight I decided to prepare a blank arbor for reaming on a lathe to produce an endmill arbor. I don't own a Taig lathe, and all my blank arbors (ordered from Taig) had about +/- 0.002" run out. Obviously, I would be unable to place the arbor in a collet or chunk of another lathe and drill/ream it as the endmill would then have the same runout, which would be unacceptable. To obtain a true OD, I placed a lathe tool bit in my milling vise, and screwed the blank arbor onto the mill head. I then turned on the mill and very slowly cut the OD of the arbor with the lathe tool using the Z feed. I took off about 0.002" at a time until there was nothing left of the original OD. Now the OD of the arbor has a runout of +/- 0.0005". Just thought someone might want to know :) Regards, Robin ------- Date: Wed, 10 Jan 2001 19:31:44 -0000 From: "Eric " Subject: How do you use a "center finder"? I recently purchased a Starrett center finder, which is basically an edge finder with a pointed end rather than the standard straight end. I am familiar with how to use the edge finder by bringing it to the edge of the workpiece with the spindle running and waiting for the abrupt "jog" to indicate your position. How does the center finder work? I can't find any information on it. Thanks, Eric ------- Date: Wed, 10 Jan 2001 15:08:07 -0500 From: Stan Zdonick Subject: Re: How do you use a "center finder"? At 07:31 PM 1/10/01 +0000, you wrote: >How does the center finder work? I can't find any information on it. Chuck the workpiece in the lathe with the center marked, usually by a punch. Roughly center the piece in the 4 jaw with the center finder near the mark. When you feel you're really close, insert the point of the center finder in the punched mark. Rotate the chuck slowly and the center finder will greatly exaggerate the error. Adjust the jaws until the center finder will no longer deflect when the chuck is rotated. Simple, fast, accurate. I'm sure there are pictures of this operation somewhere on the net. -------- Date: Tue, 30 Jan 2001 12:13:40 -0800 From: "Craig Libuse" Subject: Re: Sherline Mill Labled Wrong? >>"any opinions? Do I need to relable the Y-Axis, let sherline know, or >>am I looking at this wrong?? thanks! tauseef" Dear Tauseef, The Sherline mill handwheels are labeled in the same traditional manner as a Bridgeport or any other mill. It's not that the numbering system is "wrong" so much as that it doesn't really work in terms of a Cartesian coordinate system unless you think of upper left hand corner of the table as the 0,0 point. That way, all your X dimensions are positive and all your Y dimensions are negative. Cranking either handwheel clockwise makes the positive X numbers get larger and the negative Y numbers get larger, which is correct. If you placed the 0,0 point in the lower right corner, both of the handwheels could be considered "wrong". Placing 0,0 in the center of the table as you had it makes one handwheel right and one wrong. I am told this is referred to as the "machine coordinate system". I hope this reduces confusion rather than adds to it. Craig Libuse, Sherline Products ------- Date: Wed, 31 Jan 2001 23:37:28 -0000 From: ballendox~xxyahoo.com Subject: re: re:Re: Sherline Mill Labled Wrong? Craig, again, there is NOTHING WRONG with the HANDWHEELS! The Y axis engraving (on the machine base) is wrong! Homing location has nothing to do with this! It IS true that most machining centers (vertical, like the s/l mill) home to the most positive axis location. This means the coordinates used will be ALL negative (until reset by program or operator). This is quadrant 3 of the cartesian coordinate system. Ballendo P.S. (snips/inserts below) >>"The next generation of machinists is in our classrooms now. MANY >>are using Sherline equipment. Shall we train them in >>an 'outdated' "machine coordinate" setup, or prepare them for the >>REAL world? Suggesting that the origin be placed in the upper left >>corner is WIERD!" >but notes that you should be aware that not all machine >use the same location on the machine tool for the home position. The >example he illustrates shows a system where the upper right corner >of the table is zero and all X and Y points have negative values for >programming purposes. There are 8 possible (normal) Home positions; the 4 corners of travel with z high, and the 4 corners of travel with Z low. Industry standard is z moving upward is positive, downward is negative. Because of this, virtually ALL vertical mills and machining centers home z to the top of travel. This eliminates four (of the possible eight) home locations. The remaining 4 home positions WILL affect the 'signs'(plus or minus) of the coordinates used, BUT travel direction and orientation WILL NOT be changed! the 4 possibles: home coords LL = +X,+Y (common for CAD, engravers, routers) UR = -X,-Y (common for vert. mills and VMC's) UL = +X,-Y (not commonly used by machinists) LR = -X,+Y (not commonly used by machinists) The one additional sometimes used home position/program zero is CENTER of travel. This just means that the coords will be pos or neg depending on which direction you go on the part/table. It DOESN'T change the Labelling of the axis travel directions... >but it does show that the coordinate system for programming can be >somewhat flexible. Flexible, yes. But not willy-nilly... >It is in our best interest to follow whatever is the industry >standard. >Craig Libuse Sherline Products Yes! And that's why I've spent so much time on this thread... ------- Date: Fri, 02 Feb 2001 13:02:36 -0000 From: ballendox~xxyahoo.com Subject: RE: New Member Paul, since you are cutting wood, consider adding a dremel mount to the mill (in place of the spindle). The higher speed should give you great results. Of course, if you're using exotics like boxwood, cocobolo, ebony, etc. or fine grained stuff like pear, apple, holly, etc. you may have fine results with the slow speed(for wood) of the stock spindle. The suggestion for a "backup" gear is a good one (or use a 'stack' of gears). Masonite (tempered hardboard) is cheap and works well. I posted an ascii drawing of a dremel mount to Alan M awhile back. maybe he can re-post it. A nice, easy project, it alows some things to be done which are difficult with a stock spindle. Fine woodworking magazine had an article on wooden clocks some time back which detailed a number of ways to cut gears. Also things to use instead of 'involute style' gears. Many wooden gear trains use a lantern pinion and a different tooth style than metal gears. Do keep in mind wood movement! Your 'round' gears may turn oval and bind. Sometimes you can play with this and make the 'ovals' work together. I've even seen elliptical gears... There is a shareware gear cutting program available on the web. try a search. It's a UK listing. Hope this helps. Ballendo ------- Date: Fri, 02 Feb 2001 21:27:17 -0500 From: ron ginger Subject: Re: power feed for mill? Chuck & Joanne Johnston wrote: > Does anyone have details on a power feed attachment for a mill ? > Would like to add a power feed for smoother cutting on both axis on the > mill. Any ideas or tips ? > I don't like to spend the 400+ bucks that it takes for the CNC setup. Buy a battery operated electric screwdriver. Insert a hex nead socket screw in the center of each handwheel, and lock it with locktite. Put the right size allen driver in the screwdriver, and poke it into the center of which ever handwheel you want to power. Most of then have forward/reverse and some range of speed settings. Might be helpfull to grind some relief into the end of the allen driver, like those "ball drive' hex sets so alignment is not critical. ron ginger ------- Date: Mon, 5 Feb 2001 01:21:35 -0800 From: "Eric Solberg" Subject: Achieving good finish on mill I'm having trouble getting a good finish milling 6061 aluminum. (1/2" thick rectangular bar stock) I'm using 3/8" HSS end mills (from Sherline) running at 2000 RPM and depending on the direction I cut will either end up with a rough finish or a shinier finish but with lots of bumps from the climb-cutting. Either way I end up with a lot of filing and sanding, but on the parts I'm making this is difficult. Any advice for getting the finish better the first time? If there's a particular type of end mill that will make all the difference then I don't mind spending some money on it. I have the MSC catalog but don't know the parameters to look for to get a better finish. Thanks, Eric Solberg ------- Date: Mon, 05 Feb 2001 10:41:15 -0000 From: ballendox~xxyahoo.com Subject: Re: Achieving good finish on mill Eric, first be sure the gibs are adjusted correctly. Climb milling stresses a machine more than conventional cutting. Then check to see if you have minimised leadscrew backlash(at the nut AND the handwheel). Next be sure all machine adjustments are tight (spindle/head setscrew, etc). Be sure to LOCK any "unused" axis! Are you cutting 1/2 width of the endmill (3/16 wide passes)? Are you too deep (each pass)? means have you tried other width/depth combinations to see if one works better. NOW, AFTER you have checked all of the above, think about changing the cutter. Are you using 2 flute and lubrication? Wd-40 works well with 6061. Speaking of this, are you sure it is 6061? Some aluminums are terrible to machine. The sherline mills are good tools and capable of finishes needing no additional work. If the suggestions above don't fix the problem, try to talk to someone in your area who may be able to 'see' something we can't get from an email. Hope this helps. Ballendo ------- Subject: Re: pc bds w/ sherline Date: Sat, 14 Oct 2000 07:09:30 -0000 From: ballendox~xxyahoo.com To: KM6VVx~xxarrl.net Alan, I know you didn't ask, But Since it looks like you'll be milling pc bds soon... :-) Try making a Dremel adapter to fit the sherline mill. The speed will VASTLY increase the quality of your results. I'm including an ascii art example: made from alum plate. And a couple of cap screws. Mat'ls. Cast alum is better but wrought plate will be ok. 6061 typ. 1ea.-2.75w x 3.00l, 1.00 th. to 1.25 th. alum. 1ea.-2.75w x 3.00l, .500t alum. 2ea.-10-32 x 1 SHCS Note: The old dremels have a 3/4-16 thread on the nose. the new ones use 3/4-12. Tap is about $12 from msc, travers, enco, or the like. You COULD mill the thread with your CNC! But the cutter will cost about the same, or more. :-( The sherline head mount pin is .500dia. and 1.188 or so long. So if you use 1.00 thick alum you will need to screw the dremel into the mount before mounting it to the mill.(so you can turn the dremel) Not shown on the drawing is the hole for the setscrew which holds this thing to the mill. Use the sherline orig. head to get the dims. for this. This is a basic version. If you'rew going to do a lot of boards, you will want to redesign to have the dremel "float" vertically and use a nosepiece to control the depth of the engraving into the pcb. |--1.00+ --| __________ | | | | ___ bore .500 for sherline mount pin | | / | | / |----------|/ __|____ _ ___|____ | | |----------| | | | - | ____ Tap 3/4-XX for Dremel | | | |---1.125-----| / (see note above) | | | | min. | / |_____|_|__|_____________|_/_______ ___ | | | < | > | | |_| < | > | .500 |____|___|__________<____|____>____| ___ | | With this setup mounted on the Z axis, I use a .500 cast alum(so it stays flat) "table" (mounted to the sherline mill table w/ spacers so it clears the motors/handwheels) to give me something flat to mount the pc bd mat'l to. I use 1/8 tempered masonite(smooth both sides) as a "backup" material under the board. Think and tinker (on the web) sells bits, board mat'l and thr "real" backup stuff. Good luck. Hope this helps. Ballendo ------- Date: Tue, 06 Feb 2001 15:35:06 -0000 From: gavin.Eyrex~xxrsl.com Subject: Large Radius Cuts I am trying to make some small webbed parts that have edges curved at a radius of about 48". The parts themsleves (train connecting rods) are only about 2" long. I can get the curves on the outsides by hand filing - but to get curves on the pocket really needs me to be able to move the piece under the cutter so that I cut a small portion of a large radius. I have thought about doing small stepped cuts - ie move .030 on X and then .001 on Y then .025 on X and .001 on Y but wondered if there was a better way. Thanks Gavin Eyre ------- Date: Tue, 06 Feb 2001 11:54:55 -0500 From: "Rich D." Subject: Re: Large Radius Cuts Gavin, I have made contours by hand coordinate stepping. But to minimize the stair stepping look the number of steps has to be enormous. This is a job for CNC, for sure. A 48" radius is very large and .001" steps may be too much. I'm setting up a CNC Sherline 5400 now for this type of work. Rich D. ------- Date: Tue, 06 Feb 2001 18:29:45 -0000 From: n2562001x~xxyahoo.com Subject: Re: Large Radius Cuts Gavin: A 48" radius over a 2" span will almost be a straight line. I think you will need to scale your radius for the item to look right if I understand your project. If you scale the radius it will probably be managable using a rotary table. If need be you can bolt a plate that is well beyond the edge of the rotary table to get the radius you need. Jerry Kieffer ------- Date: Tue, 06 Feb 2001 11:18:19 -0800 From: Alan Marconett KM6VV Subject: Re: Large Radius Cuts Hi Gavin, I'd have to see the drawing, but I think you might want to do something like that on a rotary table. OR, mount the part on a pin through the center of the radius, and move the part by hand through the arcs you want to cut. The third way would be to use CNC! The radius is 48"? .48"?? More on the rotary table approach. You could use a large timing belt pulley, mount it on a short shaft and bearing that can be bolted to the ways, and use a single tooth to lock the table at various angles. bolt your part on the big pulley. Then mill holes along your arcs. Connect the holes, you've got your arcs. Driving it with a belt and a small pulley on a handwheel MIGHT give you enough control of the table to make continuous cuts. This makes what might be considered to be an inexpensive indexing head (or rotary table, with the belt drive). Enough teeth on the big gear, and you have quite a few "locked" angles to work from. Calibrate the small pulley, and you've got even more! Hope this gives you some ideas. Post the drawing, we might come up with a few more! Alan KM6VV ------- Date: Tue, 06 Feb 2001 19:19:56 -0500 From: Jim Ash Subject: Re: Large Radius Cuts Granted the Sherline is kinda small for it, but don't overlook lathe filing. In one of Guy Lautard's books, he describes a stepping method, followed by filing to smooth out the steps. His trick is to calculate the steps accurately, blue the work after stepping, then file until the blue is gone. There' no reason it shouldn't work for you on the Sherline. Jim Ash ------- Date: Wed, 07 Feb 2001 00:45:48 -0000 From: ballendox~xxyahoo.com Subject: re:Re: Large Radius Cuts Gavin, I agree with Jerry that you may want to 'scale' the radius. Much of the 'art' of modelmaking is knowing when to depart from "strict scale" measurements! If you have already taken this into consideration (or don't have a rotary table), here's a way: Turn the y axis of your mill into a "tracer" configuration, like a taper attachment on a large lathe... Then you can use one of your "outside filed" curves to cut the inside pocket curve(s). I think I described this in an archived message, but here goes. To do this, remove the y leadscrew from the machine. Using the 'disk' that the leadscrew went through(1/4 hole) fasten a "pointer" which will be a block of metal with a tapped hole for the holding screw, and a vee-shape which 'points' towards the mill table. _______ /\ | | / \ |_______| | || | | || | |_||_| |_||____| ________ | | The "O" is a threaded hole for a screw | O | which passes through the leadscrew hole |________| in the 'disk' that the handwheel rides against. Now fasten a "hand filed template" using the front t-slot (on the mill table) This will be a flat piece of sheet metal, or flat stock, which has 2 holes for mounting "off the front" of the mill table. The shape to be 'traced' should be machined (filed, in our CURRENT case; it could be a "wavy" shape, or a taper, etc.) in the edge 'facing' the pointer. Now you can see that if the mill table is "gripped" in your left hand (fingers around the back of the table, thumb on the front of the mill base), you can 'pull' the template (with table) into contact with the 'pointer' you mounted in the disk (which formerly held the leadscrew). If you use your right hand to screw the x axis handwheel, you will see that the table is "following" the template curve! Mount your work in the appropriate position on the mill table and "you've got it!" Hope this helps. Ballendo P.S. This might be a nice "aftermarket" accessory for sherline to offer. They could replace the left hand "spring" with a REAL spring or tension device. I see something adjustable, possibly "screwed into" the column support block. You could do this also, if the idea of your hand in the "cutting" area bothers you. IMO, the forces involved make for a safe operation if care is observed... P.P.S. You can also "work this out" using the "stop" screw in the machine base to hold the pointer (which is now MADE FROM a piece of angle). Position the table with the handwheel so the table is near (a little forward of) the proper position for cutting, THEN remove the handwheel. You can fine tune the leadscrew projection (if it is getting in the way) without the handwheel attached. You "may not have to" remove the leadscrew. It will depend on the size of the part, and the shape. One advantage to this position is that your hand will be "farther away from the action". It is not difficult to remove and replace the leadscrew, and going that route will give more versatility to the operation. ------- Date: Wed, 07 Feb 2001 07:57:05 -0000 From: videosx~xxmail.giga.com Subject: Re: Large Radius Cuts I don't understand your part completely so maybe this is not what you need. The best and most precise way of obtaining long radiuses is by the method astronomical telescope mirror grinders use. You start with 2 glass or metal discs of the same size, add abrasive powder in between and rock the top disk forward and back, overhanging the edges by about 1/3 diameter. The top disk gets concave and the bottom one gets convex. This can be done with rectangular shapes also. You can get a 48" radius in an 8" pyrex disk in about 1 hour with 60 grit abrasive, then use finer abrasives to get a better surface. If you overshoot your radius just put the top part in the bottom and the bottom part in the top and grind a bit to return to your desired radius. This is better explained in a telescope mirror grinding book or do a search in the net, I recall there where several places that explained this. Hope this helps. Rogerio Odriozola ------- Date: Thu, 8 Feb 2001 14:30:09 -0500 From: "Dan Statman" Subject: Re: Re: learning manual [MILLING] Actually, All of my rings are done by hand. I don't even have a rotary table, hell I don't even have a mill, just the milling column for the lathe. I use a vise, and my dial caliper and a scribe to mark of the rotational angles around the perimeter of the ring using a little trigonometry and the outside diameter of the ring. All of my curved surfaces (except the inside and outside diameter curves) are ALL filed by hand. It takes me a very long time to make certain styles of rings. There are however, some designs which I cannot make on my current equipment without converting them to CNC. I just don't make those designs, I am sure somewhere there is a non-CNC machine costing many thousands of dollars that could maybe be made to cut the designs I want, but it sure as hell would be easier, cheaper, and quicker with a miniature CNC mill and rotary table. I still wouldn't bother cutting a domed profile ring with a CNC as I can do it MUCH quicker with a hand file. Daniel J. Statman, Statman Designs http://members.rennlist.com/statmandesigns -------- Date: Sat, 10 Feb 2001 12:34:19 -0500 From: "Bill Rutiser" Subject: Re: Chips > Question: How are you folks protecting the dovetails, etc.? I know that some of the larger mills have covers over their dovetails to keep the chips away. -- Jerry Jankura < Jerry, I usually attach an improvised cover with masking tape. For vice setups, I have a piece of material from a heavy Ziploc Brand plastic freezer bag. At the bottom, its taped to the back of the mill table. At the top its taped to saddle behind the spindle. This does a good job of keeping chips from the back part of the Y axis dovetails. I have also used two pieces of cardboard. One was taped to the table and the other suspended behind the spinple by a piece of wire. The upper cardboard hangs in front of the lower piece. This works well for long X moves but the cardboard must be matched to each range of vertical positions. Bill Rutiser Gaithersburg, MD, USA ------- Date: Wed, 14 Feb 2001 23:09:54 -0600 From: "Jeffrey C. Dege" Subject: Need some help... I'm playing with my new Taig lathe, building a simple little wiggler steam engine (one of Patrick Verner's plans, from www.steamengines.org - and btw, does anybody know what happened to his site?) The body of the engine is L-shaped - and I'm wondering how to deal with finishing the inside edges of the L. Yes, I suppose that since these are non-bearing parts I could just grind them flat and polish them up, but I'm doing this to try different things with the Taig. Fly-cutting the surface, of course, won't work, because the other part of the L will get in the way. Same problem with an end-mill. But looking at things, if I had a milling cutter that would cut with its side, I'd be able to reach the areas I need. I've got (as may be obvious) the Taig milling attachment and vise, and the 1/8" end-mill, but measuring the width with my calipers show me that the width is not consistent, it has a definite taper. So it is clearly not intended to cut on its side. So next I go looking through the MSC online catalog trying to figure out what milling cutters are actually intended to cut with their sides, and which of them would fit in the Taig. And it quickly becomes obvious that I haven't a clue which types of mills are intended for what. I see center- cutting, standard, regular, etc., and I have no clear idea what is what. So any ideas? What should I be looking for? ------- Date: Mon, 19 Feb 2001 23:01:05 -0800 From: "Cliff Griffin" Subject: Re: Problems Fly Cutting Chances are you have backlash in the Z axis, and the weight of the motor etc. isn't enough to overcome the friction from the slide. As you cut, you are creating enough vibration to shake rattle and roll that slide down a bit. If you were to rap the Z axis with a mallot and THEN go do your cut, it wouldn't have taken more--or a significant amount--on the second pass. That's for discussion purposes only--don't try this at home, though. You could also loosen up the gib, but that would have detrimental effects on operations that created enough force to lift the motor assembly, and that doesn't take much at all...so don't do that either. One acceptable way to overcome this is to lower the Z axis to where you want the cut to be, and then reverse the handwheel until you juuuust feel some resistance, then lock it. This, I've found to actually work. The play in the Z axis is the main reason I only use my Sherline mill for engraving anymore. I've recently rebuilt part of it so it's better, but for the most part, I'll wait a day or two until I can borrow a friend's Real milling machine. Cliff ------- Date: Tue, 20 Feb 2001 00:05:25 -0800 From: "David Goodfellow" Subject: Re: Problems Fly Cutting I called Sherline with the same problem. Joe Martin said my gib may be too tight, so that the weight of the motor was insufficient to bring it down. He suggested I loosen the gib just enough allow the motor to come down through the backlash. I did that and it worked, and so far have not had the problem Cliff mentions below. Doesn't mean I won't, just that it hasn't so far. Dave Goodfellow ------- Date: Mon, 19 Feb 2001 11:03:43 -0600 (CST) From: Tom Benedict Subject: Re: Setting up the CNC mill I like Nick's method of indicating an edge. I use an edge-finder with a 3/8" shank, but most of my cutters are mounted in individual arbors, so this makes sense for the way I work. I'll describe that later on in this e-mail, but just understand that there are lots of ways to indicate an edge, so if you don't like one, use another. Installation 2: Mounting material to the mill bed: Now that you know your mill axes are all aligned, it's equally important to know that your work is aligned as well. Quick caveat: Most of what I'll be talking about here involves rectangular workpieces. Some workpieces don't fit into this category, so take this with a grain of salt. One example is a round piece you're drilling a bolt circle on. Rather than spending time making sure the work is square and indicating an edge, you'll be spending time clamping it down and making sure you're indicated in on the center of the piece. I won't go into great details on how to do each of these, but will only hit a couple of common ones. You can attach work to a mill bed in more ways than I can describe. Some examples are vises, collet holders, strap clamps, and tooling plates. All of these require some sort of alignment. I'll go into a couple of them: Indicating in a vise: When you first put a vise on your mill bed, it's important to make sure it's square to the bed. You use a process very similar to the one used to square your mill column. Once again, there are lots of ways to do this, so your methods may vary. The basic gist of these have a similar thread: Start by putting the vise on the mill table, and snugging down the bolts that hold it down. You still want to be able to rotate the vise, but you don't want it to slide of its own accord. Next, mount your test dial indicator on your mill head. Move the mill table until the indicator point is resting against the fixed jaw of the vise near one edge. Note the reading on the indicator. Now move the mill bed until the indicator tip traverses most of the length of the vise jaw. Chances are it'll have a different reading. Tap the vise with a soft mallet to rotate it in the right direction. Now move the mill bed back in the other direction and note the way the indicator changes. This may take a number of iterations before you get close to zero deviation across the face of the vise jaw. This is where individual methods come to the fore. Joe Martin describes his way of doing this in his book, "Tabletop Machining". My own particular method isn't very fast, but it does result in a nicely indicated vise. I'd be curious what methods other people use to indicate a vise in to see how I could improve on my own techniques. Once your vise is indicated in, you know that any rectangular piece you clamp in your vise will have one edge aligned to your mill's axes. Indicating in a Clamped Workpiece: If you're using clamps to hold your workpiece to the mill bed instead of a vise, you essentially go through the same procedure, but instead of indicating on the fixed jaw of your vise, you're indicating directly on the edge of the workpiece. But the same basic idea holds. You measure, rotate the workpiece, measure, rotate, measure, rotate, ... until the test dial indicator indicates no deviation across the edge of the piece. (Quick side note: There's no such thing as "no deviation". What you want is "acceptably close". If you're roughing out something where the edges don't really matter, "close" may be several thou across a two-inch edge. If you're cutting something that will need to mate to other parts along its edges, "close" may be less than half a thou across a two-inch edge. "no deviation" is a relative term that only you can define.) Zeroing your Axes: Once you know your workpiece is aligned to your mill axes, you need to indicate some feature on the workpiece and make that your "zero" point. (Zero is in quotes because you may or may not actually want to set your axis zeros to that point. But this is the reference point for your part. All other measurements will measure from that point. Hence "zero".) Zeroing on a Corner: To zero in on a corner, you need some way to find two edges, one in the X direction and one in the Y. Nick already described a way to do this with a dowel pin. This is an excellent way to find an edge if you're using collet-mounted cutters: On Sun, 18 Feb 2001, Nicholas Carter and Felice Luftschein wrote: > Here's how I find edges: > In a 1/4" collet I mount a 1/4" dowel pin. I set the jog to .100, > and jog the pin close to the x-axis edge I want to set as zero. set jog > to .001 and jog the dowel pin until it pinches a piece of rolling > paper between the edge and the pin. remove the paper lift the z-axis, > move it over above the vise .126 (1/2 dia. of pin and thickness of > paper) then: > setx (enter) > 0 (enter) > x (enter) \ > to zero the motor (why do I have to do this?) > Then repeat the process for the y-axis. I'm used to using an edge finder, so that's how I indicate my edges. The approach is very similar. The only difference is in how an edge-finder tells you it has hit an edge. Edge finders typically have a shank of some size (mine is 3/8"), and an indicating surface that has been ground down to a particular diameter (mine is 0.200"). The indicator surface is on a separate piece of metal from the shank. The two are connected with a spring, and can slide against each other. Once you mount the edge finder in your mill spindle, start it turning at a relatively slow speed. (I use the second-slowest pulley position on my mill for mine. You may find another speed works better for you.) The tip of the edge finder will seem to wobble. You want to bring the edge finder up against your work so that the edge of the workpiece only touches the edge finder on the indicating surface. As the edge finder contacts the surface, it'll tap it and bring the indicating surface more in line with the shank. The closer it gets, the more on-axis the indicating surface will get. Once it looks like the edge finder is spinning like one single piece, slow down. Right at the point where it's inline with the edge, the indicating surface will suddenly jump to one side and make a buzzing sound. Stop there and raise your mill head. Since the indicating surface is 0.200" in diameter, move the mill table over 0.100" to bring the axis of the mill spindle directly over the edge. That's "zero" for that axis. Repeat on the other axis, and you now have a 0,0 corner. Zeroing on a Hole or a Cylinder: To zero on the center of a hole or on the center of a cylinder, you use a method closer to how you aligned the axes of your mill. Start by mounting your test dial indicator in your mill spindle. Mine fits neatly into one of the Taig collets. You want to be able to spin it by hand while taking a reading. By eye, bring the mill spindle over the center of the hole or cylinder (I'll be refering to it as a hole from here on out. Just understand it applies equally well to cylinders.) Start bringing the mill head down until the indicator tip fits into the hole. Rotate the mill spindle by hand, and see which direction you need to move the mill bed to get it closer to alignment. Once you reach a point where it's very nearly aligned, you can start using the reading off the test dial indicator. Just remember that if you have a 10 thou difference between readings 180 degrees apart, it means you need to shift the mill bed 5 thou. Once your test dial indicator has the same reading all the way around the circle, you know your mill spindle is centered on the hole. That's your 0,0 point. Vise Stops: Nick mentioned vise stops in his post. These are Really Handy (with intentional capital letters). A vise stop is a small clamp that clips onto the fixed jaw of a vise and cinches down tight. When you mount a piece of stock in your vise, bring it up against the vise stop and close the vise. Indicate in on the corner that's up against the vise stop and the fixed jaw of the vise. Set that to 0,0. Now if you remove that piece of stock and mount a different one, you know the 0,0 point on that one will be the same as on your last one. This saves lots of time, especially if you're making a bunch of simple parts. Quick side note: When your setup time gets to be longer than your cutting time, it's a good indication that you can probably do something to make your life easier, like use a vise stop. Finding the Surface: Finding the surface of the workpiece is easiest to do with your cutter mounted on the mill spindle. (One quick caveat: The reason each of my mills has its own arbor is because it let me set them all to the same height. I can change cutters, and know that the surface height for one is the surface height for any of the others. But I still indicate the surface height with the cutter I'm going to use.) For this you use the same technique Nick uses with the 1/4" dowel pin for indicating an edge. A quick note on setting the surface height with SuperCam: When you use the Set Surface command on SuperCam, it lets you use the mouse buttons to control the height of the mill head. Once you set the surface and hit return, it will move the mill head back to where it was before you did Set Surface. For this reason, it's a good idea to simply move the mill head down until it's reasonably close to the surface before you run Set Surface. Case in point: I was making a part that required me to change cutters several times, so I'd raise the mill head up to 4.000, change tools, then set surface. The surface was around 1.125". So it spent a LOT of time traversing the Z axis. It's easier if you move it close to the surface, THEN Set Surface. At this point your work is aligned to the mill axes, you have indicated in one corner of your workpiece, and you have a cutter installed on your mill. Next installation: Cutting metal! Tom ------- Date: Mon, 19 Mar 2001 09:31:10 -0800 From: "Nicholas Carter and Felice Luftschein" Subject: Re: How to mill aluminum Jim Lewis wrote: > I've been doing a lot of milling of 3003 aluminum on the Taig CNC > mill. Just 2D stuff on 1/16" and 1/8" sheets. The only cutter I found > that works decently is a 1/8" diam round single flute router veining > bit. But it's got zero helix so chips load up and weld after some > time. I also have to go real slow - like .01"/sec. I'm using the > second to slowest pulley. The edges are not bad but could be nicer. > Faster feed breaks the bit or stops the spindle motor. I tried 2 and > 3 flute standard end mills but result was not as good. Anyone know > the right cutter? And ideal feed and speed? Thanks. Jim Are you using lube? A friend who runs a large CNC mill has a air/lube setup on a timer so that every ten seconds a blast of mist and air hits the cutter. I find I have to hit the cutter with WD-40 frequently when doing work like this, and also brush all the chips away to prevent welding. 3003 is listed as a relative "C" in machinability in Machinery's handbook, and "B" in the Alcoa handbook - this may explain some of the problem. See our web pages http://www.casco.net/~felice ------- Date: Wed, 13 Jun 2001 16:00:55 -0400 From: "Rich D." Subject: Re: Paper used in a mill setup? gartner1x~xxhome.com wrote: > Have a basic question. I've noticed in pictures of mill setups that > quite often there's what looks like a piece of paper between a vice > jaw and the part. What's the paper for? To protect the work? To > compensate for irregularities of the part? All of these? Or > something else? Thanks, Jack Hi Jack, Paper or thin cardboard helps provide a better grip (increased friction) between the part and the vise jaws. Since parts and vises seldom have truly parallel surfaces when clamped tight, at slightly compressible medium will help spread the load to more surface. Another trick is to insert a narrow bit of aluminum between the part and the moveable vise jaw as this will insure that the pressure is truly forcing the part against the fixed jaw and not at the inner corners causing the part to be effectively loose at the opposite (outer) corners. Milling across the end will frequently cause the part to grab and swing up out of the vise. Clamping with the pressure centered on one side always insures that forces are equalized across the part. Rich D. ------- From: "Rich D." Date: Tue Jul 3, 2001 10:10 am Subject: Re: [sherline] Conventional VS Climb milling SavageHB308x~xxa... wrote: >> I'm trying to understand climb milling vs conventional milling. The way I understand, since my mill spindle turns clockwise (as I sit in front of it), and I'm milling the edge of a flat plate, I would mill the edge of the plate closest to me, feeding the material from right to left? This would feed it in opposite the cutter rotation, so the cutter is pushing against the material, rather than trying to pull it along. Is this the correct direction to go (for conventional milling)? Thanks! Arden << Arden: Yes that is correct for non-climb milling. The rubbing effect is greater tho as the cutter edge starts at zero chip load and gradually increases to max at exit. A dull edge will resist entering the material until there is enough force to do so. For climb milling, the edge is coming down over solid stock and can only enter at max cut (depending on travel) and leaving at zero. This way there is minimal rubbing on the material. It is the preferred method taking into consideration the machine stiffness and slide play. RichD ------- From: "Yasmiin Davis" Date: Tue Jul 3, 2001 11:42 am Subject: RE: [sherline] Conventional VS Climb milling I will not get into a debate about this other than to warn you that climb milling can be dangerous. Is the cutter enters the work it is going to take all the end play out of the lead screw as it pulls the work towards it. This can cause the cutter to take too deep a cut and if there is a lot of end play in the machine it can break cutters, rip the material out of the work holders, etc. Perhaps this isn't significant with a Sherline but since you may some day work with larger machines beware of climb milling. As to it being the preferred method -- I would dispute that statement. Regards, Yasmiin ------- From: "Charlie Lear" Date: Tue Jul 3, 2001 8:52 pm Subject: RE: [sherline] Conventional VS Climb milling On Tue, 3 Jul 2001 08:42:14 -0700, Yasmiin Davis wrote: >As to it being the preferred method -- I would dispute that statement. Depends what you are trying to achieve. Climb milling allows faster metal removal and generally a better finish. However the machine needs to be rigid and well adjusted - you are more likely to get that with a larger mill. Cheers Charlie Lear, Melbourne, Australia Hutt Valley Model Engineer Soc. http://steammachine.com/hvmes Eastern Bays Little Blue Penguin Foundation: same site /penguins ------- From: "Rich D." Date: Tue Jul 3, 2001 4:11 pm Subject: Re: [sherline] Conventional VS Climb milling Arden, I stand by my note on climb milling and being preferred. Also note I said: "taking into consideration the machine stiffness and slide play." This goes for any machine. I was not limiting my comments to Sherline gear. All this has been hashed out in the past on other lists many times. You have to know the equipment and use the proper methods to get the job done. Climb milling is definitely more aggressive and there is an element of mishap. The end result being a much nicer finish, less wear and less work. On small machines you may have to limit the climb milling to the final pass where the best finish with a worn cutter is had. On my 5400 Mill which is CNC only and I have no "feel", I reserve the climb milling passes to the final finish cuts and these are typically under .005". When manually machining in climb mode, the slide needs to be snug to keep the cutter from pulling the lash out. The Sherline has very little mass to help resist the intermittent pulls that a 200# Bridgeport table would have no problem with. Getting the job done involves many facets to the problem and getting experience is by far the best teacher. Use the tools and find out for yourself what they can do. My Dad once "caught" me using his power drill. The one thing I remember to this day is his comment "Don't baby it, push and make it cut". That has served me for the last 45 years. Nuff said. RichD ------- From: SavageHB308... Date: Fri Jul 6, 2001 8:37 am Subject: Re: [sherline] Conventional VS Climb milling jerry.jankurax~xxs... writes: >I can see no reason why you shouldn't cut on both pieces of the stock, >provided that you can clamp it properly. When you get down to a few mils >of final size, you might want to try climb milling to assure a really >nice finish on the material. Well, in my original question, I asked about milling one side with each direction change, but my piece wasn't wide enough for that. But I did clamp it with two more clamps, and then very carefully took a smaller cut on the "return", i.e. climb milling. It really does make a nice finish, but as I discovered it also cuts more for a given movement of the dial. No big deal; it's all part of learning! Thanks to all for the comments. Arden ------- From: "Kenneth Ault" Date: Sun Aug 12, 2001 11:24 am Subject: Milling a slot - beginner's question Hello - I need to mill a 0.25 inch wide slot in a piece of aluminum. Is it best to do this with an 0.25 end mill or with a narrower mill in two passes? I thought it might be more accurate to do each side separately with a narrower mill. If I use a 0.25 mill it will be cutting on both sides to the final dimension - will that lead to problems? Thanks for your advice. Ken Ault ------- From: "Dan Statman" Date: Sun Aug 12, 2001 1:39 pm Subject: Re: [sherline] Milling a slot - beginner's question Ken, if you need the slot to be exactly .250" then you should use a smaller end mill and bring the slot width up to your final dimension. If you use a .250" endmill you will get a slightly oversized slot (probably 5 -10 thousandths too big). You will get a better bottom of the slot finish with a single pass of the 0.250" endmill, and there will be a machining line at the overlapping point if you cut it with a smaller endmill with two passes. You can also practice a few times on a piece of scrap and see how it goes. HTH, Daniel J. Statman, Statman Designs http://members.rennlist.com/statmandesigns ------- From: wanliker... Date: Sun Aug 12, 2001 2:05 pm Subject: Re: [sherline] Milling a slot - beginner's question If you want an accurate slot, this is the correct way to do it. A quarter inch mill will cut oversize if used in this fashion, also the side walls will usually be rough, due to chip problems, and mill deflection with changes in cutting feed. bill ------- Date: Tue, 23 Oct 2001 22:20:05 -0400 From: "Rich D." Subject: Re: Cutting a inside/outside radius on a mill >How do you set up the work and then how do you cut the radius >on a piece of stock with the mill. I have a turntable , but >can,t figure out how to use it for this process. >Any thoughts would be appreciated! Regards, Joe Joe, first you have to know the radius. This will be the center of rotation. The work piece is clamped to the rotary table and adjusted to obtain the radius required at the position you may have marked the piece out for. Using an endmill, cut your radius by moving the x or y mill axis toward the radius and turn the rotary table for each pass. RichD ------- Date: Tue, 23 Oct 2001 20:39:10 -0700 From: Alan Marconett KM6VV Subject: Re: Cutting a inside/outside radius on a mill Hi Joe, assuming chuck mounted "face up" (like looking at a phonograph record) on the ways, and an "outside" radius: 1) Center the "center" of the part radius you want in a 4 jaw chuck mounted on the rotary table and perpendicular to the Z (vertical) axis of the mill. 2) Position the cutter (end mill) on the above center line in 'Y', and to the right of the work piece. Bring the cutter down to the same level as the radius wanted (Z). 3) Rotate table so that start of arc is aligned with cutter. 4) Feed cutter in X until first required depth of cut, or radius is reached. 5) Rotate table Clockwise (viewed from Z or TOP) until end of cut. 6) retract cutter in X. Repeat steps 3 - 6 above until radius is finished. The key is that the rotary table is set up to "rotate" on the center of the radius we want. We want the cutter to "follow the radius", so we ultimately want the cutter's edge to be at the radius we want. Table rotation does the cutting. A four jaw chuck may not be appropriate to hold the work, use t-nuts and clamps as appropriate. For example, a rod end (piston rod) would require a "fixture"; a plate clamped to the rotary table, with a "pin" with enough head to hold the rod end in place (and perhaps another pin in the crank end), and allow the end to be cut through the 300 or so degrees wanted. One would first "center" on one end of the rod, cut the radius, then center on the other end, and cut it's radius. Alan KM6VV ------- Date: Wed, 24 Oct 2001 09:27:04 -0700 From: "Craig Libuse" Subject: Re: Cutting a inside/outside radius on a mill >I have a turntable , but can,t figure out how to use it for this process. Joe, You can find instructions for use of a rotary table at www.sherline.com/3700inst.htm It is for Sherline's table, but the instructions for tool offset and so on apply to all rotary tables. HTH. Craig Libuse Sherline Products ------- Date: Wed, 28 Nov 2001 08:50:06 -0800 From: "Marcus & Eva" Subject: Re: Milling Problem Original Message----- From: John Barnwell To: sherlinex~xxyahoogroups.com Date: Tuesday, November 27, 2001 8:31 PM Subject: RE: [sherline] Milling Problem >Got a hammer and chisel? >After all its only aluminum. >A "Cape chisel" is what you want. >John Barnwell >barnwellx~xxjlsystems.to >Voice: 978-534-4096 >Cell: 978-807-8475 >> Original Message----- >> From: doug.kelleyx~xxalaskaair.com [mailto:doug.kelleyx~xxalaskaair.com] >> Sent: Tuesday, November 27, 2001 7:13 PM >> To: sherlinex~xxyahoogroups.com >> Subject: [sherline] Milling Problem >> I just purchased a Sherline mill and I'm contemplating my first >> project. I was thinking a Soma puzzle would be simple enough for >> someone with no previous experience. If you aren't familiar with the >> puzzle, it's a 3 x 3 x 3 cube. The cube itself is made up of 27 >> smaller cubes, grouped in various configurations. The puzzle (which >> isn't very difficult to solve) is to arrange the groups of smaller >> cubes to make the larger cube. Various other shapes can also be made. >> >> I want to make the 27 smaller cubes from 1" x 1" x 1" brass. I also >> want to have an aluminum base that the cube can rest in. The base >> would be 3.5" x 3.5" x 0.5" with a .25" deep recess milled into the >> plate to accept the brass cube. If this isn't clear, maybe the >> following ASCII art will explain it: >> >> __ __ >> | |__________________| | >> |________________________| Side view >> >> >> ________________________ >> | | >> | ____________________ | >> | | | | >> | | | | >> | | | | Top view >> | | | | >> | | | | >> | | | | >> | | | | >> | | | | >> | |__________________| | >> | | >> |________________________| >> >> Use a font like Courier to view the above diagram properly. >> >> Here's my problem: I need the corners to be square but if I mill out >> the center of the plate, I'll have round corners. I want the base to >> be made from a solid aluminum plate. I know I've seen square "holes" >> before; how are they made? Or is this topic too advanced for someone >> with no experience? >> Thanks for any input you may have. Please respond directly to me. Doug Hi John: There's 3 ways to do this: 1) mill with the tiniest cutters you can and chisel, broach or file the rest. 2) insert the ends. ( make an "H" shaped pocket and pound in 2 plugs on the ends) 3) EDM the pocket. Your choice will be dictated by the space available, the accuracy required, and the gear you have. Option #2 is the most accurate for HSM's, but requires the most space. Option #1 is what most people typically do (or try to do) Making and aligning the corner broach is the hardest part of method #1 Cheers Marcus ------- Date: Wed, 28 Nov 2001 11:23:51 -0500 From: "Kevin P. Martin" Subject: RE: Milling Problem Marcus wrote: >Hi John: There's 3 ways to do this: 4) Use a v-tipped cutter and an angled head position so the tip of the cutter can reach right into the lower corner. The math is ugly (and easy to get wrong), the setup is a pain, and you get inefficient cutting at the tip of a V cutter because there is so little linear speed. Kevin Martin ------- Date: Wed, 28 Nov 2001 20:41:27 -0000 From: paul_probusx~xxyahoo.com Subject: Re: Milling Problem (See Ty's message below) The same could be done with a very small endmill (1/16" or smaller if you like) instead. Use the small endmill to make the last few fine cuts to remove the large radius from the larger endmill(s) (and bring the cutout to its final dimension)[Note: As you get within a 1/4" of your final dimensions you might consider using progressively smaller diameter endmills until the final endmill is the 1/16" (or smaller) endmill.] Then take that small endmill and carefully plunge cut out the small radius on each corner just enough so that the remaing small radius will not interfere with the blocks. It may not look exactly right since you will not have a sharp corner, but it is quicker and easier than some of the other methods suggested. If the idea is to impress other people, they probably will not notice that small "defect" at all. If the idea is to impress yourself, then use one of the other suggestions. Of course, nothing says that you can't make it with a small "defect" now and when you get more proficient at machining, make another one later. That's one of the problems with HSM's, we're always improving our techniques and going back to improve some of our previous projects. :*) Paul --- In sherlinex~xxy..., Ty Hoeffer wrote: > Or ( Possibly non-elegant but simple ) drill a small hole at the > corner ( its center being at the point that the corner should be. ) a > 1/16" or 1/8" drill would work depending on what size end mills you have: > > WARNING ** CRUDE ASCII GFX FOLLOWS ** > > o--------------------------o > | | > | | > | | > | | > | | > | | > | | > | | > | | > | | > | | > | | > o--------------------------o > > Ty ------- Date: Wed, 28 Nov 2001 21:10:09 -0000 From: jkiefferx~xxmge.com Subject: Re: Milling Problem Doug, one way of doing this would be to machine the square all the way through the material so it would look like a picture frame. Then file the corners square and press fit or recess and mount a bottom plate with screws. Jerry Kieffer ------- Date: Wed, 28 Nov 2001 21:31:11 -0800 From: "Marcus & Eva" Subject: Re: Milling Problem Hi Kevin: Good call. I forgot that one!! We used to pick out corners with that method by scribbling all over the milled sidewalls with a felt pen and then picking up the cutter position by advancing in small increments until we just touched. Zero the handwheels and away you go. Cheers Marcus ------- Date: Fri, 30 Nov 2001 15:31:14 -0000 From: "David" Subject: Re: Milling Problem When using the chisel method you might want to clamp two pieces of angle iron onto the top of the work-piece flush and parallel with the edges forming a corner above the corner you are going to cut. Use at least two clamps on each angle iron to prevent them pivoting. I have used a square lathe tool bit as a chisel for this job. Just grind a relief on the end. Hold the chisel in the corner formed by the angle irons with your fingers or attach a magnet such as a dial base to the outside of angle irons to hold the chisel hands free. The bit will fall onto the work with the hands free mathod so you should put down some paper to protect the work surface. Just light taps will do in aluminum checking visually for clamp slippage after each tap. It's still easy to mess up with a chisel so it's best to practice first. David ------- Date: Thu, 6 Dec 2001 09:12:04 -0800 From: "Marcus & Eva" Subject: Re: DRO From: "Bad Brad" To: Sent: Thursday, December 06, 2001 7:09 AM > Just starting out, > Give dial reading a go first. For the beginner the benifit of learned > dial use improves your skills. Purchase a digital caliper to do quick > calculations for cuts, a more accurate way than using a DRO mounted > on the lathe or mill and cheaper too. Forrest Yes: And do a layout on the job first. Doesn't need to be all that accurate but it keeps you from having to count turns. Use a felt pen for layout fluid, and a cheap vernier caliper with the jaws ground to a sharp tip as a layout gauge. (Unless you've got a surface plate and height gage). Layouts will save your bacon...frequently!!! Cheers Marcus ------- Date: Sun, 16 Dec 2001 19:26:45 -0500 From: "Paul & Charlene Wilson" Subject: Help needed! I need some help from experienced machinists .... I am working on a very intricate piece for my son that involves a lot of complex curves cut with a very small milling cutter - I can do all the setups, cuts, etc. but have run into a problem with actually DOING it. I have made almost the first of about 27 cuts and have already broken both ends of a new 1/16" cutter. Any ideas for getting this done? I am running a fairly high speed - 1000 rpm or so, flooding the cut with aluminum cutting fluid, cutting at low speed (by hand on my rotary table) and still breaking the cutter! Ideas? I just ordered another 5 cutters, but at this rate, it won't be enough! HELLP! Thanks Paul ------- Date: Sun, 16 Dec 2001 18:33:48 -0600 From: Jim Irwin Subject: Re: Help needed! Your 1000rpm spindle speed is way too low. I'd guess even 10,000rpm might be still low for a 1/16 dia cutter with flood or mist coolant. Can't you use a larger diameter cutter? Also, what aluminum alloy are you using? It does matter! Low machineability stuff gets gummy and causes heck in machining. Best regards, Jim Irwin ------- Date: Sun, 16 Dec 2001 19:38:48 -0800 From: Steven Harris <79ramchargerx~xxhome.com> Subject: Re: Help needed! From the back of my J&L Industries catalog it says for aluminum/aluminum alloys using solid carbide end mills the speed should be 600 - 1200 (sfm) and the feed per tooth should be .0002" - .0020". It also says if you are doing slotting applications speed should be reduced approximately 20% of lowest range value and above recommendations are to be used when axial depth of cut does not exceed 1.5 times the cutter diameter. When using long and extra-long end mills reduce feed per tooth 50%. I have not done much mill work. I hope this info helps. Merry Christmas, Steve ------- Date: Sun, 16 Dec 2001 22:55:13 -0600 From: Jim Irwin Subject: Re: Help needed! Steven Harris wrote: >From the back of my J&L Industries catalog it says for aluminum/aluminum >alloys using solid carbide end mills the speed should be 600 - 1200 (sfm) This gives about 36,000 rpm better have a really high precision spindle! >and the feed per tooth should be .0002" - .0020". This gives (2-flute cutter assumed) about 14.4 in per minute at slowest feed rate 144 at fastest! WOW! >It also says if you are doing slotting applications speed should be reduced approximately 20% of lowest range value and above recommendations are to be used when axial depth of cut does not exceed 1.5 times the cutter diameter. When using long and extra-long end mills reduce feed per tooth 50%. Reduce by all these factors and you get a feed rate of 5.76 in/min IOW...no matter how fast your spindle is going, it ain't fast enough! Best regards, Jim Irwin ------- Date: Mon, 17 Dec 2001 09:12:43 -0500 From: mark usik Subject: Re: Help needed! Make sure that you are conventional milling (cutter is trying to keep itself from advancing into the work) as opposed to climb milling (cutter tries to climb or self feed). Any backlash in your setup will allow the cutter to take too big of a "bite" during climb milling ....and we know the rest of the story. Climb milling is used on large , very rigid machines with "zero backlash" to give a better finish over conventional milled surfaces. ------- Date: Mon, 17 Dec 2001 09:34:57 -0800 From: "Bob May" Subject: Re: Help needed! The speed is way too slow. Run the machine up as fast as it will go and go extremely slow (make a bump on the wheel and you'll break a cutter!) If you're used to a 3/8" cutter as a normal sized cutter, you'll find that the speed needs to be at least 6 times faster and the feed rate to be 6 times slower. You also don't want to be cutting that deep a hole with such a cutter. Even slower is better with such cutters. I used to do mold work on a pantograph mill and that is all handwork for moving the cutter about and doing something like a 1" long cut was an exercise in patience! Bob May http://nav.to/bobmay NEW! http://bobmay.astronomy.net ------- Date: Mon, 17 Dec 2001 09:52:37 -0800 From: Frank Evan Perdicaro Subject: Help needed? SHHH! Don't tell anybody, especially any real machinists, but for problems like this that do not involve very important work, I use a wood router and a carbide bit. A wood router spins fast enough. If you can clamp it over your rotary table, prentend you have a milling machine. You can even freehand mill slots. I've done up to 5/8" slots 1/4" wide in a single pass by hand. ------- Date: Wed, 19 Dec 2001 20:22:32 -0500 From: "Paul & Charlene Wilson" Subject: Success, so far Thanks to all who sent suggestions on my intricate curves milling problem with a 1/16" mill; I got a new cutter today (actually several; no faith!) and after setting the mill to max RPM (3100 or so) I have made 4 cuts (out of 40 or so) with no breakage. So far so good ... lessons: - Max RPM - Feed SLOW! - Flood the cut with Aluminum Tap Magic - Keep chips cleared (same brush that applies cutting fluid) It's a mess, and slow, but getting there! Probably not this year, but soon >)! Paul ------- Date: Sun, 16 Jun 2002 13:55:40 -0500 (CDT) From: Tom Benedict Subject: Re: Speeds & Feeds for soft metals On Sun, 16 Jun 2002, jimbarb02760 wrote: > I will be milling(CNC) small highly detailed models made of pure tin. > Cutters will be from .010 flat conical to .250 two flute. I haven't > been able to find information on optimal spindle speeds and feed rates > for soft metals. Any help would be appreciated. Funky! My initial response was going to be, "Consult Machinery's Handbook, page..." So I went to look up the page. And I'll be danged if I can find it! You're right. All of the light metals they list are aluminum alloys, magnesium, and die castable aluminum alloys. No tin. Some things to keep in mind regarding speeds and feeds: What Machinery's Handbook calls "optimal" is "this is as fast as you can cut without destroying your cutter in seconds". They spell this out pretty clearly in the opening pages of the chapter on machining operations. Running at a slower speed means your tooling lasts longer. So a production shop strikes a balance between tool life and machining speed. If you spend all your time changing worn tools, you're losing. But if you're using a feed rate of 1"/minute, you're also losing. So you strike a balance. Unless you're making a massive production run, chances are you can run your tools at a slower spindle speed, and adjust your feed rate accordingly. Looking at the table of recommended feed in inches per tooth for milling with high speed steel cutters, the fasted feed rates (for cast aluminum alloys and magnesium alloys) is 0.003" per tooth. Most of the steels are around 0.001" per tooth. Take that as a ballpark range. I've never cut pure tin, but I'd opt toward the heavier end of the scale. If you take your spindle speed, and the number of flutes on your cutter, you can calculate a feed rate based off of those parameters. Past that, I'd see what works. Try different spindle speeds and associated feed rates, and see what kind of surface finish you get. You said they're highly detailed models. My guess is you'd be after good surface finish more than massive cutting speeds. Take a cutter and some scrap tin, run through the spindle speeds available to you and calculate your feed rates. Look at the resulting surface under a magnifier, and see what you think is acceptable. Pick that one, and cut tin. Sorry I couldn't be of more help. Like you said, that data's not easy to find! Tom ------- Date: Sun, 16 Jun 2002 23:47:17 -0400 From: Stan Stocker Subject: Re: Speeds & Feeds for soft metals Goofy as it sounds, whipping cream or half and half are about the best cutting lubes for copper. A pain to clean up after, but you do get an excellent cut. Stan ------- Date: Thu, 20 Jun 2002 08:56:51 +0100 From: Tony Jeffree Subject: Re: Depth Stop collars on milling bits >Is there anything wrong (dangerous) with putting aluminium collars with >setscrews onto end mills so as to limit the depth they are inserted the >collets? Can't see why this would be a problem, as long as there is no possibility of the collar coming loose during milling. If you used a split clamp type of collar rather than setscrew, there would be less chance of it coming loose. Regards, Tony ------- Date: Mon, 24 Jun 2002 08:49:42 -0500 From: Bob Kelly Subject: Re: Carving Semi-Precious Gems On 23-Jun-02, rrhewson wrote: > I tried carving a small piece of jade using diamond tips with my > Dremel. It works, but sure was slow. Jade is a lot harder than I thought. > Good magazine to reference is Lapidairy Journal (Boreds, Barnes & > Nobel, Chapters etc shold carry it. Bob > --- In taigtoolsx~xxy..., "rainnea" wrote: >> Seeing as we're discussing glass-cutting I was wondering if it > would be possible to carve a pattern into gemstones with for example a >> diamond tipped dental bur. Has anyone tried this sort of thing? Rab Bob, the difference between a Dremel and a dental drill is amazing. I got a brand new air drill when new rules about autoclaving (sterilizing) came out and a dentist had to scrap a new one. That was probably 15 years ago. I think it runs over 150,000 rpm and really eats stone. I am thinking of making a mount for it on the taig so I can hand crank the lathe and let the drill do the work. About the only thing the drill doesn't like is aluminum. It clogs whatever bit I try. Bob Kelly ------- Date: Thu, 7 Nov 2002 13:04:36 -0500 From: "j.guenther" Subject: RE: Advice on milling material larger than machine capacity > I am considering purchasing a Taig CNC Mill and was wondering if it > is possible/practical to work on material that is 6.5"(L) by > 6.5"(W). The Y axis on the machine I am considering has a maximum > travel of 5.5" and I will need to cut slots in the piece that go all > the way to both ends. > I imagine I could probably make half the cuts then move the > workpiece over some and make the rest of the cuts, however, I'm > concerned about how easily and accurately this can be accomplished. > Has anyone done this, and if so, is it worth the hassle or should I > look for a larger capacity machine. I will be producing a fair > number of the same part so if it is significant trouble getting > everything to line up properly I would probably look for a larger > machine. On the other hand, if it is relatively easy to make the > adjustment and get the machine lined up correctly, I think I would > go with the Taig. Any help would be greatly appreciated, Wally I had a similar problem when milling the 4.5 x 14 inch front panel for my CNC driver box. What I did was to make an "L" shaped alignment guide (sort of a jig) to align the panel along the X and Y axis. This allowed me to machine 1/2 of the panel and then flip it over to machine the other half. I made only one front panel and one back panel but I could have easily made as many as I wanted. This "L" shaped alignment jig was just two pieces of aluminum bar bolted to the tooling plate on my Sherline mill table and the inside surfaces aligned to the X and Y axis. This could be done with a DTI or you could take a light cut on the inside faces of the L to square them up to each axis. I wrote the code to cut the panel such that there was a program for the right half of the panel and one for the left half of the panel. I cut one half, flipped it over and cut the other half. When complete the panel looks as though it was cut in one setting. The panel contains 4 2" diameter holes for cooling fans, a hole for a standard printer connector, holes for 4 connectors for the stepper motors, 3 switches and 30 holes for screws to mount the fans, connectors and some internal brackets. I can provide a picture of the completed front panel if needed. HTH. John Guenther 'Ye Olde Pen Maker' Sterling, Virginia ------- Date: Fri, 07 Feb 2003 17:03:16 -0000 From: "cobbkev " Subject: Setup for subsequent holes I have what you might consider a VERY basic newbie question: I am adding multiple holes to a plate that require multiple passes. First center drill then through drill and finally a counter bore and maybe a slight chamfer at the rims (eight total). Do I center drill all the holes first (noting handwheel revolutions and direction) and then change to drill and then through drill all (matching handwheels and direction), etc? Or is it better to center drill, switch to drill, then counter bore etc. before going to the next hole? I've tried MUCH reading before making too many first newbie chips but I don't see this anywhere. Most books usually say "after all your holes are finished, do the following"... Am I making this too complicated? Thanks a bunch! Kevin ------- Date: Fri, 7 Feb 2003 12:21:58 -0500 From: "Ned Carey" Subject: Re: Setup for subsequent holes >Do I center drill all the holes first noting handwheel revolutions. Kevin Which is more of a pain in the the ass to you, changing bits or turning the handwheel and counting revolutions? I don't think it really makes a difference as long as you remember your backlash and count correctly. Ned ------- Date: Fri, 7 Feb 2003 19:20:30 -0800 From: "Carol & Jerry Jankura" Subject: RE: Setup for subsequent holes Hi, Kevin: I'd suggest that you drill all of the center holes, then go back with the drill to complete the job. You'll have to be careful - 1. Set the Zero for both the X and Y axes after you've moved to the edge of the material from a direction which moves the table towards the spindle center. 2. Approach all holes from the same direction. IOW, start with the table to the right of the spindle and moved all the ways into the Z axis column. 3. Always approach a new Y by moving the table away from the column. 4. Always approach a new X by moving the table to the left. Don't 'zig-zag' left and right. 5. When returning X or Y to the 'zero' location, always overshoot and approach your zero from the same side. -- Jerry ------- Date: Fri, 7 Feb 2003 20:58:11 -0800 From: "Marcus & Eva" Subject: Re: Setup for subsequent holes Hi Ned and others: Once you've established the locations with the first tool (or even with a layout), there's no need to count revolutions anymore. All you need to remember is what the dial reading was at each location, and which way the backlash was when you approached the location the first time. You can use the divot in the job that you made with the first tool to eyeball within one dial revolution and then just go to the handwheel setting you memorized (or wrote down). I run a Bridgeport daily, and I've NEVER counted handwheel revolutions in my life. (No, I don't have a readout on the machine) I scribble on some magic marker and scratch a layout onto the workpiece, often just with a beater vernier caliper that I keep pointy on the jaws with an India stone. The layout doesn't have to be accurate, it just has to be close enough that you can't misread the position by one handwheel revolution. So, you just run from your reference location to "pretty close" to the layout line, and then dial in the reading you want. This method is as accurate as the table feedscrew is, and it's WAY faster than a readout once you get good at it. So...abandon the painful tedium of handwheel counting...on a Sherline with its fine pitch screw, you'll be counting forever, and you'll never know if you've made a miscount screwup until you measure the locations, and say those words that you can't let your kids hear. Cheers Marcus ------- Date: Wed, 26 Feb 2003 18:50:32 -0800 (PST) From: Pete Brown Subject: Cutting a perfect square inside material Just a puzzler (for me anyway). I don't have need to do this just yet, but I suspect I will. Without file cleanup, is it possible to cut a perfect square or rectangle with 90 degree inside corners on the interior of a flat piece? For example (square holes are marked with "h"). Assume the holes go all the way through the material. Best if viewed with a font like courier. +--------------------------+ | +-----+ +-----+ | 1" | | h | | h | | | +-----+ +-----+ | +--------------------------+ 3" Assume the piece is 1" x 3" and the holes are each 3/4" x 1". Assume thickness of the piece is 1/4" or something like that. Without resorting to a file or cold chisel after the milling, I can't see how to do that on a mill. Any suggestions? Thanks. Pete ------- Date: Wed, 26 Feb 2003 19:10:45 -0800 From: Alan Marconett KM6VV Subject: Re: Cutting a perfect square inside material Pete, you have to use SQUARE endmills! ;>) Alan KM6VV ps Not to my knowledge! I think you'd have to use a broach. Mill out as much as you can, then press a broach through the holes. ------- Date: Wed, 26 Feb 2003 22:42:09 EST From: tadici283x~xxcs.com Subject: Re: Cutting a perfect square inside material Hey I got a laugh out of that, but to answer your question No, you cannot get a perfect square from a round endmill based on the equipment mentioned, you can use a small diameter endmill to get a very square hole, but it will in the corners still be rounded, so how can you do it? One way is to broach it, like a keyway in a collar; another way is to mill it in two parts and screw, weld, glue it together, by machining it in two parts with the endmill cutting to the side of the square and not form the top. Why do you need it perfect anyway? Almost any project can be done with a nearly square hole that is tightly machined. Note there are other ways to make square holes such a punching it out, but I did not mention it due to the fact that this doesn't pertain to Sherline equipment and the equipment is expensive and specialized. Chris of Bradenton FLA. ------- Date: Thu, 27 Feb 2003 04:18:42 -0000 From: "Les_Grenz " Subject: Re: Cutting a perfect square inside material It could be done with a shaper. However, a shaper is not always available. Regards, Les http://www.lesgrenz.homestead.com/Leshomepage.html ------- Date: Wed, 26 Feb 2003 20:24:02 -0800 From: Brian Pitt Subject: Re: Cutting a perfect square inside material I had to do something like that once on a knee mill and one of the 'old boys' walked me thru it you use a cutter with a 60deg point like a center drill with the pilot ground down to the center flutes and thin the web so it is as pointy as possible tip the head 45deg to the side and 45deg back (or forward) then raise the knee to make the cut down the inside corner on the sherline you don't have the knee but you can tilt the head on the Z-axis and mount the work at an angle on the table to get the same kind of thing going on with maybe some adjustments to the angles (the trig part of my brain is broken right now :) the cone of the cutter should be 90deg looking straight down on it to make a square inside corner make a big 60deg paper cone and hold it at the right angles to fit into the corner of a room or doorway and you can get a good idea how it works Brian ------- Date: Thu, 27 Feb 2003 14:35:04 -0000 From: "lan_brooks " Subject: Re: Cutting a perfect square inside material Another, much more complex solution is to get the Home Shop Machinest book on building an Electronic Discharge Machine, build the EDM and using a square/rectangular electrode erode the hole. Actually, I am faced with a similar situation where the hole I need is 3/32" by 1/4 " but 1" deep and a need two holes per part and about a dozen parts. Broaching is one solution, EDM another and I hadn't thought about making the part in two pieces since it is a prototype and I like real looking prototypes. I started gettign ready to make the EDM but did not have easy access to appropriate parts in the small town where I live at a reasonable price. For your part, many of the ideas others have had sound workable especially the pointed end mill, the real issue is how thick is the part. For a thick part, where the pointed mill will not go all the way through, broaching would work well. You would need to make a bushing that fits the hole, had three chamfered corners sufficient to clear the radius left by the end mill and a square or rectangular notch in the remaining corner that fit the broach. This won't work for my project due to the cross section of the 3/32 standard broack. If you can select the end mill size, you can then select a broach with a square cross section. Good luck, Lan ------- Date: Mon, 10 Mar 2003 21:32:26 -0000 From: "JohnW" Subject: Re: cutting ovals [sherline] kevin_sedota wrote: > > How would you cut a plate in the shape of an oval or ellipse? > > Without CNC. thanks, kjs Alan Marconett KM6VV wrote: > Hi Kevin, > It would be tough! You could generate a set of coordinates using BASIC > or a spread sheet, and then TRY to go to each coordinate in sequence. > Trouble is, you should turn both X and Y handwheels at once to get to > the new coordinate! If the moves were small, perhaps it wouldn't be too > far off, even if only one were turned at a time. I wouldn't be up to it! > The other option is to rig a pantograph (sp?), or tracer somehow. > This is done on lathes, don't know about doing it on a Sherline mill. > Alan KM6VV Kevin: The oval chuck in HSM than Glen mentioned should do the trick. It was mounted to a rotary table to get the circular motion. The chuck works on the same principle as the "do nothing crank". I'll try to describe how the crank works, but don't ask for a picture or drawing ;-( A block of wood has tracks cut at right anges to each other and crossing in the middle. The crank has two small rectanglular pieces of wood attached that ride in these two tracks. When you turn the crank each sliding block moves back and forth in its respective track. The handle travels in an oval. The difference between the major and minor diameters of the oval depend upon how far apart the two sliding blocks are mounted on the crank. I'm sure you've seen one and I hope that my description was good enough for you to guess what I'm talking about. John ------- Date: Wed, 16 Apr 2003 07:00:31 -0000 From: "sikn1gh7" Subject: Re: Drip Oiler for Cutting Steel on Mill? Pick up a separatory funnel from your local science surplus store. You can tune the teflon stop-cork for some pretty nice drip rates. If I were to home-brew a drip coolant system, that's the route I'd go. http://www.sciplus.com/category.cfm?subsection=4 Terence ------- Date: Wed, 16 Apr 2003 13:48:16 -0000 From: "JohnW" Subject: Re: Drip Oiler for Cutting Steel on Mill? Mug a hospital patient and take his IV drip. ;-) Or copy the concept. Use a small valve or an adjustable pinch clamp to control the drip rate. Copper tubing is easy to bend and can be used to direct the drips where you want them. Haven't done it yet but that's my design. John ------- Date: Wed, 24 Sep 2003 09:51:19 -0700 From: "Marcus" Subject: Re: Working outside of Sherline's milling envelope [NOTE TO FILE: sherline group posting but of interest to other machines] > I'm a couple of weeks away from my first major project using a CNC'd > Sherline 2000 mill. I'd like to see if I'm on track so that I don't > scrape some relatively expensive material (aluminium tooling plate). > The piece is to be an 18" X 5.5" slide milled from 3/4" stock. It > requires a dovetail, straight within 0.001", and 10 threaded holes to > be machined into it. How committed are you to completing this job in-house?? It sounds like your requirements can only be met if you are willing to spend a lot of time fussing over your setup. An 18" slide milled to within 0.001" is a reasonably difficult challenge even on a machine that has the stroke. Just the warpage of the block is likely to throw you out of tolerance, nevermind the errors introduced by the progressive warming of your entire setup as the cuts progress. If you are certain you can get there by milling and scraping, then you may choose to do it in spite of the time penalty, but you can be certain it'll be a long process if you REALLY have to get within 0.001" over 18". I'm assuming the job will be aluminum? If you get a nice hard grade like 7075 or Alumec 89, you can surface grind it successfully. I'd mill this job on a reasonable sized mill and then plan to grind it to final dimensions. Good luck with it, however you choose to go. If you do choose to mill it, you'll want to let it stabilize after you hog out the worst of the stock. I'd rough mill it within 0.030" and stick it in the freezer for a week. Then I'd semifinish to within 0.005" and freeze it again. Last I'd kiss it with brand new cutters freeze it one last time, and then scrape it in. The subzero ageing is supposed to accelerate the stress relieving process. Shot peening is supposed to help too. Remember to remove stock from both sides of the block, otherwise the asymmetric stresses will make it curl. I know tooling plate is not supposed to do that, but in my experience it often does anyway. Cheers Marcus ------- Date: Thu, 25 Sep 2003 14:19:16 -0000 From: "Antonius J.M. Groothuizen" Subject: Re: Working outside of Sherline's milling envelope Marcus: Thanks for your insight. I am committed to completing this in-house as it is personal, and I can't afford to farm it out. I blew my wad buying the equipment. I can afford to take my time to do this right and will test some of my procedures using PVC and smaller pieces of cheap aluminum from the scrapyard. I set the tight tolerance for myself as this is the first step in expanding the milling envelope on my Sherline 2000. The accuracy of future projects depends on this one. I was considering precipitation strengthening (aging) the 7075 by putting it in the oven at 250 F for 24 hours and air cooling it after hogging out the material, and once again after final machining. (I do the cooking around here, so it's my oven ;-) From your comments it would seem that I'd be better off putting it in the deep freeze. Would a semi-controlled return to room temperature (fridge freezer, fridge, room) offer any advantage? I'll hog the material out starting with a 'W' profile, alternating sides from the center, and allowing cool-down time between cuts to minimize curling. Tony ------- Date: Thu, 25 Sep 2003 08:41:14 -0700 From: "Marcus and Eva" Subject: Re: Re: Working outside of Sherline's milling envelope Hi Tony: The information I have on subzero ageing is all hearsay, so I can't comment definitively on its value. Certainly any process that accelerates stress release will help you and temperature swings will do so. Once upon a time castings were aged by leaving them out in the yard for a decade. They were also hung up and thumped with rawhide hammers. As I mentioned previously, shot peening has been used as well. The short version is that anything you can think of to accelerate the stress release process will help you. With regard to the actual machining operation, you want to minimise stresses from clamping and realigning. Get yourself some thin shim stock or a couple of packs of feeler gages. You'll want to have a clock on the part at all times as you tighten the clamps down...that way you can tell immediately if you're pulling it out of alignment with the clamp. I've laid parts like these on double sided tape and then just blocked them into position, so they can't shift sideways. With light cuts, this is a very successful way of avoiding the twisting forces of clamps. The main thing is be gentle as you set up the parts when you're finishing them. There'll be a whole lot less scraping to fit if you do. Cheers Marcus ------- Date: Thu, 25 Sep 2003 16:47:13 -0000 From: "Charles Hixon" Subject: Re: Working outside of Sherline's milling envelope Marcus, Good call with "subzero ageing". Since temperature does change dimensions ever so slightly, it will allow a non-measurable amount of crystalline slippage where internal micro stresses are the greatest. One "subzero age" cycle in aluminum might be equivalent to one thump with a rawhide hammer. With reference to aluminum, and metals in general, ageing typically means hardening by inducing internal stresses through the precipitation of compounds into a crystalline lattice structure. Hardness dervied by inducing internal stresses warps the metal. This is the opposite of dimensional stability. Better terms which may be used to define enhancing dimensional stability might be annealing, normalizing, tempering, stress- relieving, or softening. An exception you brought up is "aging" of castings, which was done to cull out those castings which would crack for mysterious reasons. The mystery is gone now through our understanding of metallurgy and the application of heat treatment. There is a "subzero" treatment applied to certain hardened steels but that's another topic. Shot peening introduces residual stresses and hardness to the surface by virtue of cold working - if the material grade responds to work hardening. If it doesn't, then shot peening only roughens and possibly warps the surface. Either way shot peening creates a dimensional stability problem. Charles Hixon ------- Date: Mon, 17 Nov 2003 08:27:18 -1000 (HST) From: Tom Benedict Subject: Re: Turning on Mill [POSTED TO TAIGTOOLS GROUP] On Mon, 17 Nov 2003, Robert MacLellan wrote: > Thanks all for their responses to my really simple question posted > earlier. Am now starting to think the Micro Mill might be a better way > to go. Will likely be seeing a 70/30 milling/turning environment. So, > is it possible/advisable to turn using the Mill? Yes it is, but there are some caveats. For starters the mill spindle motor is a lot weaker than the one used on the lathe. If you're turning large stuff, you'll either want to replace the mill spindle motor with something a little beefier, or you'll want an honest to goodness lathe. Changing setups takes time. What that means is it's a pain to go from lathe to mill to lathe. Any time my hobbies get to be a pain, I lose interest in the hobby. If you're looking at a 90/10 milling/turning environment, I'd say go for it with few or no hesitations. If you're talking about a 70/30, still consider picking up a lathe. Something to think about: The Taig lathe and mill both use the same spindle. The accessories that go on the one will go on the other. My lathe cost me less than two hundred bucks. My lathe accessories easily cost me twice that. When I got my mill it meant I didn't have to get a lot of extra tooling for it because I already had it for my lathe. The reverse would've been true if I'd bought the mill first. If you're going to be tooling up with a mill, consider picking up a bare-bones lathe along with it. > Either by: 1. mounting chuck on mill head (after all is same unit > as lathe) and tool on mill bed? Yep. This is how I've done some face milling on my mill. At one point there were some pictures in the Files area showing my mill set up as a lathe. I asked Nick to erase them because they were photos and not files, and were eating up too much space. As soon as I can get around to it, I'll duplicate the setup and take more pictures to post in the Photos area. Mounting the chuck this way is dead easy. It just screws onto the spindle, same as on the lathe. Mounting the lathe tools is a little tougher. With the mill spindle mounted vertically, you can bolt all the lathe tools to the mill table with the pointy ends facing up. But it means lowering the mill spindle WAY down. With the mill spindle pointed horizontally you need the tools mounted pretty high up to get decent throw. I've been cobbling setups for both configurations, but your best bet would be to treat it like an honest to goodness shop project and make a lathe tool holding fixture for your mill table. The way I'm doing it right now is juuuust frustrating enough that it takes some convincing to make me set my mill up as a lathe. If I had a dedicated fixture I'd be a lot more likely to do it. > 2. Using vertically mounted rotary table/chuck and maybe tail stock? I haven't done this, but I did make an adapter plate so my lathe can mount on the mill table. That lets me do lathe work with two live spindles, or pull the headstock off the mill and replace it with conventional lathe tooling. I'm going to be using this setup pretty heavily in the next couple of weeks, so I'll take pictures and report on how it works. > Anyone had any experience doing this? Some. But no, not enough. Never enough. ;) Tom ------- NOTE TO FILE: This thread was how to mill large areas in a Taig lathe, with the suggestion that hogging out most of the metal with a drill bit first was the best way to proceed. Then someone started talking about using mill bits in a drill press, and Clive contributed the following message. To see the rest of the thread go to the file Taig Lathe Tips. It is generally accepted that MILLING ON A DRILL PRESS IS UNSAFE AND IT IS NOT RECOMMENDED. ------- Date: Tue, 2 Dec 2003 15:05:36 +0000 From: Clive Foster Subject: Re: Milling large volumes Gents, I can confirm that attempting to use an end-mill in a normal drill press will cause the chuck to walk out if it is on a separate morse taper arbor. The chuck wont walk off a good jacobs taper so if its a press fit on the end of the spindle you will almost certainly be OK providing the tapers are somewhere near accurate. Unfortunately the end mill will probably walk out of the chuck! The spiral side flutes put a decent pulling force on the mill which the hard steel on hard steel grip of the chuck jaws just wont withstand for long. Light end milling on drill presses is possible. Some makes were specifically made with that capability eg Fobco but the bearings etc are a cut above the usual. However you can upgrade, within reason, even a cheapy for light milling. Do it somewhat like this:- To start with it is best to pick one with a morse taper arbor and a proper spline drive from the pulley. A single slot key-way drive can be used but you ill almost certainly have to make a snug fitting, full depth key properly retained in the drive pulley. Hard work if you don't have machine shop access 'cos its gotta be accurate. Make the end-mill holders from blank end morse taper arbours, one for each size of milling cutter shank. Plain holes with a side set-screw engaging in a flat on the cutter shank will do fine (its what is used for the throw-away cutters after all) but if you are feeling swanky thread them as well for screw in cutters. You can buy suitable morse taper holders but they are threaded for a draw-bar so you need add a tang substitute so that the ejector drift has something to work on. A hollow cap nut passing over the business end and screwing onto the spindle will stop the end-mill holder walking out. Depending on sizes you may want to weld on a washer to the big end of the morse taper to give the cap nut more to register on. Obviously the hole in the cap nut must pass all sizes of end mill holder. You need a better down-feed. Basic principle is a substantial bracket on the bottom of the quill with some sort of screw thread arrangement to push things down. Time to get creative I'm afraid but its probably best to have a coarse adjustment slide movement which can be locked so the screw thread is only used for fine adjustments. Include suitable reference faces so you can use your digital calliper as a down feed measurement device. Fit a good solid quill lock clamp. Squeeze is probably better than screw in but really the drill layout determines what you can do. What you do to upgrade the bearings is again dependent upon how the drill is designed. Perfection is the ball thrust, needle roller side bearing units made by SKF and others but a pair of those will prolly cost about twice as much as the drill did! If you are lucky simple substitution of good quality bearings for the originals will do the deed. I think the best method is to use a pair of taper roller bearings but these will cost you a bit of quill movement as the relatively large diameter will require a pair of carriers to be pressed on to the quill to hold the outer races. Collars on the spindle will hold the inners in place but you need to make provision to get the end pre-load right. Shims are best but need a few trial assemblies and appropriate comments before you are finished. User strategy is obviously to set the cutting depth, lock everything up and feed across. Apart from getting hold of, or making, suitable feed slides the biggest problem with a converted drill is the difficulty of doing a accurate down-feed cut. Naturally you have the table to quill registration problem endemic to all round column mill-drills to cope with as well. Its a lot more work than it seems at first sight. I converted a BIG power feed drill to a mill for a friend somewhat in this fashion but that has a no 5 morse up the spindle and suitably huge bearings so it was all much easier. HTH. Clive ------- Date: Fri, 2 Apr 2004 15:05:51 -1000 (HST) From: benedictx~xxhawaii.rr.com Subject: CNC Turning Teensy Stuff Had another episode of CNC-mill-as-lathe I thought I'd share: Some really nice folks who are into 1:600 scale ship models approached me about cutting barrels for deck guns so they could make casting masters. I approached the project with all my normal bravado, only to find out I really was in over my head. I posted a picture of the result in my folder in the Photos area. It's a picture of a US dime with five Dahlgren XI barrels and five Brooke 7" double banded barrels. They're pretty small, but held detail ok. Before I get into the trick I used to make them lemme preface it by saying I never did figure out a good way to cross-drill these things for trunnions. For the Dahlgren and the Brooke barrels, the trunnions are on the centerline of the barrel. For some of the other barrels the trunnions are set lower than the centerline. So a simple V-block jig won't answer in all cases. The jury's still out on this. In the mean time the folks making the carriages say they have a way to drill the barrels for trunnions. I take my hat off to 'em. Ideally I'd have made these using a right hand tool and a left hand tool. I'll admit, I'm lazy. I did them using a single tool and setup. The tool needed to have a really fine diamond shape to it (about a 7.5 degree included angle in this case.) It needed to be able to hold an edge throughout several barrels, and it needed to be easy to replace in case I screwed up. The tool was a Stanley box cutter blade with the tip ground down almost 90 degrees to the razor edge. It's about 80 degrees, giving 10 degrees of relief at the tip. The tool is positioned so the ground surface is on centerline with zero rake, just the way brass likes it. Because of the geometry of the razor edge this gives relief at the tip and on both sides of the cutting edge. Just to be clear, it's the flat ground tip that does the cutting, NOT the razor edge. The razor edge is the relieved part of the tip. I wound up rounding off the razor edge a little. Using it straight out of the box and shaving-sharp, it tended to make the part look threaded and not at all smooth. A couple of swipes on a fine bench stone took the edge off without making the rounded part TOO round. I figure the radius is less than a thou. You can't take deep cuts or move too fast, but it worked well for what I needed. Tom P.S. You betcha I wore eye protection! And I positioned things so if anything cut loose the blade flew AWAY from me. Luckily nothing ever cut loose. ------- Date: Sun, 04 Apr 2004 02:02:03 -0000 From: "n2562001" Subject: Re: CNC Turning Teensy Stuff Tom, drilling the trunnion holes should not be a problem. The easiest way would have been to drill the hole in the work stock before turning. You can do this by putting the stock in a mill vise and running a small end mill over the stock so it just touches the top. This will give you a small flat spot top dead center on your stock. From this point you can spot drill with a 000 center drill or a spade drill of the correct size and drill the hole. Since the barrels are cut, if I had to do this I would put the end of the barrels in a ww collet in my Sherline indexer and drill as above. If you do not have a similer method of holding them, I would put the end of the barrels in a GOOD QAULITY pin vise and put it in a regular mill vise. From that point you can center drill and drill as above. I don`t think anyone would ever notice if the trunnions were slightly below center,However if you must you can spot drill with a end mill down to .005". Jerry Kieffer ------- Date: Thu, 03 Jun 2004 18:05:19 -0000 From: "Jim Stoll" Subject: Beginner seeking milling process advice Rank-beginner seeking some fixturing and process advice... I'm cutting a gear out of some plate material (plastic). (I'm doing this on a CNC setup, but I'm guessing that's largely irrelevant to the basics here...) I first need to use a fly cutter to get down to the right thickness (3/16" - the material is about 5/16" thick to start with). Then, I need to cut out the gear, including a decent- sized hole (ie, milled, not drilled) in the middle (this is for a kids toy and will be spinning on a solid axle, so tolerances need not be such that a bearing is press-fit or the like...) and 4 large-ish holes (also milled, not drilled) in a bolt-hole pattern (though not actually for bolting anything to...) First question - how should I go about fly cutting the blank material? Clearly, it needs to be fixed to my table, but my vise is too small to hold it by the edges, and clamps or blocks will clearly be above the top surface, so I can't face the whole thing down to the needed thickness if holding w/ clamps/blocks. (Should I maybe just face it close to the edge, but not all the way? - so that I can clamp it...) Next question - I'll be cutting the gear free of the plate. I plan to use a piece of MDF as a sacrificial surface beneath the plate (as I'll be through-cutting the plastic plate). But, I clearly can't have the work piece flopping about on the table as I complete the contour of the gear... My current plan is to: - start by drilling two holes in the surface of the plate (in the interior of the gear contour and also interior to two of the bolt- hole-pattern holes), and then boltinig the material to the sacrificial MDF surface through these holes - cut the gear contour - cut the center hole - cut the 2 bolt-holes that don't contain the hold-down bolts - pause, clamp the gear down along the outer edge (since I'm done milling out there), remove the two bolts that were holding it down - mill the two remaining bolt-holes (and now the original hold-down bolt holes are gone) Should I also bolt or clamp down the outer material? (ie, the waste which is outside of the gear contour) Any other thoughts, ideas or suggestions? (I'm not particularly attached to the above-described process - its just my initial stab - fire away if you have better ideas!!) Thanks!! Jim -------- Date: Fri, 04 Jun 2004 23:43:51 -0000 From: "Lynn Livingston" Subject: Re: Beginner seeking milling process advice Jim, I just finished machining some aluminum grille mounts for my brother's '56 Chevy Nomad. I faced the same dilemma as far as having to cut the pieces out. Also, I had to flycut the stock down to the planned thickness. However, I couldn't use screws to hold down the grille mounts because they were going to be solid except for some slots. In my case, I just used a piece of stock that would allow me to use clamps around the perimeter. Concerning the pieces that needed to be cut out and considering the stock also needed flycut to thickness, I choose to setup the cutting operation to plunge cut the outside of the parts to within .005" of the stock's thickness as the last cut for each part. When all the parts were made, I flipped them over to flycut the back to within .001" of releasing the parts. I left them this way because the pieces needed to be polished. I then mounted the plates (containing the loosely held parts) to the workbench with doublesided tape and polished them with my hand held buffer. When the finish was done, I simply "pushed" the parts out kinda' like taking model parts off of a sprue tree. It was very easy. I then cleaned the edges with sandpaper and mounted in a small soft jawed vice to further polish the edges with the buffer. It turned out great. Your plan seems to be in order. However, there is a type of clamp you might want to look at that would make your task easier. It's on the Sherline site under the tools and tips section. It is a clamp designed to hold the stock to the table but does not locate above the stock. Therefore, the tool can pass over without interference. I have made a couple of these clamps and use them ever so often. I also find MDF a very good sub-table. I made one like a tooling plate, with 200 threaded holes spaced every 3/8". I bought plastic plug screws from McMaster-Carr to occupy the unused holes to keep swarf out. A trick I learned with the MDF is to spray a couple coats of clear sealer on before you start to use it the first time and whenever you put tool marks in it. It will help seal the surface and keep the oil and such from swelling the surface and the threaded holes. Well, I've rambled enough. Good luck with the project and take care. Lynn Livingston ------- NOTE TO FILE: There is a great deal more information on holding down objects or material for milling in the file "Workholding". ------- Date: Tue, 10 Aug 2004 23:48:07 +0000 From: "steve sc" Subject: Dovetail Advice.... [taigtools group] I want to try my hand at building a fixture with a sliding dovetail. A few questions for the experts: * Looks like it is hard to come by a dovetail cutter with anything less than a 3/8" diameter shank... so I guess I just use a spindle arbor and make a 3/8" mill holder? * Are there any tricks to mill the dovetail slot? Rough out as much as possible with a straight cutter? Do the whole thing with the dovetail cutter? Any tricks/hints appreciated ...I be working in brass and aluminum. TIA Steve ------- Date: Tue, 10 Aug 2004 11:48:47 -1000 (HST) From: benedictx~xxhawaii.rr.com Subject: Re: Dovetail Advice.... Rough out as much as you can with an end mill. Dovetail cutters are fragile so the more wear 'n tear you can spare them, the longer you'll have them in your toolbox. Tom ------- Date: Mon, 16 Aug 2004 16:48:54 -0700 From: Alan Rothenbush Subject: Re: Dovetail Advice.... After breaking two dovetail cutters in short order, I made up my own "dovetail rougher", using a triangular carbide insert. It looks a bit like a flycutter, only instead of a long slot for a toolbit, there is a 60 degree notch milled for the insert. I forget the exact number of the insert, but it is like a TNMG, only with 15 degrees of relief. Once I'd removed 95% of the material with this tool, I switched to the genuine thing for a finish pass. Slow, and LOTS of coolant. Worked great. I think part of the problem is that there is such a big surface speed difference between the top and the bottom of a dovetail cutter. Alan P.S. Here's a few pics of the final product http://www.sfu.ca/~alan/burke/ ------- Date: Tue, 11 Jan 2005 22:07:09 -0000 From: "vibeanders" Subject: Making a cube [sherline group] I am a newbie and a proud owner of a Sherline mill. My first task is making a cube, and I run into some trouble right away. Probably very simple, but I cannot figure it out. I start by cutting a piece of 2" x 2" rod. I assume the 4 sides not cut by the hacksaw are in right angles. But: How do I set everything up to assure, that when I mill the recently cut sides with a fly-cutter, those sides will be in right angle with the other four sides? I have a squared mill vise. The accuracy Iam looking for is a few thou max error on the 2 inches. I hope someone can give me a good procedure, and that you apologize for the newbie level. Btw, I do not have an angle plate, somehow I have a feeling that would have been helpful here, although I cannot really see how there either. Anders ------- Date: Thu, 13 Jan 2005 06:08:48 -0500 From: "Jerry G" Subject: Re: Making a cube Anders, welcome, and here are my suggestions.... By "rod" do you mean round stock? Yes, an angle plate would be very good for this application. I will explain why. You can do it in a vise also. Let's take the vise first, since you have one. First, the basics. Have you "trammed" up the head to the table for perpendicularity? Have you indicated the solid jaw of the vise for the same thing? OK, let's say you have. Put your workpiece in the vise. Now, if the sides you are going to clamp on are not parallel, you will not be able to get where you want. So, when you clamp on the part, put a small rod, or bar across the part,(about 1/8" diameter) a little below the movable jaw side and clamp the part. This will pivot the side of the piece into the solid jaw. But, only in the front to back (Y) direction... But, that might be enough. Take a very light cut with your fly cutter, until you clean up the surface you are cutting... Take the piece out of the vise. Mark the solid jaw side with a "J" , and the cut side with a "1". Check for squareness with a good square. If you had an angle plate and a surface plate and a surface gage, and a dial test indicator, you could test for squareness that way. If it is square, put the piece back in the vise with the cut side ("1" )against the solid jaw. Use the pivot rod again. Cut the next side, mark it "2". Check for square. Cut the last side, which will be "3". You should now have four square sides. Next, the ends... Put the piece in the vise without the pivot rod. Clamp any two milled sides. Use your indicator to align the side (and tap gently to get it there) vertically to the spindle travel. Now, clamp it firmly. Cut the end. Mark it "e". Turn the piece over. Tap the piece down on to a good set of parallels. Cut the second end. You should now have a cube, if you have controlled the amount removed. As far as the angle plate, the advantage is no moveable jaw to throw your piece out of alignment. No pivot rod needed. You just clamp the angle plate on the table, check it for perpendicularity. Clamp your workpiece against the angle plate with two c clamps or toolmaker's clamps. Cut the side with the flycutter. Mark the angle plate side "A" and the cut side "1". Follow the same procedure as with the vise. Regards, Jerry G (Glickstein) ------- Date: Thu, 13 Jan 2005 09:48:28 -0800 From: Alan Marconett Subject: Re: Making a cube Hi Anders, you might want to get a copy of Joe Martin's "Table Top Machining" book, sold by Sherline. [This book has lots of stuff for any small mill.] A little Machinist's square will help you get the sides square to the ways. The fixed jaw is square, but you should use a little packing, like a 1/4" rod between the moveable jaw and the stock, to enable the stock to seat against the fixed jaw squarely. Alan KM6VV ------- Date: Thu, 13 Jan 2005 13:31:23 -0500 From: "Jerry G" Subject: Re: Making a cube The guy that taught it to me was.............ME! That was a time when no one would show anyone anything, for fear of losing their job to a better man...I learned by doing...I learned what did not work. I described the procedure the way I learned it, in regard to a cube, as mentioned by Anders. For a rectangle, I would do the same thing, with one small change. If I could get an end mill long enough to cut the "ends" in the vise and IF the end mill was ground parallel without a back taper, as most of them are. Regards, Jerry G (Glickstein) ------- Date: Thu, 13 Jan 2005 21:03:47 -0500 From: "William Rutiser" Subject: Re: Making a cube Jerry, do you mean that most end mills have a back taper or that most end mills do NOT have a back taper? Thanks Bill ------- Date: Thu, 13 Jan 2005 21:12:42 -0500 From: "Jerry G" Subject: Re: Making a cube Bill, Sorry, I was not clear....In my experience, most of the end mills have a back taper... For example, a 1/2" (.500") diameter end mill usually is .501"-.502" at the end, and a back taper of a few thousandths going towards the shank.... So, any "ends" machined in the vise will be out of square. Regards, Jerry G (Glickstein) P.S. Depending on the accuracy requirement, I used to grind the part all over using a good toolmaker's vise and/ or a angle plate on a surface grinder. ------- Date: Fri, 06 May 2005 15:36:48 -0000 From: "Tom Munroe" Subject: Milling a Flywheel Hi. I was wondering if it would be possible to machine a flywheel instead of turn it on a lathe? I've been looking at a machine that has 11.5 inch flywheels and my lathe is a Heavy Ten with of course a 10 inch swing. I thought it may be possible to use a rotary table and do the machining on my knee milling machine. Any thoughts, maybe just find something smaller? Thanks for any advise folks. Tom Munroe ------- Date: Fri, 6 May 2005 10:51:57 -0500 From: "HLahantubbe" Subject: Re: Milling a Flywheel If you have a rotary table, absolutely you can machine a flywheel. You'll need to balance it or at the very least check it. Your biggest problem will be alignment to insure your bore is coincentric with the outer diameter. With a little care at setup, it shouldn't be a problem. This is done on CNC mills all the time. Use a slow speed and very rigid setup. Rabid Uncle Rabid (http://www.unclerabid.com) We Repair Electronic Speed Controllers For Asian Mini Lathes and Mini Mills ------- Date: Fri, 6 May 2005 12:51:42 -0400 From: "Ken Strauss" Subject: RE: Milling a Flywheel If your table is like mine you could turn a MT2 taper with a spigot on the other end and insert it into a pre-bored shaft hole. Or you could clamp the fly wheel to the table and "bore" the center hole and shape the outside in a single setup. This should ensure that they are concentric. The other possible problem is wobble about the axis of rotation unless you have a rather large (12"?) rotary table. I suspect that supporting the periphery of the fly wheel on a suitably placed blocks would help a lot with this problem. I have successfully used my mill to "turn" a 7" diameter piece of cast iron on a 6" rotary table. My problem was that a cast projection from the base of the circular piece prevented swinging it in my lathe. ------- Date: Fri, 6 May 2005 12:03:04 -0700 From: "Alan Marconett" Subject: RE: Milling a Flywheel Hi Tom, Yes! I've machined a few flywheels on my Sherline mill's rotary table. So the same will be true for you. Making the cutouts for the spokes can be as simple or complex as you like. I enjoy CNC, so I can make my cutouts fairly complex. But just drilling the corner holes of the cutouts, and "milling between the holes" will get you there as well. I can make a bigger flywheel on my mill because all I have to cut is one cutout at a time, and rotate the table to get to all 5 (or 6). The 6" "Baby Beam" flywheel on my webpage was done on the Sherline mill, and the 4" rotary table. http://www.HobbitEngineering.com Alan KM6VV ------- Date: Sun, 12 Jun 2005 18:29:16 -0000 From: "n2562001" Subject: Re: HELP! Need sleeve adaptor for Sherline Motor to Taig's Motor pulley In taigtoolsx~xxyahoogroups.com, "Kenny Wu" wrote: >my Taig... but I need a adaptor sleeve from Sherline Motor to Taig's Motor Pulley and I don;t have a lathe! :-( I'm hoping someone would be nice enough to help me out and make me one. I'll be more than glad to pay for your time and materials. Anyone? :-) BTW, I was considering making the sleeve using my Taig Mill... but I have never been able to sucessfull drill center on a round stock on the Mill before... it's always off by a little and am afraid with the motor's rpm. I'm going to get a lot of vibration. Does anyone know how to make a sleeve (or drill dead center) on a Mill?? < Ken: To accurately machine a sleeve on the mill is actually very simple. First mount the stock in a chuck on the mill spindle. The center hole can be bored by standing a boring tool vertical in the mill vise. The hole will perfectly center itself in the stock. The outside can be machined by mounting a lathe tool vertical in the mill vise and machine the length as you would on a lathe. The end result will be a sleeve as accurate as if it were cut on a lathe. Jerry Kieffer ------- Date: Sun, 12 Jun 2005 12:16:34 -0700 From: "Kenny Wu" Subject: RE: Re: HELP! Need sleeve adaptor for Sherline Motor to Taig's Motor pulley Jerry, Rick is already making me a sleeve...but your recommendation interests me. I understand what you are saying is to turn a mill into a lathe... except vertically. but without a tail stock perfectly aligned and/or a live center (like ones on the lathe), how will you find center? It seems if you put a drill or end mill of any kind in a vise and lower Z (with the stock) to mate with the tool, this still may not find center because you might end up missing center and start cutting a hole larger than the diameter of the tool (although the hole should be perfectly rounded... humm). What kind of a "boring tool" are you refering to? It has been at least 15 years since I stood in front of a lathe in metal shop back in college... if memory serves, on a lathe, the tail stock is always perfectly aligned center of the spindle and all one needs to do to find center is to use a live center or... put a drill in the tail stock. Correct me if I'm wrong here... it has been quite a while and I didn't spent that much time on any machines when I did. Thanks! Ken ------- Date: Sun, 12 Jun 2005 20:51:41 -0000 From: "n2562001" Subject: Re: HELP! Need sleeve adaptor for Sherline Motor to Taig's Motor pulley Ken: Actually a mill is a lathe depending on how you look at it. A boring tool is generally used in a lathe to remove metal from the inside of a hole in the same manner you remove metal from the outside of stock. The tool is held in the tool post and for this project a tailstock would not have been used. Drilling a hole for a pulley sleeve would generally not be accurate enough. By machining (boring) the hole it will be straight, round, and accurately sized. Take a look at boring tools in a catalog and I think you will see how they work. The mill vise will serve the same purpose and position as a tool holder on a lathe. If you look at the mill at the right angle. An accurate tailstock for a mill is easily made by locking the ways and drilling a hole in stock held in a vise if needed. A drill could then be held with a predrilled setscrew in that stock. Many people have used large mills as lathes, or lathes as mills, until they could afford both. Almost all machining operations can be done on either a lathe or mill if that machine is properly utilized. If by chance this is still unclear you may contact me off line and I will send you a drawing. Jerry Kieffer ------- Date: Sun, 12 Jun 2005 21:28:30 -0000 From: "Jim Knighton" Subject: Re: HELP! Need sleeve adaptor for Sherline Motor to Taig's Motor pulley Ken, my comments here are probably unneccessary, but Jerry is absolutely right. I used my Jet mill/drill as a vertical lathe in the manner he suggests until I could afford a more traditional machine. It worked reasonably well and was adequate for the kind of projects I was doing back then. In addition, I recall an article from either HSM or its companion publication about a guy who took great pride in the fact that he didn't have a lathe, didn't know how to use one, and didn't want one. He did all his turning on his mill/drill, again in the manner Jerry suggests. As an aside, one of the more obscure cutting tools is a "left handed boring bar". It can be used with a standard boring head on a mill to machine the OD of a spindle, boss, hub or other round feature. I have one of these in the drawer for this kind of setup. It doesn't see a lot of use, but that isn't the point. There are times when only something really strange like this will get the job done. You might have to do some searching, but MSC has them in their catalog. Mine has a 1/2" shank and is solid carbide. Regards, Jim ------- NOTE TO FILE: There is a conversation, Subject: Tooling Marks [taigtools], starting 05 Aug 2005 that is found here in the Finish and Polish file. Part way through the discussion, the thread switched to buffing and polishing tips. This thread will be of interest to anyone trying to reduce or remove tooling marks, whether caused during milling, turning, or whatever. Good machining tips are included. ------- Date: Sat, 13 Aug 2005 23:50:50 +0100 From: Steve Blackmore Subject: Re: Re: Milling mild steel & tool life [taigtools] On Sat, 13 Aug 2005 18:29:45 -0000, you wrote: > There is one big difference, the new endmills were all 2 flute. > Carbide, like before. 2 flute are slot drills, not end mills - Are you cutting a slot or using them for general side/facing operations? If the latter they will snap. For general milling use HSS 4 flute. Lack of rigidity, run out and thermal shock will all snap small carbide mills too easily, don't use them unless you have to. When side or facing, use a 4 flute with feed movement opposite to tool rotation. (Conventional milling) The other way, (Climb milling) with feed movement and tool rotation in same direction, is great on a rigid machine with no backlash, it should generally be avoided on a Taig. Any backlash and the tool gets tugged into the work and with very small bits they snap. Steve Blackmore ------- Date: Sun, 14 Aug 2005 13:42:58 -0000 From: "jensen_remote" Subject: Re: Milling mild steel & tool life I'm using them for slot cutting, not side/facing. They snap anyway :) They are listed in catalogs, like Enco, as 2-flute endmills. I'll call them slot drills if you like; I'm curious why anybody bothers with 2-fluted slot drills when 4-fluted endmills (center cutting) are the same or nearly the same price, and seem to work better. What am I missing here? Any good sources for low cost, 4 flute HSS endmills? Cheers, Peter ------- Date: Sun, 14 Aug 2005 14:42:01 -0000 From: "Gordon Reithmeier" Subject: RE: Milling mild steel and tool life Perhaps you would have more success by switching to a "free machining" steel. Ordinary cold rolled steel sold in North America (1018) is not suitable for machining especially with light equipment. This is just a suggestion. Gordon ------- Date: Sun, 14 Aug 2005 14:49:31 -0000 From: "Lynn Livingston" Subject: Re: Milling mild steel & tool life > Any good sources for low cost, 4 flute HSS endmills? Peter, I've used these folks a few times: http://www.discount-tools.com/hssemindexmain1.htm I've been quite please with the products, price seems good also. I've been trying to come up with a reason you are having problems breaking endmills while cutting mild steel, and I guess I'm not experienced enough to get it. One thing you could check though is belt slippage. It's just grasping for straws in any case, but if your belt WAS slipping, it would slow the bit down and bog the cut. This would feed on itself and would cause a snapped bit. Also, excessive runout could cause the same sort of scenario I suppose. I just remembered you said you are using a different collet than stock; better check that the collet and/or spindle is not slipping also. The spindle could slip in the pulley; are you hearing any unusual sounds while machining? Something somewhere is limiting the endmill's ability to cut, which ends up causing enough flex or bind to break it. Or rather, that's the only scenario I can think of. Also, have you trammed the mill lately? It might be prudent just to give a cursory check to make sure the table and column or square to each other. What exactly do you hear, or sense, at the point the endmill are snapping? Is the motor bogging, or the tool making more noise? Surely, there is a clue somewhere we can work with. I'm sure there are a lot of folks watching this thread, trying to visualize what's going on. But, a lot of us have cut mild steel exactly like you are with good results, so we are kinda' baffled here. Keep throwing out clues you come across, and somebody will figure it out I'd bet. Lynn -------- Date: Sun, 14 Aug 2005 15:06:09 -0000 From: "Lynn Livingston" Subject: Re: Milling mild steel and tool life > Perhaps you would have more success by switching to a "free > machining" steel. This is a good suggestion. While I have machined 1018 successfully on the Taig, I was sure suprised when I got hold of some 12L14, like the Taig blank spindle arbors are made from. It does machine much easier. However, it doesn't seem to come in all the shapes and sizes that hot or cold rolled does, or maybe I'm not looking in the right places. I've even machined 303 stainless (because I had a piece) on the Taig lathe and mill, and with patience and conservative machining, it went alright albeit slow. I've recently got hold of some titanium, and would sure like to make a pen body out of it. I've been putting it off, but do plan to try and machine it some day. I will try and find some material to "read up" on the nature of machining ti before I do though. Polished ti sure looks nice! Lynn ------- Date: Sun, 14 Aug 2005 16:24:01 +0100 From: Steve Blackmore Subject: Re: Re: Milling mild steel & tool life >I'm curious why anybody bothers with 2-fluted slot drills >when 4-fluted endmills (center cutting) are the same or nearly the >same price, and seem to work better. What am I missing here? A 1/8th 2 flute slot drill will cut a 1/8th slot (near enough), a 4 flute 1/8th mill will cut an oversize slot ;) A 2 flute cutter bites into both walls at the same time and, when cutting to the front, cannot cut the sides. A 4 flute end mill will cut both the front and sides at the same time and the front cut will cause the cutter to flex, varying the depth of the side cuts making the finish rougher and the slot wider. > Any good sources for low cost, 4 flute HSS endmills? In the UK J&L, Chronos, RDG - there's also always plenty off mills on ebay. I got 4 slot drills and 4 end mills in the following sizes 1/8, 3/32 & 1/4 a few weeks ago, brand new, Osborne for £14 . Steve Blackmore ------- Date: Sat, 17 Sep 2005 10:24:01 -1000 (HST) From: benedict-listx~xxhawaii.rr.com Subject: Re: Router OR Spindle?? [taigtools] On Sat, 17 Sep 2005, victorf57 wrote: > I'm in the process of building a gantry style machine, It is all > aluminum construction with frelon linear bearings and shafting. Here is > the problem and I'm hoping some of you can help. I have also posted on > another group, so sorry if some of you have seen this :-). > I would like to use the machine for cutting plastics such as PVC and > aluminum. My problem is the spindle, do I use a router?? some have > suggested some such as Makita for noise and porter cable for power. but > now I'm thinking taig spindle!!! have any of you done this??? I haven't done that, but I do have a Taig spindle on my Taig. ;) > Do any of you have any Idea how the taig spindle would stack up against > a 21/2 hp router on depth of cut?? Depends on what you're cutting and what size motor you've got on it. But more than that the geometry of your machine will determine whether it'll work or not. Unless you're building a seriously beefy machine, the forces involved in cutting aluminum can cause vibration and flexure issues. I'm guessing that's going to limit you more than the spindle, regardless of whether you use a router or a Taig spindle. > how deep of cut can the taig take in 6061 alum with a 3/8 mill??? now > the other factor is does anyone know how much the taig head weighs with > the motor?? the reason I ask about the weight is I plan on using a > stepper motor to drive it . and I know a good router weighs 8 to 10 LBS > also taig has 2 spindles the normal which costs $65.00 and the ER- > $106.00 have any of you found a way to run 3/8 end mills on the standard > spindle?? I can use 3/8" mills on my standard Taig headstock using an end mill holder I made from a blank arbor. Holding tools that size is no problem. If you put a big enough motor on the headstock, it'll drive a 3/8" mill plenty deep in aluminum. I haven't been able to find out just how deep because the rigidity of the machine causes problems before the spindle will stall. This is using a 1-1/2 HP VDC treadmill motor. I've got the speed controller limiting it to about 1HP, so figure that's all I'm getting at the absolute most. I'm guessing it's less than that. Most of the parts I make are dimensionally critical, so I'd rather shallow up my cut or slow down the feed rate than have things get thrown off to one side by the cutting forces. Sorry I can't answer that question any better. One huge difference between a router and the Taig spindle is the speed. For plastic, you could probably use a router. For aluminum I wouldn't want to, especially if you're looking at 3/8" end mills. Metalworking typically requires spindle speeds much slower than woodworking. Routers are fantastic spindles for working wood and some plastics (though heating and melting of the material can cause serious problems), and for using smaller cutters where the higher spindle speeds are a benefit. But for metalworking they're a little fast. With a treadmill motor, the spindle and motor combo probably weighs as much as a good router. It's hefty. One solution would be to pick up a gas spring or a constant force spring to balance out the weight of the head. It helps to have a little downforce on the Z axis, but you can cut it by a lot and take a bunch of the load off the Z axis motor, leadscrew, and nut. > Sorry for all the questions No sweat. It's what the group's for. Tom ------- Help with pocket cutting on 2mm (80 thou) Aluminium sheet [sherline] Posted by: "Andrew Wells" nz120x~xxxtra.co.nz Date: Tue Jul 4, 2006 12:38 pm (PDT) Hi. I'm trying to cut out a simple shape in 2mm aluminium sheet. It is basically a 3.5" x 2" rectangle, with a concentric 1.5" by 1" approx cutout. The problem that I am having is that when I try to mill out with a 1/8" cutter, the aluminium "pushes" away from the tool, so even when the tool gets to a theoretical depth of 90 thou (after stepping down at 15 thou intervals), it still has not cut through the sheet because the sheet has created a raised line the shape of the cutting path on the underside of the sheet. I have tried both clamping the sheet down to a piece of hardboard, and having it open underneath (i.e. supported at the edges only), and I get the same result. I haven't tried plunging the cutter through the whole depth (or using a pilot drill hole) and cutting around in one pass, but I guess I would have to run a low feed speed for this? Any suggestions gratefully received. Thanks & Rgds Andrew Wells BTW - I am using Turbocnc/HobbyCNC setup on a Sherline 8 Way Mill. ------- Re: Help with pocket cutting on 2mm (80 thou) Aluminium sheet Posted by: "Keith Green" ksggx~xxtelus.net Date: Tue Jul 4, 2006 1:38 pm (PDT) You can still do it with your light cuts. Drill a hole, as you suggest, but do it near one edge (not at the edge). Plunge into the precut space and do an arc move out to the edge of your pocket. When you get back to the start point, make sure there is a tiny overlap in the cut (maybe .01) and make an arc move back off the profile. Raise the cutter up above the part (safety) and move to the center of the hole and plunge again. A light cleanup pass at full depth will give a great finish. You could leave a space under the part but I might tend to leave solid hardboard under there to support the thin material you're using. Make sure your speed is very high throughout and that your finish pass (at least) goes CCW around the profile. Keith ------- Re: Help with pocket cutting on 2mm (80 thou) Aluminium sheet Posted by: "Alan Marconett" KM6VVx~xxarrl.net Date: Tue Jul 4, 2006 3:20 pm (PDT) Hi Andrew: Use sacrificial stock, and and allow the final cut or two (go past your depth) to cut into the sacrificial stock? I've observed what you're describing. Just cut past it, and use a fine file to clean off the edge if needed. Alan KM6VV ------- Re: Help with pocket cutting on 2mm (80 thou) Aluminium sheet Posted by: "n2562001" jlkiefferx~xxcharter.net Date: Tue Jul 4, 2006 6:31 pm (PDT) Andrew: You should be able to cut .080" aluminum at full depth with a 1/8" endmill at high speed using cutting fluid (WD-40 works well for Aluminum) almost like cutting butter. That is if you're using a sharp, quality end mill. The problem that you have described is very common with dull/overheated or poor quality endmills from Asia/India. Jerry Kieffer ------- Re: a really dum question........about drilling holes Posted by: "leasingham_connelly" martin.connellyx~xxsiemens.com Date: Mon Aug 14, 2006 12:38 am (PDT) In LittleEngines, "ky1duck" wrote: > i have a really dumb question about drilling holes where i want them. > first the machine is a HF mini-mill, have tried from the cheap bits > to good (not great) drill bits. no name, dewalt, bouch. but the > problem is every time i try to drill a hole it never seems to be in > the right place, tried gluing copies of the drawing to the part, even > center punched and tried; still the same problem. even all the way down > to a 1/16" bit. any ideas on what i might be doing wrong. rob Do you have backlash in the table? If there is backlash and the ways are too loose then the first contact of the drill on the workpiece can move the table under the bit; lock the ways before cutting as well. If the ways are tight then the other important point is to always move to the required place from the same direction so that backlash can be ignored. For x axis travel pick your preference, such as always moving from right to left, and get in the habit of always doing it that way. If you overshoot the required point, move back more than the backlash and approach from the chosen direction again. The same process should be used for y axis travel. I have a DRO on my mill and still do it this way through habit. Martin ------- Squaring up a piece of stock [atlas_craftsman] Posted by: "buzzurd00" buzzurd00x~xxyahoo.com Date: Thu Jan 18, 2007 4:45 pm ((PST)) How can you take a piece of stock with 2 opposite side uneven back to being parallel with each other? I'm attempting this on a mill with a vise that I know is in tram with the spindle. There is probably a simple answer but I've been out in the shop and for some reason just keep banging my head against the wall. Thanks, Buzzurd ------- Re: Squaring up a piece of stock Posted by: "r_corriveau" r_corriveaux~xxyahoo.com Date: Thu Jan 18, 2007 5:31 pm ((PST)) Sit the good side of your block down on parallels, as high a possible, in your vice. Mill the top surface parallel. Now you have 2 sides parallel. If you want to continue to square the block, push a good side up against the rear jaw, and use a bar or cylinder between the moving jaw and block. This makes sure you are up square against the back. now mill the top. and so on and so forth.... ------- Re: Squaring up a piece of stock Posted by: "Ian Sabey" ianx~xxsabey.uklinux.net Date: Fri Jan 19, 2007 3:15 am ((PST)) Just my £0.02 If the bottom of your milling vice is not true I'd be inclined to mill it flat. If it's too hard to mill, then pack it up with shims until it's flat. Use a dial gauge mounted on the spindle to tell you when it's flat. HTH Ian. ------- Re: Squaring up a piece of stock Posted by: "buzzurd00" buzzurd00x~xxyahoo.com Date: Fri Jan 19, 2007 1:40 am ((PST)) Problem is I don't have a good side. ------- Re: Squaring up a piece of stock Posted by: "Bill Lee" Billx~xxWRLee.com Date: Fri Jan 19, 2007 4:48 am ((PST)) No sides square/flat: Grab the piece as best as you can in the vice, positioning it as close to "flat as possible (by eye is good enough). Take a light cut on the top until you have a flat surface. Now you have one "good side". Then turn it over in the vice and use some parallels or the bottom of the vice with the newly flattened surface down, and then mill the top surface flat. Now you have two parallel flat surfaces on your piece. Bill Lee ------- Re: Squaring up a piece of stock Posted by: "Mario L Vitale" mariol.vitalex~xxatt.net Date: Fri Jan 19, 2007 5:24 am ((PST)) One little addition ... When you place the block in the vice to machine the second side you must be sure that the fixed jaw is, in fact square with the bottom of the vise (ususally not a problem) but also when you tighten the moveable jaw, make sure it does not "lift" the part. One approach to minimize this is to put a piece of round stock, horizontally, between the block and the moveable jaw so you only have line contact and the jaw can pivot allowing the block to remain in contact with the fixed jaw. Even better is to use a good sized steel ball (1/2" -3/4" dia) so you only have a point contact. Good luck, Mario ------- Re: Squaring up a piece of stock Posted by: "Jon Elson" elsonx~xxpico-systems.com Date: Fri Jan 19, 2007 9:48 am ((PST)) In atlas_craftsmanx~xxyahoogroups.com, "r_corriveau" wrote: >Sit the good side of your block down on parallels, as high as >possible, buzzurd00 wrote: >Problem is I don't have a good side. Well, then it doesn't matter. Take the most flat side, and put it on parallels or a spacer block of some sort that puts it nearly level across the vise ways. Mill the top flat, and flip over and repeat. You should now have two sides that are as close to parallel as the vise's ways are to its base. If this is not reasonably true, then you'll never be able to make a true rectangle. Once you have two sides parallel, you turn one of them against the fixed jaw and do it again. It may be necessary to use pins, wood blocks, etc. so that closing the vise's jaws don't tilt the piece away from the parallels and/or the fixed jaw. You should now have something that is a pretty good rectangle in one cross-section. You can slide the block to one end of the vise, so part of it is sticking out past the jaws, and side-mill that end. Now, you have 5 orthogonal faces. Turn it 90 degrees so it is resting on that last end, and face the top to do the 6th side. If this is not practical, you can use a machinist's square to set the piece with the unfinished end up while the sides not gripped by the jaws are held square to the base. Jon ------- Re: Squaring up a piece of stock Posted by: "jmartin957x~xxaol.com" Date: Fri Jan 19, 2007 6:28 am ((PST)) Just keep in mind that this is an Atlas group. The methods suggested are good, but may not be appropriate if the user is doing it on an Atlas mill. Yes, you can do it exactly that way with a wide slabbing cutter, with multiple passes with a plain cutter, or, for a small workpiece, with the side of a long heavy end mill. But he is more likely to be using the end of an end mill, a face mill, or a flycutter. With those, on a horizontal mill, the procedure will be a bit different. Probably the nicest feature of the horizontal - other than its rigidity and the ability to remove metal very quickly - is that, once you have a flat surface, you can clamp that surface directly to the table and accurately mill an adjoining surface at a perfect right angle with an end mill, face mill or flycutter. Cutting a parallel surface - unless you are using a slabbing cutter, etc. - will require setting the workpiece up on a right angle plate. My horizontal mill is a lot heavier than an Atlas, but when I need a parallel surface I'll usually find myself turning instead to the shaper or surface grinder. One place the horizontal really shines is in squaring up a large plate - say an 10" x 12" x 1". Pretty tough to mill a 1" edge with the side of an end mill, and you may not be able to get 12" on edge under your vertical mill. On a horizontal, though, it's a piece of cake. If I had to make a guess, I'd guess that, while some members of the group have Atlas lathes, mills and shapers, most are like me and have just one Atlas machine - a lathe. If they have a mill, it's likely to be a non-Atlas vertical. Shaper doesn't really matter, because, Atlas or non-Atlas, they all work pretty much the same. The original poster might get an even better answer if he mentions what size workpiece he is thinking of, and what equipment and tooling he has available. Otherwise, we're assuming what he needs and has available, and he's assuming our answers will apply to him. You know what happens when you assume... John Martin Cumberland, Maine ------- End Milling : maximum depth [sherline] Posted by: "jcbrooks75" jcbrooks75x~xxyahoo.com Date: Sat Mar 31, 2007 3:29 pm ((PDT)) I'm new to machining and could use some help. I am using the double sided end mills that sherline provides. I would like to remove some material from an existing part. The layout of the part does not allow me to mill perpindicular to the face. I think I can remove the material by running the end mill parallel to the face. How far can I plunge the 3/8" end mill? How far can I plunge the other end mills before the side cutter is rendered ineffective? I'm not looking for the maximum depth per pass, but the maximum allowed distance the end mill can intrude into the part. Thanks, Jon ------- Re: End Milling : maximum depth / Length of Cut Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Sat Mar 31, 2007 4:09 pm ((PDT)) Hi Jon: Usually, all end mills have a LOC* * = Length Of Cut This just tells you effective length of the end mill teeth. Plunging is not recommended unless you first relieve the center where you want to plunge. Even so called "end cutting end mills" have a "dead spot" or web where the teeth on the end meet in the center of the cutter/end mill. Later, Jerry G (Glickstein) ------- Re: End Milling : maximum depth / Length of Cut Posted by: "Keith Green" ksggx~xxtelus.net Date: Sat Mar 31, 2007 6:47 pm ((PDT)) I would have to take slight exception to that, Jerry. Slot-drills and center-cutting endmills have one flute ground off-center so that it cleans up the little nub normally left at the center. About the only thing they will leave is a slightly conical bottom at the bottom of a hole which is simply plunged; the end of the cutter has a slight angle on the lips so that the periphery touches the work first. Keith ------- Re: End Milling : maximum depth / Length of Cut Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Sat Mar 31, 2007 11:50 pm ((PDT)) Hi Keith: Yes, what you say is true, but you plunge a nominal end mill (of any size) without relieving the center first, and you will find an oversize and usually eccentric hole/bore as a result. Even if locked, the table tends to pull under the machining stresses. It is good machine shop/toolroom practice to do as I said. If I need a really flat bottom hole/bore, I bore through and then press fit a plug that is really flat. By facing or grinding. Later, Jerry G (Glickstein) ------- Re: End Milling : maximum depth / Length of Cut Posted by: "Keith Green" ksggx~xxtelus.net Date: Sun Apr 1, 2007 11:13 am ((PDT)) I agree; if plunging I drill a hole at the plunge point if that is practical. In the case of a blind slots and keyways I just plunge them though. That being said, a Sherline probably won't be able to plunge much more than an 1/8" cutter without an unacceptable amount of 'walk'. I'm used to much bigger machines I'm afraid. Keith ------- Re: End Milling : maximum depth Posted by: "Michael" kbuiltx~xxverizon.net Date: Sat Mar 31, 2007 6:49 pm ((PDT)) Jon: First of all welcome to the group. To give you an example, with a 3/8" endmill, the length of cut (LOC) options are 1", 1.25", 2" and 3". Remember what JerryG said about relieving the center first. Michael ------- Re: End Milling : maximum depth Posted by: "Alan Haisley" alanhyx~xxadelphia.net Date: Sun Apr 1, 2007 9:49 am ((PDT)) Michael & Jon: The Sherline supplied 3/8" endmill has nowhere near 1" LOC. I believe that it is actually 9/16". Alan Haisley -------- Re: End Milling : maximum depth Posted by: "Tom Bank" trbankx~xxpaonline.com Date: Sun Apr 1, 2007 2:01 pm ((PDT)) As Michael (kbuiltx~xxverizon.net) wrote, end mills of 3/8" diameter come in 1", 1.25", 2" and 3" lengths and are available from various sources. Depending on where you are at, you pick the the source that suits you. My preference is MSC, which has shipping points scattered around the U.S. and one of them is within driving distance of me (in Central Pennsylvania). MSC has a really huge catalog, which they will be glad to send you if you call them at (800) 645-7270. Also ask that you be put on the mailing list for their monthly flyer. They have some very good deals on special purchases, manufacturer overstocks, and the last of discontinued items. I picked up some steel ground flat stock that was listed as "Made in U.S.A." It turned out to be overstock made by Starrett. Now, to the point of what you ask, you can side mill for the whole length of the the cutting part of an end mill, but it is best to leave a little room at the top so you don't run out of cutting edges. Assuming that you buy new U.S.A. made end mills, the cut will be straight. However, be aware that end mills are tapered. The end of the cutter has a slightly smaller diameter than the part up by the shank. If you need a "perfectly square" corner between the side and the top or bottom, you would need to measure the taper of the mill and accommodate it with a shim under the edge of the work piece. Another thing to be aware of is that end mills are made up to 1/2" in diameter with a 3/8" shank and, just to complicate things further, there are end mills made specifically for cutting aluminum. I have two 1/2" -- 3/8" shank end mills with 1" length of cut (LOC), one for steel and the other for aluminum. The advantage that these mills have is that I can make a second set of cuts, one below the other, and not rub the shank of the end mill against the first cut, which would prevent cutting a smooth side. The disadvantage is that if I come to an inboard corner, it will have a 1/4" radius. Another thing to watch when using an end mill is that you set the set screw in the recess which is cut into the shank and then, before tightening the screw, pull down on the end mill so the tightened screw seats at the top of that recess. The cutting action of the spiral flutes pulls down on on the end mill and will cause the mill to drift lower and lower as your side cut progresses if the mill is not down as far as it will go in the recess before you start. I spoiled several parts before that was explained to me. Finally, since you are new to machining, may I suggest that if you have -- or have access to a high speed cable or DSL connection to the Internet (unlike my 56K Baud modem) you can go to YouTube.com, then do a search for "Sherline lathe mill" and then select the video clips submitted by "gmark". He has a number of clips with various projects that he makes while you watch him. A lot of beginners question how fast the Sherline equipment should be run when performing various cuts. Quoting speeds is not nearly as effective or reassuring as watching a video and listening to the sound of the motor as the operator does this and that. ...And, of course, the things gmark makes will give you ideas for future projects of your own. Regards, Tom Bank ------- Re: End Milling : maximum depth Posted by: "Michael" kbuiltx~xxverizon.net Date: Sun Apr 1, 2007 2:33 pm ((PDT)) Tom, I just checked out youtube again for the hundredth time myself and found a video from gmark that I had missed. The video is the cross slide accessory block for the lathe. There is a part in there where he used a woodworking router bit to do the grooving. Is this normal practice for material like brass and aluminum? I would naturally assume these would be the only material candidates for using router bits, being they are the softer metals. Just wondering is all. Michael ------- Re: End Milling : maximum depth Posted by: "Tom Bank" trbankx~xxpaonline.com Date: Mon Apr 2, 2007 7:19 am ((PDT)) Michael: Yah, I downloaded that one and have a block of aluminum to cut up to make one of those blocks. Answer to your question: D*** if I know! He seems to have done it successfully. Don't know whether the router bit will cut wood after being mistreated thusly. I remember "Doc" LaFever, my Junior High woodshop teacher (so nicknamed because he resembled the character in Disney's Snow White) being rather emphatic about never using woodworking tools on metal and vice versa. Reminds me of the old story about the Cornish miner with his buddy in the front row at church on Easter morning when the spinster in the balcony fainted while singing a hymn. She pitched over the rail, but miraculously her laced up shoe was caught by an ornamental spike on the chandelier, suspending her upside down. The rector quickly held up his hand and shouted, "Anyone who looks will be stricken blind!" The miner leaned over to his buddy and whispered, "By gore, I think I'll risk one eye on it." I checked. I have an old HSS router bit I think I'll risk on it! Regards, Tom Bank ------- Re: End Milling : maximum depth Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Mon Apr 2, 2007 7:41 am ((PDT)) Funny Story, Tom, Let us know how it works....I have a number of router bits.....Logically, to me there must be a reason why they are designated router bits....I believe the RPM's are in the 35,000 range. I have a couple of great routers from Bosch. I used them to make display cases for my ship models using Acrylics. And oak for the grooving of the framing. Later, Jerry G (Glickstein) ------- Re: End Milling : maximum depth Posted by: "Steve Boylan" boylanx~xxworld.std.com Date: Mon Apr 2, 2007 8:07 am ((PDT)) What, nobody else works with both wood and metal? Woodworking router bits generally have aggressive rake angles and deep flutes to clear big chips of soft material (compared to steel, white oak is a soft material). They are also designed to run at high speeds. They're doing basically the same job as milling cutters, with the geometry adapted to the needs of a different material. Solid carbide router bits tend to be fairly brittle, which is not a problem in wood but I'd say it's risky in metals. High speed steel bits are made from the same stuff as milling cutters and drill bits. If you can control the feed and speed, they ought to cut brass and aluminum. I'd just be wary of the steep angle - I expect a router bit would tend to bite too deep into the metal and grab. Clamp the material as tight as you can, or back it up with something that will keep it from moving, and try light cuts to see how it works. Most "form" cutters are carbide brazed to a steel body. I could be tempted to try using one on aluminum or brass, but very, very carefully. I've had one send a tooth flying, apparently from a defective braze. Happily, it hit the wall instead of me. Steve ------- Re: End Milling : maximum depth Posted by: "David Clark" dcclark111x~xxcomcast.net Date: Mon Apr 2, 2007 9:10 am ((PDT)) A short while ago there was a discussion in the mlhorology group on using a router on brass. Go to that group and look for the thread "routing clock plates" for some interesting information. DC ------- Endmill choice: size [sherline] Posted by: "Charles Fox" cafox513x~xxgte.net Date: Mon May 21, 2007 6:17 pm ((PDT)) What's a good principle for choosing endmill size? Specifically, I'm looking at a workpiece that is .500" wide, 4.000" long. I just want to mill .050 off the top, flat. I could use my largest endmill, 3/8" and have significant overlap on the two strokes. Or I could take the next smaller, 5/16" and have either next to no overlap . . . or I could take three passes. I know not why, but I'm leaning toward three passes with the smaller one. Maybe because it seems this will put less strain on the workpiece, setup and endmill because it's cutting (admittedly on a little) less material. Does that make any sense? Or should I know another of The Secrets of Machining that hasn't been downloaded to me yet? This could be considered idle curiosity unless there is some important consideration I'm missing. As always, my thanks ------- Re: Endmill choice: size Posted by: "Keith Green" ksggx~xxtelus.net Date: Mon May 21, 2007 7:59 pm ((PDT)) I use the biggest one I can. Run it so the overlap is down the middle more or less and it'll still look good. Keith ------- Re: [MEworkshop] Endmill choice: size Posted by: "Charles Fox" cafox513x~xxgte.net Date: Mon May 21, 2007 6:56 pm ((PDT)) Jerry G (Glickstein) wrote: > 'Twere me, I would use a flycutter. Endmills are handy. Flycutter is packed away. And the question still stands, because I used the endmills so much more often. ------- Re: [MEworkshop] Endmill choice: size Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Mon May 21, 2007 7:20 pm ((PDT)) In that event, use the 3/8". Cut in on all edges so there is little or no burr. Jerry G (Glickstein) ------- Re: [MEworkshop] Endmill choice: size Posted by: "Charles Fox" cafox513x~xxgte.net Date: Mon May 21, 2007 8:27 pm ((PDT)) Hah! So I used the 5/16", and had to work at it to get it looking good. More questioning . . . I was taking bites of 10 thousandths. I have the (cast aluminum, rought exterior) workpiece on parallels in the vise. Could taking that much actually move the workpiece? I swear it wasn't cutting evenly throughout the pass. The ends -- hanging out, unsupported, over the sides of the vise -- made more noise. But at one point the endmill seemed to dig in harder. I doubt the endmill was slipping, so figure maybe there was the tiniest slip twixt vise and workpiece. At any rate, I stopped taking .010 and did the last two passes at .005. That seemed to make everything copacetic. PS Next time I'll probably use the flycutter. But I figure, if I don't understand what endmills do, I ain't gonna understanding milling. Luckily, I have fat on this piece and sneak up on final dimensions, all the while learning. ------- Re: [MEworkshop] Endmill choice: size Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Mon May 21, 2007 8:51 pm ((PDT)) When you put the workpiece in the vise, did you tap it down and try to move the parallels to insure the part was sitting down on the parallels? SOP in parts in the vise. If the part does not have at least one square edge, preferably the one against the solid jaw, the part will never sit down properly. BTW, end mills work on the sides too! Now, to dress up the surface after overlapping cuts.....Take a piece of 3M wetordry Silicon Carbide abrasive paper. Grit # 240 or # 320. Doubleside tape it to a flat surface, glass plate, etc. Don't use your surface plate. Deburr the edges of the .500" by 4.00" with a small fine file, and then pass it over the abrasive paper in a figure eight pattern so as not to dub the edges. Try to keep an even pressure on the part. Once in a while, check the surface until the tool marks from the end mill are blended in. (See Keith Green's message) Jerry G (Glickstein) ------- Re: [MEworkshop] Endmill choice: size Posted by: "Charles Fox" cafox513x~xxgte.net Date: Mon May 21, 2007 10:14 pm ((PDT)) > did you tap it down and try to move the parallels to insure the part > was sitting down on the parallels? I did indeed. And it wasn't easy. The top and bottom were very close to parallel (out maybe .001" in four inch length, same side to side). There are two somewhat (!) parallel flat surfaces on each side. I don't think they're exactly flat or exactly parallel, but they're cast and supposed to stay that way, so they will. Seemed to fit in tightly and well, though. I couldn't rock anything by hand. And the parallels remained locked in. Couldn't move them still, even after all the machining was done. Will do! I already tickled both top and bottom with a flat file, and that helped already. Will use wetordry tomorrow. ------- Re: Endmill choice: size Posted by: "Peter Harrison" peter.harrisonx~xxhelicron.net Date: Tue May 22, 2007 9:46 am ((PDT)) Suppose your mill head is 1 degree off vertical in the direction of the length of the piece. (I expect it is much better than that but bear with me.) Next, suppose you have a 1 inch cutter - end mill or flycutter diameter - whatever. Now the cutter will cut shallow grooves with the deepest part 0.5*sin(1) deeper than the edges. That is nearly 0.009 inches. With the same geometry, use a 3/8 end mill. Now the groove will be only (3/16)*sin(1) = 0.003 deep - a significant improvement. This illustrates the importance of making sure the head is properly aligned and that, in general, for any amount of misalignment, several passes with a small cutter will give a flatter surface. If the misalignment is at right angles to the direction of cut, double the numbers. Pete Harrison ------- Re: Endmill choice: size Posted by: "Alan Haisley" alanhyx~xxadelphia.net Date: Tue May 22, 2007 8:29 pm ((PDT)) Charles Fox wrote: > What's a good principle for choosing endmill size? Charles: It may depend on your goals. I was milling parts for a small steam engine and decided that the repeated pattern made by the end of the mill was attractive, so I used a smaller cutter and a lot of passes. If, as Jerry suggests, you want a near mirror finish with no tool marks, you probably want either a big mill or a fly cutter - after carefully tramming the machine. If you like the appearance of the tool marks, try a small cutter with lots of passes. Alan ------- Re: Endmill choice: size Posted by: "Peter Harrison" peter.harrisonx~xxhelicron.net Date: Wed May 23, 2007 12:06 am ((PDT)) > If you like the appearance of the tool marks, try > a small cutter with lots of passes. One sign of a well set up machine is the cutter marks. If all you see are curves in the same direction, ((((((, the head is inclined in the direction of travel. With the head perfectly perpendicular you are likely to see trailing edge marks like those in this page: http://www.scottycameron.com/articles/details.asp?id=86 Pete Harrison ------- Re: Endmill choice: size Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Wed May 23, 2007 5:31 am ((PDT)) Hi Pete: Went to the link. High RPM of the spindle with a fine feed gives less cut per tooth. (Not too high, or you can get sympathetic vibes in the table.) A small radius on the cutting edge/tip that is larger than the feed is highly recommended. That, plus a little finishing will give a good finish free of toolmarks. Jerry G (Glickstein) ------- Re: Guys, I've got a question. [MILL A CIRCULAR UNDERCUT sherline group] Posted by: "Marcus" implmexx~xxaxionet.com implmex Date: Tue Jun 12, 2007 8:17 pm ((PDT)) "Alan Haisley" ] wrote: >> On a Sherline mill, would you do this with a rotary table? If all you had were a manual Sherline mill and a manual rotary table, would you use a boring head with enough offset in the table to cut the groove as an eccentric and manually rotate the table to bring it into circularity? Or some other way? Alan << Hi Alan: Milling a circular undercut in a round bore, say for a snap ring, can be accomplished many ways on manual equipment. If the part is small enough to fit on the rotary table, and the bore to be machined is centered well enough in the part that you can swing it 360 degrees, then it's a simple matter of centering the bore to be machined over the rotary table axis, dropping the tee slot cutter to depth, feeding out to the correct location with either the X or the Y axis and revolving the workpiece one rotation. A boring head is not used for this operation. The trouble occurs when the bore to be machined is way off in the corner of a fairly large plate...you can't swing the plate without crashing it into the machine column. Under these circumstances, the best way is to fake it. Center the cutter over the bore with the plate bolted to the machine table. Zero the handwheels and determine your backlash. Pick (or better yet, make) a cutter that's very close to the bore diameter (slightly smaller of course so you can drop it into the hole while it's spinning). Drop the cutter to depth and traverse out to the correct dimension, first in X, then in Y, both positive and negative directions for each axis in turn. Be sure to allow for the backlash amount that you determined earlier. You now have a four leaf clover shape for the periphery of the undercut. Re-center the cutter with the dials, then go out 0.707 times the distance you moved before, but do it in both X and Y sequentially. Pick out all four corners this way...now your undercut will look like a daisy at the periphery. Calculate the offsets needed for 22.5 degrees and refine the shape even more...continue till you get bored. For shallow undercuts like a snap ring, you can cheat and just go out in the cloverleaf pattern, simply cutting a bit deeper than nominal, so the snap ring can drop into place without binding. If you're trying to make an O ring groove however, you have to do a bit better than that. Back in the days before CNC, the "correct way to do this kind of work was to use a boring and facing head, which has a mechanism in it to allow the tool slide to be traversed in and out while the head is spinning. Narex made a good one, so did Wohlhaupter. They were ridiculously expensive, weighed a ton, were clumsy and time consuming to get set up, and were flimsy and chattery. So lots of guys cheated just like I described, on non critical features. Cheers Marcus ------- Fly cutter question [LittleEngines] Posted by: "patmack_1" patmack_1x~xxyahoo.com Date: Tue Sep 11, 2007 2:48 pm ((PDT)) Being a newbie, I have not found an answer to my question in surfing the forums. In trying to machine a surface smooth with a flycutter, mine always seems to cut on the back side or trailing side as well as where it is fed into the material -- apparently cutting a full circle. Using minimum overhang, various speed and feed doesn't seem to matter. What am I missing--? Is it flex somewhere in the set-up? ------- Re: Fly cutter question Posted by: "Andy Wander" awanderx~xxverrex.com Date: Tue Sep 11, 2007 2:56 pm ((PDT)) It could be a number of things(BTW, when I use a flycutter, it also cuts on the "backswing, but I don't really think it's that much of a problem) 1) Your setup is flexible enough so that it doesn't cut full depth when it is doing the initial cut, and then when it swings around, it takes the rest of the cut due to the removed material being out of the way. 2) Your Z axis is slightly tilted. This would cause the symptoms only when cutting in the direction opposite the tilt, or on the front or back side of the work if the tilt is orthogonal to the axis travel. Andy Wander ------- Re: Fly cutter question Posted by: "Stan Stocker" skstockerx~xxcomcast.net Date: Tue Sep 11, 2007 3:33 pm ((PDT)) Greetings: First: Try feeding a bit slower. If you are using the correct tool, but feeding too fast this can happen. If not, hopefully the following will help you sort it out. I doubt this is it, as you say you've already varied feed rate. If the back side cut is just fine scratching it's normal on a perfectly trammed mill. If it's heavy cutting, cut in the other direction and see if it goes away. If it goes away, it's the mill that's out of tram. If it's the same, the likely culprit is flex. Use less overhang, up the speed, decrease the depth and/or feed. You sound like you've already covered these bases pretty well also, so... Look closely at your tool also. You need a tool similar to a left hand lathe tool, with more heel relief. A rounded nose also helps with fly cutters. If the cutter geometry is wrong, it all goes in the toilet, as parts of the tool rub rather than clear the work. Rubbing can flex the tool or work, burnish or work harden the work, in short just ruin your day. Cheers, Stan ------- Re: Fly cutter question Posted by: "David Clark" dcclark111x~xxcomcast.net Date: Tue Sep 11, 2007 4:37 pm ((PDT)) This is both normal and desirable; one of the best indications that your mill is correctly trammed. If I DON'T see that second cut I know that I must tram the mill. To prove to yourself that you're flycutting correctly, replace the flycutter with an indicator and check the flatness of the surface you just cut. The second cut happens because you're cutting with the inside edge, and the tool isn't loaded as much, on the back of the cycle. Think about it this way: do you really only want to see cutting on half the tool rotation? Which half? Whether you're seeing cutting only on the leading edge, or only on the trailing edge, or only on one side, you're not cutting flat. You want to see that full circle. DC ------- Fly Cutter Answer Posted by: "patmack_1" patmack_1x~xxyahoo.com Date: Thu Sep 13, 2007 1:32 pm ((PDT)) I really appreciate your prompt response and comments, fellows. You have certainly relieved my mind. No doubt a lot of my distress was not knowing what to expect out of a fly cutter. I seem to get the same result regardless of the feed direction so sounds like the tram is OK. And, it cuts on the front side and 'scratches' on the back stroke. I just didn't understand that's normal -- and I now see that is the only way to get a smooth surface(Duh!). It did seem to do much better with a little more speed, slower feed, and a lighter cut. It will take more practice for me to be accurate since I've just been doing 'clean up' cuts so far. I do need to take a careful look at the tool just to be sure I'm not 'rubbing' and have the proper edge. Again, thank all that replied -- you made my day! Pat ------- NOTE TO FILE: Jerry Kieffer was involved in a discussion in the Sherline group comparing milling machines. During that thread he described how he engraves small numbers freehand on a mill. Well worth trying. See his message Mon Dec 31, 2007 in the Milling Machine Comparisons file here. ------- Speeds and Feeds [taigtools] Posted by: "Ronald Lambier" ronald_41x~xxyahoo.ca Date: Sun Jan 6, 2008 1:46 am ((PST)) Check out www.colinusher.info, there is listed a beautiful little FREE program called Model Engineers Utilities. You'll find that it covers anything that you will ever need in the way of formula's. ------- Machining Wheel spokes [sherline] Posted by: "n2562001" jlkiefferx~xxcharter.net Date: Sun Apr 13, 2008 11:19 am ((PDT)) While Hobby CNC machines may not be practical for many one and two off items for model building or whatever, Wheel spokes are not one of those items. Other than first time Gear cutting it seems to be one of the most dreaded jobs complained about. However it is actually one of the easier jobs requiring no math even for tapered spokes. On CNC of course it is only a matter of programing and single tool setup. For those who have no CNC system, but have a Mill and rotary table with no desire to use math you are still in good shape. When doing Horology Wheel cutting classes it seems like 100% of the students prefer simple easy setups requiring no math on manual machines. For these classes I do tapered and straight wheel spokes for both watch and clocks as follows. This procedure can of course be applied to any type wheel. First the wheel blank in an arbor is mounted in the rotary table on the mill in the horizontal position. Second scribe point is mounted in the spindle and centered to the arbor/wheel. Third the scribe point is moved to the base of the spoke on the hub, where light pressure is applied to the wheel while it is rotated 360 degrees. This scribed mark locates the base of the spokes. When completed a second circle is scribed at the top spoke position in the same manner. Fourth the width of the spoke at the hub is determined and a pin gage of that diameter is mounted in the spindle. The rotary table is then set to zero. From that point the pin gage is then centered on the Hub circle and scribed on each side. The rotary table is then indexed for the number of spokes and the scribing is repeated for each spoke. When completed the same procedure for the top of the spoke is performed on the outer circle. Fifth the scribe marks from the top and bottom of each spoke are used to scribe the sides of each spoke with a straight edge. Sixth a small center cutting endmill is mounted in the spindle to machine the spokes. Seventh one of the spoke scribed side lines is aligned 90 degrees to the mill column. This is easily done with a machinist square resting on the column and by rotating the table until aligned. Eighth the spoke side is then machined along the scribed line. When complete both top and bottom curved surfaces are machined by rotating the table with the endmill positioned next to the scribed line. The table is rotated until the endmill reaches the scribed line of the next spoke. This process is then repeated for the same side of each spoke. Ninth the opposite side if the spoke is now aligned 90 degrees to the column in the same manner as above. When compete the side of each spoke is machined and the center section will fall out for each spoke. This process works equally as well with either straight or taper spokes. Once one wheel has been machined it can be used to scribe the spokes of additional wheels. Jerry Kieffer ------- Setting tool height on really small endmills Posted by: "clickmrmike" mrmikex~xxclickbang.com Date: Fri May 23, 2008 10:02 am ((PDT)) Hey all- I'm machining some wax molds with some small (for me) endmills -- .001"-.004" diameters -- and I'm looking for a way to accurately set the tool height. There are some good tool height jigs for larger bits, but I'm afraid I would snap off these little end mills using them. I've been setting height with another tool, than swapping in the new tool and collet (I've got a 2019CR with standard, not ER, spindle) but it's not always repeatable. Anyone have a suggestion on a good way to set a bit this small with 0.0005" or better accuracy? Or am I nuts for trying? Thanks, clickmrmike ------- Re: Setting tool height on really small endmills Posted by: "Nicholas Carter and Felice Luftschein" felicex~xxcasco.net Date: Fri May 23, 2008 10:18 am ((PDT)) I'm thinking the only way would be to use a microscope and optically determine where you are. All the tool setters likely have too much backforce to use them with such tiny bits. See our homepage at www.cartertools.com/nfhome.html ------- Re: Setting tool height on really small endmills Posted by: "Shad" shendersonx~xxthegeekgroup.org Date: Fri May 23, 2008 10:52 am ((PDT)) There's the optical method, but that requires a microscope. Bits that small should have a collar on them, and be a known length from the tip to the collar. If they've been resharpened, that length may be wrong. I'd suggest one of the "touch and light" blocks for setting it. Make sure the surface of the block and the table are spotlessly clean, though. May be worth checking the block for parallel across the top and bottom. Be careful, bits that small are usually solid carbide. They'll break with the slightest bit too much side load. I recommend safety glasses and a face shield, as they run fast, and are very "energetic" when they shatter. Hope it helps! Shad H. ------- Re: Setting tool height on really small endmills Posted by: "Ken Cline" clinex~xxfrii.com Date: Fri May 23, 2008 11:58 am ((PDT)) I built a tools setter that could be adapted for really small end mills [described here http://www.newvernacular.com/Tool_Setter.html]. It may work as is, but switching to a lighter springs would certainly do the trick. Last time I checked, repeatability was about .0002", which I find pretty amazing since it was built on a Taig, not a precision grinder. I've been thinking about making a batch of these (with better quality finish - this was one was my first attempt). Let me know if there is interest. The cost should be reasonable. ------- Re: Setting tool height on really small endmills Posted by: "Rick Reyes" aztaigx~xxyahoo.com Date: Fri May 23, 2008 8:19 pm ((PDT)) Maybe using a feeler gage connected to some kind of continuity circuit. ------- Re: Setting tool height on really small endmills Posted by: "kd006" kd006x~xxyahoo.com Date: Fri May 23, 2008 9:26 pm ((PDT)) I know it's low tech but how about cigarette papers, just guaged one of mine and it's like .0005" thick, they come in packs of a hundred for about a buck and can even be torn in half or strips for checking clearance. Probably been used for a hundred years for just this purpose. Kristin ------- Re: Setting tool height on really small endmills Posted by: "Steve Blackmore" stevex~xxpilotltd.net Date: Sat May 24, 2008 1:27 am ((PDT)) >Anyone have a suggestion on a good way to set a bit this small with >0.0005" or better accuracy? Or am I nuts for trying? Possibly Nuts :) What's the minimum resolution/repeatability of your machine? As you say -- it's not always repeatable. Taig says: Mechanical Resolution: 0.0005 in. So you could end up that far out anyway. Microstepping down and watching the tool tip until it just touches the surface is probably the best scenario for tiny bits. You'll need some of those clip on type jeweller's loup magnifiers on your safety glasses for that (or spectacles if you wear them) at least. DONT have the spindle running, too easy to hurt yourself, just turn it by hand until you JUST scrape the surface, and you're there. Steve Blackmore ------- Re: Setting tool height on really small endmills Posted by: "n2562001" jlkiefferx~xxcharter.net Date: Sat May 24, 2008 8:09 am ((PDT)) I have found this thread interesting and a reminder of several years of frustration. Having work with Micro Machining and Micro tooling for many years, one of the first things you learn is that conventional machining practices are of little to no value. One example would be Steve's comment on turning the spindle by hand while touching the metal with a small mill. I also assumed this in the beginning but soon found that in practice a .005" endmill will simply snap off when it touches the metal. Another critical thing was to have absolute minimal runout on mounted Micro tooling. The only thing I have found that works well for mounting this type tooling are quality Watchmakers WW collets. Micro tooling set ups are just too small to be measured with standard measuring tools or procedures. After years of frustration you find that the most effective solution is to actually be able to see what you are doing. Nick was correct to suggest a Microscope. You learn that accurate observation and comparision is really the only practical way to consistently and accurately set up Micro Machining tooling. You also learn the hard way that the Microscope MUST BE CORRECTED FOR DISTORTION. If not you will be looking at one thing while doing another. The Microscope is used to observe tooling for setup the same way you observe a 2.000" cutter in a bridgeport. It is also used to observe stress on the tooling to avoid problems and breakage. To be effective I found that the Scope needs to be mounted to the headstock so it can be centered and focused on the cutter at all times while machining. In addition it was also found that it must rotate 0 to 90 degrees while remaining centered and focused. Various cutting angles will need to be observed for accurate setup and machining. In addition to that it must tilt and angle for the best surface observation. When set it must also remain centered and in focus when rotated. When a .005" endmill is made to look like a fence post it can easily be positioned within .0005". Under proper quality optics .0005" will appear like .050". On inexpensive Optics it will appear like looking through the bottom of a Beer bottle. The ability to see what you are doing in this case cannot be explained but must be experienced. It is a very powerful tool. The Milling Machine Mount as discussed above and compatible Microscope rugged enough for machine tool use are now available from Sherline. (It can be seen on their Web site under Microscope and mount.) While the setup was designed for the Sherline mill, it can be easily modified to fit a Taig Mill with the standard Taig headstock. Three things are required. First the front two mount 1/2 radiuses need to be filed or machined square to fit the sharp square curners of the Taig Headstock. Next a .475" thick by .750" square mounting spacer is required. And finally a single 10-32 hole must be drilled and tapped in the headstock for mounting. The only issue on the Taig Mill is that the larger leadscrews are not as sensitive as the Sherlines for the smallest Micro setups. For one job this setup is of course expensive and probably not practical, but indispensable for ongoing Micro Machining procedures. Jerry Kieffer ------- Speed of metal removal - fly cutter vs. endmill [sherline] Posted by: "Alan Haisley" alanhyx~xxroadrunner.com Date: Wed Nov 19, 2008 10:32 am ((PST)) I have a piece of 6061 aluminum, about two inches square. (Actually an L shape.) I need to remove about .2 inches from the face. Will this be faster with a Sherline flycutter or with an endmill of some size. If with the flycutter, assuming the swing is about 1.5 inches, what spindle speed and depth of cut should I attempt? If with an endmill, should I use a 3/8 inch two flute mill? What spindle speed should I use in that case? Alan (I misread a plan and used 1/2" thick bar when I needed 1/4" thick. Read twice, measure twice, cut once - I should have.) ------- Re: Speed of metal removal - fly cutter vs. endmill Posted by: "Alan Wright" alanx~xxyahoo.com Date: Wed Nov 19, 2008 10:55 am ((PST)) It would take a lot of passes with the flycutter. I would use the 3/8" mill. You can turn the spindle up quite high, and do it in just a couple of roughing passes and finish cut. You could follow with one pass with the fly cutter if you need maximum flatness. Not really sure if this is any faster, but fly cutters are generally more trouble than end mills. I rarely bother flycutting any more. If the milled finish just needs to look prettier or be smoother, I use a deburring wheel or a scotchbrite belt, and follow that with a quick buffing if I really want it shiny. It can be a battle to get (and keep) a good finish right off the machine, but a no brainer with the finishing tools. Alan W. ------- Re: Speed of metal removal - fly cutter vs. endmill Posted by: "Alan Haisley" alanhyx~xxroadrunner.com Date: Wed Nov 19, 2008 11:20 am ((PST)) Thanks Alan W. I was leaning toward the endmill myself, although the flycutter leaves a clearer surface. For appearance, I might switch to a 1/4" mill for the finish pass. That often seems a more attractive finish than the optically flat mirrored finish that people usually seem to go with. (Except Jerry K, who bead blasts carvings to look like castings, but he is replicating the finish of a scale model.) Alan H. ------- Re: Speed of metal removal - fly cutter vs. endmill Posted by: "n2562001" jlkiefferx~xxcharter.net Date: Wed Nov 19, 2008 2:43 pm ((PST)) Alan H. Removing large amounts of metal with a Sherline mill is all about creating stability. Cutters are most stable in these machines when held as close to the spindle nose as possible. If you happen to experiment you will find that maximum metal can be removed with a 1/4" endmill held by a MT collet. In addition for maximum metal removal no more than .625" of flute should be extending in front of the collet. Under these conditions you will be able to remove your .200" depth in Aluminum per pass if you wish. Larger endmills held in endmill holders can be used, but are far less stable because of the distance held from the spindle nose decreasing metal removal and accuracy. Speed can be adjusted under load to create observed optimum cutting conditions. Cutter manufacturer suggested cutting speeds for cutters when used on these machines will be of little to no value. Jerry Kieffer ------- Re: Speed of metal removal - fly cutter vs. endmill Posted by: "Alan Haisley" alanhyx~xxroadrunner.com Date: Wed Nov 19, 2008 7:06 pm ((PST)) Jerry: Thanks for the information. While I have a 1/4" collet I don't yet have a mill in that size. I allowed for it when I bought the Sherline but am still tooling up as needs arise and figured at some point to need a 1/4" carbide endmill. Sounds like I could stand to get a couple small shank HSS endmills too. As you indicate that stability is the important factor here, I'll take lighter cuts using a 3/8" endmill in a holder since I have that available. More time but I'll get done eventually. Alan ------- Re: Tslot cutter for Sherline [sherline] Posted by: "Fred Smith" imservx~xximsrv.com Date: Sun Feb 1, 2009 10:34 am ((PST)) "Bradford Chaucer" wrote: > Does anyone know where I can obtain a "T" slot cutter to cut slots > which match the Sherline products. I want to make a general purpose > riser block that will allow me to attach the normal tool holders and > other accessories. I recently made some t-slots for Sherline sized parts. The woodruff cutter mentioned in another response works quite well. However, that type of cutter is not really designed for extended undercutting like needed for a long t-slot. I solved this problem by relieving the entire bottomside of the t-slot with a 3/8 thru slot from the back. I left approximately 1" attachment ribs (every 4-5 inches in 1/2 inch material) so that the material would retain plenty of strength and rigidity, even though the t-slot went all the way through the length of the material. The only area that really stressed the t-slot cutter was at the 1" ribs, and once they were cut through, the chip cleared away, awaiting the next 1" challenge. Fred Smith - IMService http://www.imsrv.com ------- milling [atlas_craftsman] Posted by: "soveral36" soveral36x~xxyahoo.com Date: Fri Jun 5, 2009 4:59 am ((PDT)) I am a newbe who has aquired (and resurrected) a Craftsmen 12 X 36 that was a Hurricane Katrina victim. Info gleened from this group has been invaluable. Many thaks to the past and present contributors. My issue is the work holding in the milling attachment. The vise-like jaws and shim plates are awkward for round and odd shapes. Has anyone devised an insertable fixture or some better methods for securing the workpiece? The issue may be my inexperience, any guidance would be appreciated. ------- Re: milling Posted by: "Bruce Freeman" freemab222x~xxgmail.com Date: Fri Jun 5, 2009 9:39 am ((PDT)) I have a 10" Atlas, and the milling attachment has no moving jaw, just two screws. I milled myself a V-block of 1" square aluminum to hold round things. I use an upper block with two dimples to receive the two screws. Works quite well. ------- Re: milling Posted by: "Rexarino" rexarinox~xxgmail.com Date: Fri Jun 5, 2009 3:09 pm ((PDT)) Congratulations on your lathe! Really odd shapes can be cast in a plaster of Paris shell, in a convenient container, machined, then heat the plaster to crack off the big chunks, and finish with acid (vinegar, muriatic pool acid, etc) to dissolve the rest. Flat chunks can be clamped to a plate, with a boss on the back to clamp in the screw vise. If the part will have holes when finished, you can screw through those into a backup block that goes in the vise. rex ------- Re: milling Posted by: "catboat15x~xxaol.com" Date: Sat Jun 6, 2009 12:48 pm ((PDT)) Depending on the shape, you sometimes can solder the part onto a block of brass or steel. Sometimes "Crazy Glue" will hold a part in place while machining. Watch and clock makers use what is called a "Wax Chuck" a cup of wax that is soft enough or can be softened and the odd part pressed in place. ------- Re: milling Posted by: "Rexarino" rexarinox~xxgmail.com Date: Sun Jun 7, 2009 12:04 am ((PDT)) On Sat, Jun 6, 2009, Norman Griffin wrote: > Thanks for the tips. I copied them all and they worked great. The > plaster of paris tip was really cool. You're welcome! I saw the plaster of Paris tip in a Popular Mechanics magazine when I was too young to own a power tool. Later, I saw someone use it to hold a round rock in the rectangular vise of a lapidary saw, and the epiphany stuck. Other tips: You can grip a sacrificial piece in the vise or chuck, and mill or turn a recess to hold your work with a little hot glue, double face tape, or cyanoacrolate. Some items can be embedded in a bath of low-melting point metal (the name is not recoverable from my memory tonight, might be Wood's metal, or a bismuth alloy...) I've seen work soldered, brazed or welded onto a stub that went in the vise or chuck, such that the last operation separated the useful part from the stub. Sometimes a part can be machined "nearly" to the point of separation from a larger piece, but enough is left to hold the part for further machining steps. The final separation can be a snap-off and file smooth. Rex ------- Re: how to mill angled edges? [sherline] Posted by: "a3sigma" dcclark111x~xxcomcast.net Date: Mon Jun 8, 2009 4:17 am ((PDT)) Kenny Gorman wrote: > I am a complete newbie, and I have some books on the way. But in the > mean time I have been playing around with my Sherline 5000. Here is > my dilemma. > I am making a small bracket out of ABS for a prototype. The part has > many different angled edges that need to be milled to form the shape. > How can I do this w/o NC or CNC? I can't turn each X and Y perfectly > by hand to make the angled cut. It appears I need to do a new setup > for each angle so it's in-line with the X axis? Am I missing > something being a complete newbie? Thanks -kg Without CNC there's really no good way to mill other than parallel to the axes. Consider a mill vise with rotating base: http://tinyurl.com/nf36nm or a rotary table: http://tinyurl.com/n86878 Various fixtures can facilitate the work. If you post a sketch of what you're making, we can make some specific suggestions. DC David Clark in Southern Maryland, USA ------- Re: how to mill angled edges? Posted by: "DA Dossin" danatlx~xxyahoo.com Date: Mon Jun 8, 2009 4:44 am ((PDT)) Also add in a tilting angle Table #3750 ------- Re: how to mill angled edges? Posted by: "chieftoolmaker" chieftoolmakerx~xxearthlink.net Date: Mon Jun 8, 2009 5:58 am ((PDT)) And a good angle plate plus a good protractor. (plus clamps) Jerry G (Glickstein) P.S. Since you are typing about milled edges, I assume the part has a reference face. ------- Re: how to mill angled edges? Posted by: "Marcus" marcusx~xximplant-mechanix.com Date: Mon Jun 8, 2009 9:34 am ((PDT)) Hi Kenny: There are a bunch of ways to achieve what your're trying to do on a manual mill, but all involve some extra setup time compared to CNC milling. If you are looking down on the top of the part, and you have a bunch of non-parallel edges to cut in order to profile your part, the easiest and fastest way on a manual machine is to mount the workpiece on a gadget called a "rotary table" or "turntable". This accessory allows you to accurately rotate the workpiece relative to the X and Y axes of the machine so you can rotate until your profile is parallel to one or the other axis, lock it down and then cut the angled face to size. It works well but has limitations in the size of workpiece you can mount and the difficulty you sometimes have finding a way to attach the workpiece to the table. Another way is to clamp the workpiece directly to the mill table and re-position it for every non-rectilinear feature. This way works well too, but as you can imagine, it takes up a LOT of time, especially if you are trying to work accurately. A third way, is to walk the cutter along the angle in stairstep motions, by calculating how far you must move in each axis in turn to keep following the desired angle, and making the motion increments very small. This sounds dreadfully tedious, but it's actually very effective for certain angles over short distances...45 degrees is the best example, since each axis is moved the same increment in turn. Typically a decent result for appearance and precision can be achieved with a 1/4" diameter cutter moved in increments of 0.005", so if you need to move an inch, you've got to pay attention for a total of 400 moves (200 in X and 200 in Y). Sounds terrible but it's surprisingly not too bad. Another way is to stand your part up on edge and clamp it to a suitable right-angled block or squeeze it in the vise, tilted to the angle you want to mill off. You set the angle using any one of a number of different gadgets...you've seen by now, references to angle blocks, sine bars, angle plates, protractors, etc etc etc. These are all variations on a common theme and a dissertation on all their uses and advantages would be a whole 'nuther topic but their common purpose is to tip the block to the proper angle before clamping it into place. When you get to wanting angles on other faces, say for example a chamfer around the profile of a part, there are yet more ways you can get there. A common way is to make a form cutter that has the proper angle ground onto its cutting edges...this can then be walked around the profile. Another way is to use the stairstep strategy as described earlier, but involving up and down (Z axis ) motion. The block can be tipped; the machine spindle can be tilted; etc etc. The attraction of CNC is easy to see, as you can achieve all of these motions with comparative ease and without a mountain of accessories, but there are a few things to remember there too. First, CNC milling is a variant on the stairstep milling strategy... especially with stepper motor driven machines, so its accuracy is dependent on many things not so much an issue with many of the manual methods. Second, you have geometry limitations...for example, you can't mill to a sharp internal corner by profiling around a block...the cutter makes a radiused corner on each internal angle. Third, you need a different bunch of stuff...in this case it's a CAD CAM program, if you're going to make anything of any real complexity; CAD CAM doesn't come cheap and involves a learning curve of its own. There's also a very real loss of immediate motion control...once you hit GO, it GOES!!! and cares not what it wrecks. Lots to think about, I'm sure, but it is all fun and very satisfying to learn. Cheers Marcus ------- Milling a step [taigtools] Posted by: "Mike Nicewonger" twmasterx~xxtwmaster.com twmasterx~xxrocketmail.com Date: Sun Aug 30, 2009 5:47 pm ((PDT)) I need to mill a 1/8" step into the edge of a piece of 3/4" wide 3/8" thick 1018 bar. Would I be better off to place the part in the vise with the narrow end oriented vertically or does it not matter? Mike N ------- Re: Milling a step Posted by: "Michael Fagan" woodworker88x~xxgmail.com Date: Sun Aug 30, 2009 6:31 pm ((PDT)) In general (not always but the majority of the time), you will get a better surface finish with the bottom of the endmill than the side. Thus, you should keep this in mind. Also, it depends on the size and how confident you are in your machine's tram compared to the part tolerance. An out of square column will make the slot variable depth, but an out of square vise will make it a variable width. This becomes more pronounced over a long piece (particularly once you overhang the vise). ------- Re: End Mill Cutting - Basic Question [taigtools] Posted by: "rachaelseven" katzengx~xxhotmail.com Date: Mon Sep 7, 2009 7:33 am ((PDT)) "noisillator" wrote: > I need to cut a slot through a 6061 bar. The material is .75" thick, and the slot will be .200" wide by x 4" long. All I have on hand to do this are a couple of 3/16" end mills. One is a 4-flute, the other a 2-flute that came with the mill. Each has a 3/16" shank. My question is whether an end mill with flutes only 1/2" long is OK for a 3/4" deep cut like this. Jack < That will be a tough one. Since the slot is so close to the size of the mill, chances are that the flutes will cease to clear once you get 0.5" deep. Rather than risking trashing the material, I think you'd be well advised to invest in a long flute end mill, something with at least as much flute as the depth of the slot you want to make. -------- Re: End Mill Cutting - Basic Question Posted by: "George Plezia" toolsrulx~xxbellsouth.net Date: Mon Sep 7, 2009 8:08 am ((PDT)) Flip (rotate) the part. Op. 1 first side, op. 2 second side. Might have to make a locating type fixture for when you flip, no big deal. Possible? ------- Re: End Mill Cutting - Basic Question Posted by: "Stan Stocker" skstockerx~xxcomcast.net Date: Mon Sep 7, 2009 8:11 am ((PDT)) Hi Jack: The short answer is no, but there are ways if you must do a slot deeper than your endmill, provided the total depth is not more than twice the length of the flutes plus the extension from the collet or end mill holder. First - use the two flute, two flute end mills are made for end cutting. As the slot if wider than the endills in use, you can do the slot to size to the flute depth, then plunge through the center of the remaining waste. Remove as much as possible then do a final fine cut pass with the endmill shank just rubbing the sides of the full size slot. It isn't stylish or sexy, and tends to need a little bit of clean up when it's all over, but it works. Same idea as a piloted router bit, just it's the shank that rubs. You can even go deeper than twice the flute length, up to the point that the end mill holder no longer clears the work surface this way. Very ugly, not recommended, but some days you need to get a job done and waiting on a cutter and the brown truck to appear just isn't an option. Rig a shop vac to extract chips, this is not the time to jam a cutter up with swarf. Alternatively, you can cut the slot to flute depth from one side, flip the piece, and finish up. Work for up to twice the flute length, or in combination with above up to four+ times the flute length if you're feeling bold or lucky :-) You have your choice in methods to locate. You can through drill the ends of the slot and pick up from the holes. You can pick up the edge, basically cutting two pockets, one from each side, then let them meet in the middle. You can fix a fence and / or stops to the table. Just remember to use the same edges of the bar as references. As delivered, bar stock isn't particularly precise; while you usually don't notice a thou or two variation, a two thou step in a slot is enough to cause problems in some applications. In any event, plan on a little file or abrasive work to clean up the slot interior when the cutting is over. And for a really old school solution, you can always chain drill the waste and file the slot to size. I've done it and it isn't such a big deal for one-off stuff. If possible, it would be preferred to obtain a two flute end mill with longer flutes. As you are plunging, a four flute is usually not the tool of choice as MOST are not end cutting (can't plunge) although SOME four flute endmills have the ends ground to work like a two flute for end cutting. Have fun, Stan ------- Re: End Mill Cutting - Basic Question Posted by: "kd006" kd006x~xxyahoo.com Date: Mon Sep 7, 2009 9:10 am ((PDT)) Jack: Since it seems most of your project is 3/4 thick stock, I second the suguestion about getting long flute end mills. Might want to shop around the catalogs and order a couple of each size in the small ones with 7/8 flute length. There are workarounds but having the correct tool is the best. Kristin -------- Re: End Mill Cutting - Basic Question Posted by: "noisillator" tech.writerx~xxearthlink.net Date: Tue Sep 8, 2009 5:56 am ((PDT)) That's a good idea. Most of my work won't be this thick; this is just a fixture for the table. Still, it wouldn't hurt to have a few of those around for times like this. For the current project, I've decided to handle it differently. The slots are meant to hold 10-32 cap screws that will be recessed below the surface of the part. There will be washers under the heads. I'm milling the 0.200" wide slots to a depth of 0.4" from the bottom of the part. When that's done, I'll turn it over and cut wider slots (to clear the washers) down from the top. That will provide a 0.35" depth for the heads and washers, as well as a through slot for the 10-32s. Thanks for everyone's advice. ------- Re: End Mill Cutting - Basic Question Posted by: "kd006" kd006x~xxyahoo.com Date: Tue Sep 8, 2009 9:06 am ((PDT)) Jack: Why flip your part? Mill the wider slot first, then your 3/16th cutter can finish up the through slot without binding. Just clamp up your part with some spacer to protect the mill table. Kristin ------- NOTE TO FILE: The following conversation deals with a simple question as to how to make a flat on a small stepper motor shaft. While the question originally was about milling such a flat, there are indeed other simple solutions. ------- machining flats on stepper motor shaft [taigtools] Posted by: "gotham_hunter" gotham_hunterx~xxyahoo.com Date: Tue Oct 6, 2009 5:41 am ((PDT)) I've recently acquired a Sherline rotary table with the motor mount installed. I have some double-end shaft steppers I'd like to use, but the shaft has no flat. In the install documents I see that Sherline does not advise tightening the set screw onto the round part of the shaft. I have the mill available, and I'd like to know if anyone has milled flats onto the end of motor shafts like this? Is it practical to do so? Am I likely to make more trouble for myself than by clamping the set screw onto the round shaft? All help appreciated. ------- Re: machining flats on stepper motor shaft Posted by: "Michael Fagan" woodworker88x~xxgmail.com Date: Tue Oct 6, 2009 6:05 am ((PDT)) If you clamp the set screw directly on the shaft, you will raise a ding that will nearly permanently seize the parts together. However, I think that milling the flat is overkill. A few swipes with a file or a touch with an angle grinder should make all the flat you need. ------- Re: machining flats on stepper motor shaft Posted by: "Shad" shendersonx~xxthegeekgroup.org Date: Tue Oct 6, 2009 7:03 am ((PDT)) Easy-peasy. Firstly, short all the wires together. That'll make the motor incredibly difficult to turn, and will pretty much keep the shaft in the same orientation. Next, poke a small hole in a sheet of paper, and poke the shaft through the hole. Tape the paper to the motor, and around the shaft to the paper, so no grit gets into the bearing. Then, grab the motor *gently but firmly* in a bench vice. I recommend some wood or corrugated cardboard to pad the jaws. Then take your trusty Dremel tool with a grinding wheel and make a small flat. Doesn't have to be precise, it just has to be there. Once that's done, wipe and brush off the motor shaft, then remove the paper carefully. Beware that the shaft may be slightly magnetic, and the grinding debris may stick to it. Clean it within an inch of its life. The flat is necessary because the setscrew will mar the shaft, and probably cause the coupler to become stuck on it. Prying on stepper motors isn't a Good Thing. You can use a file, but the shaft may have a tendency to rotate, even with the wires shorted together. A Dremel is faster and easier, albeit messier. Hope it helps! Shad H. ------- Re: machining flats on stepper motor shaft Posted by: "gotham_hunter" gotham_hunterx~xxyahoo.com Date: Tue Oct 6, 2009 7:24 am ((PDT)) Thanks. I appreciate the help. ------- Re: machining flats on stepper motor shaft Posted by: "joseph arnold" jspharnoldx~xxyahoo.com Date: Tue Oct 6, 2009 4:11 pm ((PDT)) I think you can file a flat on the motor's shaft by hand with a flat file faster than you can prepare the set-up for milling it. I believe it would be a mistake to try tightening the set screw onto a round shaft. Have fun. Tom Arnold ------- Re: machining flats on stepper motor shaft Posted by: "Joseph Heath" jtheathx~xxheathcreative.com Date: Tue Oct 6, 2009 6:22 pm ((PDT)) I simply poked the shaft through a sandwich baggie and touched the shaft to my bench grinder. Cheers, Joe ------- Re: Drilling holes in a circular pattern on the Sherline Mill [sherline] Posted by: "Pierre Coueffin" pcoueffinx~xxgmail.com Date: Sat Nov 28, 2009 5:45 pm ((PST)) On Sat, Nov 28, 2009, retabeth wrote: > I need to drill a series of small holes indexed (5) in a circle and was wondering if I need to buy an indexing attachment for the Sherline Mill? Has anyone done a homemade version? < If you only need to do it once, a bit of trig will get you the x-y coordinates to drill at. Try this website: http://www.selectsmart.com/darex/bolt_cir.html ------- Re: Drilling holes in a circular pattern on the Sherline Mill Posted by: "Mike Bauers" mwbauers55x~xxwi.rr.com Date: Sat Nov 28, 2009 6:17 pm ((PST)) I've seen the like as production jig/fixtures. You make a holder for the disk with an over-layer or restraining bars to lock/bolt-down the disk. You have one drill hole and another locator hole that duplicates one of the other holes in the part. It works by you centering the drill-hole under the chuck of the mill with a rod of the same size as the drill you are going to use. You lower the rod into the drill-hole and wiggle the fixture just a bit to ensure it is centered under the chuck. The fixture is designed to be clamped to the mill table. For ease of this example the holes you want to drill are equally spaced around the disk and in a circular line on that disk. You now have the fixture positioned and locked to the mill table. You leave the mill table alone and use just the up and down of the chuck tower. The fixture is designed to have the disk nest into a matching recess. Depending on what materials you have to work with and how large the disk is, you have designed the fixture to lock the disk with a restraining top plate or a couple of bars that conveniently bolt into place. You place the disk into the fixture and lock it down. You then insert the proper drill, run it while raised to ensure it's running straight and true, then lower the running tool down to the drill the disk. When you made the fixture you also laid out and drilled what will be the next hole, you also polished and rounded the cut end of a rod that is the same size as your drill. It only needs to be about the length of a finger, just a conveniently long enough rod to handle. Once you drill your first hole in that disk, you will next unlock the disk, rotate it so that the hole lines up with the next hole in the fixture. That is a locator hole. You will next insert that matching diameter into the locator hole, re-lock the restraining plate/bars over the piece, drill the new hole, unlock, rotate, lock-down the disk, repeat, repeat........ Expected variables may be provisions in your fixture for burrs around the holes on the backside, how thick of a base you decide to make your fixture from, even if you make the fixture all metal or just some metal. [You can always use some quality thick plywood or any hardwood scrap for the fixture base.] If your disk is moderately small and you only want to make a very few parts, you can use a chunk of hardwood board and a cover plate of a plain common hardware store metal electrical box flat cover. Those covers are about 6 x 6 of likely thick enough steel......... and cost about 50 cents new. Best to ya, Mike Bauers Milwaukee, Wi ------- Re: Material for Trial Cuts? [taigtools] Posted by: "Ken Cline" clinex~xxfrii.com Date: Fri Dec 18, 2009 9:19 pm ((PST)) On 18 Dec 2009, at 5:28 PM, Jack wrote: > Some of the work with my mill is becoming sufficiently complex that I would like to make a mockup first. Looking at plastics like Delrin and Nylon, they seem to be just as expensive as aluminum. Is there anything besides wood that's cheap and readily available? < Polyethylene (HDPE, UHMW-PE, etc.) is a waxy plastic that won't wear your tooling. Cost is 1/3 that of acetal. I buy scraps by the pound at my local plastic store/fabricator at even lower prices. 1/4" sheet makes a nice sacrificial base for through milling operations. Getting a good surface finish on the stuff sometimes requires good cutting strategy. The machinable wax that Rick mentioned will cut better, but you'll have more initial cost. Don't overlook foam, either. ------- Re: Material for Trial Cuts? Posted by: "Will Schmit" anchornmx~xxyahoo.com Date: Sat Dec 19, 2009 6:45 am ((PST)) Make sure that you store it flat. It thinks it is a liquid, and will sag if it is stacked unevenly. ------- Re: Material for Trial Cuts? Posted by: "mbonfire2002" mbonfirex~xxhotmail.com Date: Sat Dec 19, 2009 3:26 pm ((PST)) Cheap and OK but will not give the finest cuts: foam sold in craft stores for floral arrangements (typically colored green). Better: find a supplier in your area that supplies materials for making outdoor signs. They have polyurethane foam boards that are using with CNC routers to make those fancy gold lettered signs for fancy stores. I bought a slab that is 2 inches thick and about two square feet for about $30. I use it with good results. One spec for this kind of material is pounds/cubic foot...the denser, the more $$ and the finer the details and higher the strength. Best: there are polyurethane slabs available specifically for proofing machining. The ones I am familiar with are maroon color and almost look like wood. Mill beautifully and hold sharp, fine details...but not cheap. You can get the material to very thick sections...2 inch thick slabs common. Steve ------- Rough center in cut? [sherline] Posted by: "botwire" botwirex~xxyahoo.com Date: Thu Dec 31, 2009 6:14 am ((PST)) Hello all, I'm new to milling. I just got a 5400 milling machine and have been practicing manual operations since I don't have CNC for it yet. I have noticed there is a rough center in the cut when I use a 1/8" end mill. Is this becuase the speed is either too fast or too slow? I don't seem to have the same problem with the 3/8" end mill. ------- Re: Rough center in cut? Posted by: "chieftoolmaker" chieftoolmakerx~xxearthlink.net Date: Thu Dec 31, 2009 7:27 am ((PST)) Check the end mill geometry rather than the speed. Although smaller end mills require higher speed. What material are you cutting? Jerry G ------- Re: Rough center in cut? Posted by: "botwire" botwirex~xxyahoo.com Date: Thu Dec 31, 2009 7:43 am ((PST)) I have been cutting aluminum and wood scraps I have around the house. My goal right now is learning to use the mill, making arbitrary cuts so that I can learn the characteristics of the machine and how different size bits at different speeds cut. When you say end mill geometry, do you mean look for signs of chipped flutes? ------- Re: Rough center in cut? Posted by: "chieftoolmaker" chieftoolmakerx~xxearthlink.net Date: Thu Dec 31, 2009 7:50 am ((PST)) Chipped flutes are a possibility, but I meant if you have the proper rakes (clearance angles) for the stuff you are cutting. Even new end mills with the wrong clearance cutting angles will behave badly on the wrong material. That is the reason for the tremendous variety of cutters available. Jerry G ------- Re: Rough center in cut? Posted by: "botwire" botwirex~xxyahoo.com Date: Thu Dec 31, 2009 8:29 am ((PST)) I'm at work so I can't post any pictures right now. The endmill (double end)that I am using, is the one that comes with the sherline accessory pack. I have no idea what the rake is on those. I will try to post some pictures of it tonight. ------- Re: Rough center in cut? Posted by: "Ian Newman" ian_newx~xxyahoo.com Date: Thu Dec 31, 2009 8:44 am ((PST)) Hi. What is the width of the cut you are taking? You should not attempt to cut more than 1/4 of the cutter diameter on each pass and you will get a poorer finish if the side of the cutter doing the work is "climb cutting" (or "down cutting"). The above problems are worse if you use a non-centre cutting end mill. If you are surfacing with an end mill you should use a centre cutting type (a slot drill) which only has two flutes (although the larger sizes are available with three flutes). Ian ------- Re: Rough center in cut? Posted by: "botwire" botwirex~xxyahoo.com Date: Thu Dec 31, 2009 10:00 am ((PST)) I'm taking about .005 to .010" off each cut on aluminum material I've bought from the hardware store years ago. I'm not sure if it's 6061-T6 or not. The bit is a double ended 1/8" 4-flute end mill that came with my accessory pack. The cut seems to leave swirl marks along the center of the cut on the aluminum as well as the oak wood. ------- Re: Rough center in cut? Posted by: "Ian Newman" ian_newx~xxyahoo.com Date: Thu Dec 31, 2009 12:48 pm ((PST)) Hi. You will always see some circular machining marks as a result of surfacing with an end mill - these cutters are not designed to be used in this way (they are designed to cut with their sides - for profiling). To surface you should use a "side and face" cutter or a slab mill (neither are realistic propositions on a Sherline) or use a face cutter or fly cutter. Light vertical mills struggle with the task of surfacing and if you intend to do a lot of surfacing without access to a horizontal mill, a small shaping machine is worth getting. The reason for the marks is that the end mill is thin for its diameter, which makes it rather flexible and so it will tend to bend as it is pushed into a cut. This bending tilts the face of the cutter so it is no longer parallel to the surface being machined, and the leading edge of the cutter cuts more deeply than the rest. The machining marks are not very deep in reality and you will find that marks that are so shallow that you cannot feel them will still be clearly visible - if this an issue you can polish the marks out. You quote a dimension of 0.005 to 0.010 inch - is this the depth of cut? If so it should be OK - as long as you avoid cuts less than 0.005 (the cutter must cut, not rub). If you are using an end mill, it is the width of the cut rather than the depth that is important, especially with a four flute cutter. To get an idea of the problem, imagine a four flute cutter cutting a slot (so it is cutting the full width of the cutter). Picture the plan view of the job, the cutter rotating clockwise and call the direction of the slot being cut the "front" of the slot. As one of the cutter teeth cuts away the front of the slot, it will tend to bend the cutter to the left (looking at the plan view) and push the left hand cutter tooth into the side of the slot. This causes a very rough, lumpy and poor quality side to the slot - this is why you should never cut a slot with a end mill (or if you do, use a cutter smaller than the width of the slot that you wish to cut and cut each side of the slot separately). The two flute slot drill does not suffer from this problem as when the front of the slot is being cut and the cutter flexes, there is no other tooth in contact with the slot sides. The advice to limit the width of the cut to less than 1/4 of the cutter diameter is to minimise the sideways flexing of the cutting tool and the associated problems. I realise that none of the above offer any real solutions to help you to achieve the result that you want, but understanding what is going wrong is a major step towards correcting problems. Ian ------- Re: Rough center in cut? Posted by: "botwire" botwirex~xxyahoo.com Date: Thu Dec 31, 2009 1:08 pm ((PST)) Hello Ian. Thanks very much for your explanations. I could clearly picture what you were saying and it makes plenty of sense. The marks you described under normal circumstances I am aware of. The marks left from my cuts are more gouges than fine swirl marks. I will use that 1/4 width rule and I was not aware of the tool deflection you described and I appreciate the shared knowledge. I have a lot to learn obviously, but you can't learn as much unless you screw up right? :) ------- Re: Rough center in cut? Posted by: "Dave Hylands" dhylandsx~xxgmail.com Date: Thu Dec 31, 2009 2:35 pm ((PST)) Hi. The aluminum that you get at the hardware store is usually pure (or close to pure) aluminum, which is quite soft and very "gummy" to machine. I would avoid it all costs. 6061 is harder and machines much nicer. 7075 is even nicer, but more difficult to get. Here's some photos of some 6061 that was machined using the end of an end-mill (probably 3/8"): http://www.davehylands.com/Machinist/Projects/Fly-Cutting-Cla mps/03-The-Pieces.html In particular, look at the bottom right. For really smooth finishes, I use a fly cutter. If you click Next twice from the previous picture you can see a fly-cut finish. You also need to make sure that the end-mill is perpendicular to the work. With the Sherline, because of the way the motor is mounted, the head tends to have a tilt to the right. This can cause uneven cuts as one edge of the endmill is slightly lower than the other side. For 1/4" or small end-mills, I always run the mill at full speed (I don't have the 10,000 RPM splindle - just the stock one). Dave Hylands Shuswap, BC, Canada http://www.DaveHylands.com/ ------- Re: Rough center in cut? Posted by: "botwire" botwirex~xxyahoo.com Date: Thu Dec 31, 2009 3:23 pm ((PST)) Hello Dave. It does seem very soft and gummy now that you mention it. Here are some photos I took to better explain. http://groups.yahoo.com/group/sherline/photos/album/2031504465/pic/list ------- Re: Rough center in cut? Posted by: "Dave Hylands" dhylandsx~xxgmail.com Date: Thu Dec 31, 2009 5:01 pm ((PST)) Hi botwire, I also generally use 2-flute cutters on aluminum. I think the 4 flute cutters are generally used for steel. Using some cutting fluid (I use a syringe with some tapping fluid in it, but there are lots of cutting fluids that should work) will help. When working with aluminum, you also need to look for bits of aluminum which "weld" themselves to the cutter. They can normally be scraped off (I use an X-acto knife). Using cutting fluid will reduce the occurrence of this. I also like to use a 10x - 25x magnifiers to examine the cutting edges to see if there are gouges or if the cutting edge is getting dull. Dave Hylands Shuswap, BC, Canada http://www.DaveHylands.com/ ------- Re: make spline? [Metal_Shapers] Posted by: "Ingrid and Alan" puddleduckx~xxproaxis.com Date: Mon Jan 25, 2010 8:22 am ((PST)) > Do you have any advise on cutting external splines [on a shaper] > please?? Thanks in advance. Regards Andy T No, sorry Andy, I've never tried that. I think I'd probably use a horizontal mill for that. Alan Painter ------- Re: make spline? Posted by: "f350ca" f350cax~xxyahoo.ca Date: Mon Jan 25, 2010 11:03 pm ((PST)) Andy: Haven't cut external splines on the shaper, a vertical mill is easier. Would be the same as cutting a keyway, just index the shaft and cut a series of them. Looking at older equipment you need to spot drill a hole at the end of the key or spline in your case for the cutter to end the stroke in, or turn a recess around the shaft. You may need to grind your cutter to give the correct profile on the splines sides, but any I've done on the mill ended up just needing a square profile. Hope this helps. Greg ------- Drill holes in a circle 60 degrees apart [sherline] Posted by: "len_woodruff" sbcsystemsx~xxgrandecom.net Date: Sun Nov 21, 2010 12:01 pm ((PST)) I need to drill 6 holes at 60 degrees separation in a circle. I centered the part and then moved it to the 1st hole but when I turn it to the second hole, it is out of alignment. Here is a picture of my setup. Any ideas? http://images116.fotki.com/v695/photos/9/219739/9264849/DSC02514-vi.jpg ------- Re: Drill holes in a circle 60 degrees apart Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Sun Nov 21, 2010 1:02 pm ((PST)) Hi Len, I suggest you move out of the rotating vise base setup. Set up your part in a regular vise or clamped on parallels . Drop your holes in using rectilinear coordinates. Jerry G (Glickstein) P.S. There are formulas for locating holes accurately around a circle without moving the part. Try Woodworth Circular Tables. ------- Re: Drill holes in a circle 60 degrees apart Posted by: "Ian Newman" ian_newx~xxyahoo.com Date: Sun Nov 21, 2010 1:06 pm ((PST)) Hi Len, I would check that the centre of the part is really over the centre of rotation of the rotary table (checking the x and the y axis). Also, I would not use a rotary table to do this - you have calibrated x and y feeds on the milling table so use the machine as a jig borer and use x-y co-ordinates to locate the holes. It will be more accurate than the degree calibration on the table. Ian ------- Re: Drill holes in a circle 60 degrees apart Posted by: "len_woodruff" sbcsystemsx~xxgrandecom.net Date: Sun Nov 21, 2010 1:21 pm ((PST)) Why is a rotary table not a good option. I would think that would be the preferred method? ------- Re: Drill holes in a circle 60 degrees apart Posted by: "Alan" alanhyx~xxlive.com Date: Sun Nov 21, 2010 3:00 pm ((PST)) Len: A rotary table is one of the preferred methods. The other is to calculate the x,y coordinates for each hole and move accordingly. In your case though, you have a rotary vise base. First, it is nowhere near as accurate as the two methods mentioned. Secondly, to use it in this mode, you need to find its true center of rotation and position your part's center of rotation at the same spot. I'm not sure though how to locate the center of rotation of the vise though. Anyhow, if these two points CAN be co-located, you should be able to drill your holes. Even then, the graduations on the vise rotary base will leave a lot of room for error. Alan ------- Re: Drill holes in a circle 60 degrees apart Posted by: "len_woodruff" sbcsystemsx~xxgrandecom.net Date: Sun Nov 21, 2010 6:19 pm ((PST)) If I were to get a rotary table then I would still need a centering device like a chuck to hold the material correct? Just shows how little I know about this stuff, I thought the base would do it for me. ------- Re: Drill holes in a circle 60 degrees apart Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Sun Nov 21, 2010 7:07 pm ((PST)) Len wrote: > Thanks for the help Jerry. I will try the xy route. You are quite welcome. It is all about how close you need to be. It is also good to give as much info as possible so anyone can help you. Happy Bird-Day. Jerry G (Glickstein) ------- Re: Drill holes in a circle 60 degrees apart Posted by: "a3sigma" dcclark111x~xxcomcast.net Date: Sun Nov 21, 2010 8:21 pm ((PST)) Len: Following up on Ian and Jerry's comments: Are you certain you're clear on the concept of datuming the workpiece? In this case, ensuring that the center of rotation of the part is at the desired center of the hole circle. This is going to be an issue no matter how you rotate the part. In the case of using Cartesian coordinates, establishing a datum means ensuring that the origin is coincident with the desired center. The more you tell us about what you're trying to do, the more we can help. I'm guessing from your photo that you want to hold the work within the four pins sticking out of the blocks held in your vise. I note the block that's against the fixed jaw is free to pivot about another pin that's further constrained by the vee in the fixed jaw. That's a nice idea for a quasi-kinematic clamping scheme, but may not be the best in this case. A possible problem is that when you tighten the movable jaw, you change the center of the pins. Do you have an indicator and/or an edge finder? It would also be useful to know if you have a lathe. David Clark in Southern Maryland, USA ------- Re: Drill holes in a circle 60 degrees apart Posted by: "Dave Hylands" dhylandsx~xxgmail.com Date: Mon Nov 22, 2010 12:09 am ((PST)) Hi Len: Len wrote: > If I were to get a rotary table then I would still need a centering > device like a chuck to hold the material correct? Not necessarily. I have some pictures here that show using a jig to hold parts: http://www.davehylands.com/Machinist/Techniques/Rotary-Table-Setup/ > Just shows how little I know about this stuff, I thought the base > would do it for me. The base will work fine - you just need to find the center of it. I took a look at my base, and if you remove the vise and the portion that holds the vise, then you could use the edge of the large circle to center the spindle. Dave Hylands Shuswap, BC, Canada http://www.DaveHylands.com/ ------- Re: Drill holes in a circle 60 degrees apart Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Mon Nov 22, 2010 1:03 am ((PST)) Hi Dave, you have "joggled" my mind.... About four years ago, I made a pair of drill jigs for a ship modeler in Port Coquitlam, B.C. in Canada. For Deadeyes. Two sizes. Bolt Circles were 1. .075" with three holes equally spaced of .018" Dia. drilled through 1/4" thick brass. 2. .058" with three holes equally spaced of .016" Dia. drilled through 1/4" thick brass. Made a right angle frame. Used the "shot pin" method to control the rotation of the holder. Worked great. I have the jigs back for teaching aids in my Basic Machining Course at MEworkshop Yahoo Group* ... When I find them, I will upload some pics to the Photo Section here. Details at that time. Regards, Jerry G (Glickstein) * Model Engineering ------- Re: Drill holes in a circle 60 degrees apart Posted by: "a3sigma" dcclark111x~xxcomcast.net Date: Mon Nov 22, 2010 5:50 am ((PST)) Good Morning Jerry, looking forward to seeing that. Good jigs and fixtures are always instructive to study. I wish more members would post more of them. BTW Len, thanks for the very high quality of the photos of your setup. Worth more than words, it would be next to impossible to discuss your specific issues without them. DC ------- Re: Drill holes in a circle 60 degrees apart Posted by: "len_woodruff" sbcsystemsx~xxgrandecom.net Date: Mon Nov 22, 2010 5:10 am ((PST)) Here is how I was trying to center the part. I have a .1015 hole in the center which I thought would be a way to center the part, then move the part to the 1st hole, then I could rotate at 60 degrees to do the other holes. Part in jig for centering http://images112.fotki.com/v503/photos/9/219739/9264849/DSC02519-vi.jpg ------- Re: Drill holes in a circle 60 degrees apart Posted by: "a3sigma" dcclark111x~xxcomcast.net Date: Mon Nov 22, 2010 5:46 am ((PST)) That seems perfectly reasonable, so long as the center of rotation of the vise base is first made coincident with the mill spindle. That is the vital first step in using any rotating work holder. After that, don't touch either mill axis, move the vise in relation to the rotating base, and, if needed, the part in relation to the vise jaws to center the hole in the part under the spindle. (Here, your kinematic mount may cause problems.) Then rotate the base to ensure that it's still centered through 360 degrees. Once that's good, don't move the vise in the base, or the part in the vise. Move either mill axis by the radius of the desired hole circle, drill the first hole, rotate the base, repeat. Should work. Dave Hyland's suggestion for centering the vise base is a good one. I'm looking at the exploded view of it here: http://www.sherline.com/3570inst.htm and see no reason you couldn't bore a tooling hole in the center of the rotating base and through the clamp ring to facilitate alignment in the future. Just be very sure you get the exact center. Then use a pin or dead center in the spindle axis to center the vise base on the mill table, zero your DRO or hand wheels, and you're good to go. Boring the tooling hole on a lathe is by far the best way to do this. If you don't have a lathe, I can walk you through a procedure to do it on a mill. DC ------- Drilling six holes in a c ircle [sherline -- continuation of above thread] Posted by: "Jerry G" chieftoolmakerx~xxearthlink.net Date: Sun Nov 21, 2010 3:47 pm ((PST)) Hi Len, I have sent you direct, a scanned page from my book; " Holes Contours and Surfaces" Page # 233. If the quality is not good enough, let me know , and I will type out the coordinates..... Jerry G (Glickstein) ------- [DIY-CNC] YouTube video - making Tormach TTS-style toolholders on a Grizzly SX Posted by: "devers6" devers6x~xxcomcast.net Date: Thu Dec 2, 2010 7:51 pm ((PST)) I've been concerned about the activity in the Group recently, so I thought I would post something to help pick it up. I sure miss Ballendo - he tought me a lot of what I know as a CNC newbie through this group, so if there is any way of giving back I'd like to think I made an effort. I love watching machining videos on YouTube, so I made a couple of my own. This two-part video covers the making of Tormach TTS-style toolholders using my CNCFusion-converted Grizzly SuperX3 Mill/Drill as a lathe (mounting a lathe tool in the milling vise, mounting the work in a 3-jaw chuck in the spindle, and running the work past the tool to do simple lathe operations). I say Tormach TTS-style toolholders because they are not 100% copies of the genuine article. I don't harden them, and I don't bother cutting the relief on the face of the holder that contacts the spindle. I never use that feature - the main purpose of the holders for me is convenience in switching out tools (assisted by my homebrew pneumatic drawbar) - but I'm sure if needed, others could figure out how to run a few facing cuts to replicate the true TTS holders. Anyway, I think they are fun to watch, and I thought I would post the link here for your enjoyment: http://www.youtube.com/watch?v=_2w8cYXt5_o http://www.youtube.com/watch?v=B-cAnQqpXs0 Dave [AND HERE ARE SOME COMMENTS ON You Tube ABOUT THE VIDEOS] kingjamez80 2 days ago How do you mount your drill chuck perfectly vertical? I haven't had much luck on super precision with the probe method of centering. How accurate are you getting? I'm lucky? to have 0.003" repeatability. devers6 2 days ago I haven't measured, but it has been good enough for my purposes. I get better centering on the mill than I do with my mini-lathe and its tailstock. I didn't show it in the video, but the way I make sure the drill chuck is vertical is to mount another drill chuck in the spindle, leave the lower chuck loose, and chuck the rod in both. Then I tighten up the bolts mounting the chuck to the table. I wouldn't call it super precise, but it has worked for me so far. saunixcomp 2 days ago Great video - very nice quality and well produced. Have you thought about drilling & reaming before profiling the outside? That should prevent the alignment wobble seen around 2:15 ? devers6 2 days ago Thanks - I enjoy watching your videos as well. I'll try switching around the order of operation the next holder I make, and see if it makes it any better. I'm happy with the results I've gotten so far; these toolholders are mostly for my non-critical tools, so I haven't tried to get ultimate precision. I know the methods of dialing in with a DTI when I have to get it exactly right, but for hobby work I seldom need to. ------- Re: YouTube video - making Tormach TTS-style toolholders on a Grizzl Posted by: "Ron Ginger" rongingerx~xxroadrunner.com Date: Fri Dec 3, 2010 5:08 am ((PST)) Great video, very well done. I was going to spend today making a wizard to find the center of a rod by probing around it. Your Idea of a hollow probe is great. I'm going to make a couple sizes of cups and just use the probe center finding I already have. You do miss one important feature of the Tormach system. The undercut on the shank side is to insure the holder bottoms out on the spindle nose, not on the collet. That will give more repeatability of tool length. When you bottom out on the collet face your tool gets pulled up a bit by the drawbar. nice work, ron ginger ------- Re: YouTube video - making Tormach TTS-style toolholders on a Grizzl Posted by: "devers6" devers6x~xxcomcast.net Date: Fri Dec 3, 2010 4:20 pm ((PST)) Thanks for the kind comments. I have been doing quite a bit of explaining on CNCZone and YouTube regarding the relief on the shank side. I recognize that it is required to clear the part of the collet that projects from the spindle, and also to provide a positive registration surface against the spindle for accurate Z repeatability as well as tool support. I don't cut the relief mainly because I rarely use it. I never rely on the tool offsets, I just do the auto-Zero on the Z using the Mach3 macros. Most of my toolholders are for accessory tools like spot drills and center/edge finders, so holding power isn't the primary concern. But I do understand the value of the relief; and I figured anyone who felt they needed it would be able to add the extra facing cuts necessary to make it. It would likely take either a significant tool repositioning, or even a different tool altogether; and I just don't take the time. I appreciate all the feedback - I learned all I know from reading these groups and watching videos; and I am happy that I am able to give some of that back. I have a number of additional videos planned, covering the CNC conversion and electronics, more about the auto-centering tools, the pneumatic drawbar, and other enhancements I have made to my SX3 over the years. I hope you find them of interest as well. Dave ------- Re: YouTube video - making Tormach TTS-style toolholders on a Grizzl Posted by: "Jim S." mrjschmidtx~xxhotmail.com Date: Sat Dec 4, 2010 2:43 pm ((PST)) I agree that the undercut is an important feature on the Tormach system, but it is a bit of a bother to put on. Why not grind the end of a 3/4" collet back so it is recessed into the spindle slightly? The grind wouldn't have to be pretty, just out of the way. Then when you tighten the drawbar you get the holder bottoming without the need for an undercut. Seems to make sense, but it's been a long day. Let me know what you think folks. Jim (Just a guy who likes to build stuff) ------- Re: Mill engages on material/stock [SherlineCNC] Posted by: "timgoldstein" timgx~xxktmarketing.com Date: Sat Jan 15, 2011 9:18 am ((PST)) Scott Meyer wrote:---SNIP--- > You can use a end mill that is center cutting. Depending on the profile > and the part, sometimes it's necessary to plunge down into the part with > the end mill. You don't want to plunge straight down even with a center cutting end mill. They are not drill bits. As I was learning from Career machinist, they would use the term tool pressure when talking about plunging. Never meant anything to me and I continued the practice of straight plunges as it worked, but with funny noises. How I finally learned what they were talking about is as follows. I was using a 1/2" carbide 3 flt center cutting end mill in the Haas mill. The Haas is rated for 2000 lbs of thrust on an axis. I was plunging straight through a piece of about 5/8" thick Fortal which is a French made aluminum that is similar to a 7000 series alloy. So harder and less gummy than the normal 6061 stuff when machining. Plunges were all the way through at 10,000 rpm and probably something like a 50 ipm feed. For the machine, cutter, and setup that was all fine. After making a number of these plunges very successfully, I opened the doors and went to take the part out. All fine there also. But I found in the coolant tray that is on the front of the table some interesting bits. There were a number of lenticual shaped pieces of aluminum that were about 1/2" diameter and roughly .150 thick in the center with nice even convex faces that tapered to thin edges. I was baffled for a while where they came from. It was obvious they came from the plunged holes, but just were not making any sense to me. Then suddenly the light came on and I now had a physical representation of this tool pressure concept the pros had been telling me about. What was happening is as follows. The surface speed of the end of the mill varies from the outside to the centerline. At the geometric center of the bit there is no surface speed. As you go out it increases. OK, this is common sense and we all know that little bits have to spin a lot faster than big bits to cut properly. But it just never dawned on me that the same is going on across the face of a center cutting end mill. So the way these lenticular pieces were being formed is that the center of the bit was cutting through the material slowly. Closer to the edge a little faster and all the way to the edge the fastest. The machine had enough thrust to push and dimple the metal in the center that was not cutting in a downward direction so that the bottom of the plunge hole as it was being cut was flat. But if you looked at the bottom of the plate between the parallels the metal was bulging out. When the bit finally broke through the hole there was a .150" or so budge of metal in the center of the plunge hole and the edge of the bit cut through the edge of the hole. At that point the load on the budge was release and the center popped back from the flat form on one side with a large convex buldge on the other that was there while cutting to the nice even lens form I found in the tray. So there is my real world lesson on tool pressure. It was an eye opener. I got away with it on the Haas because of the stiffness of the big machine and the power it has. On a little machine it just flexes everything in the Z axis and angles the cutter in the hole. Makes a mess of everything. The moral of the story is I no longer plunge except with a drill bit that is made to handle it and has a wedge to push the metal out to where it can cut. Instead, I now ALWAYS ramp the bit into the part. For aluminum I ramp in at a 5 deg angle. For steel even more shallow. I like a helical ramp because it is cool to watch, but also use a back and forth ramp if there is no room for the helix. The important point is, never let the center of the tool stay in the same spot and move it far enough so the edge of the bit goes to where the center was. If there is not enough room to ramp, I either use a smaller bit or pre-drill and then plunge into the hole so only the outer 1/3 or so of the bit is cutting on the way in. Hope that helps some people see that issues with machine deflection and poor fidelity to the program can really be bad machining technique. Tim Goldstein A2Z Corp A2Z CNC division 3955 S Mariposa St Englewood CO 80110 720-833-9300 Toll Free 877-754-7465 www.A2ZCorp.us/store USA made accessories for desktop mills & lathes. Specialized No Mar tools for the jewelry industry. ------- Re: How do I machine a T-slots and dovetails? [sherline] Posted by: "Grif" kgriffitx~xxwolfenet.com Date: Tue Jun 21, 2011 7:37 am ((PDT)) > > I have been wondering about how to mill dovetails and slots and also > > T-slots for a while. Is this realitively easy to do with the Sheline > > mill? I have here a cross slide for a watchmaker lathe but it needs > > the topslide part made, which requires a brass block with a dovetail. >you need to buy or make special cutters. you can do on a sherline mill. >easier in softer metals. Don't forget, for T-slots, something that was really popular years ago, just mill the slot, and overlap it on top with strips to form the "T" and the surface of the table. Lots of screws, but no undercuts, just end mill work. ------- Re: How do I machine a T-slots and dovetails? Posted by: "imserv1" imservx~xximsrv.com Date: Wed Jun 22, 2011 6:05 am ((PDT)) To machine a Dovetail, you will want to get a mill cutter with the same angle as your dovetail They are accurately measured by using a micrometer and precision pins slid in the dovetail. Machinery's handbook has some instruction. T-slots are usually painful. I have made small to large, and in all cases you should plan to use plenty of flood coolant. I usually mill the channel with a cutter just slightly larger than the shank of my t-slot cutter, all the way to depth, then the t-slot cutter is removing the minimum material needed to finish the slot on each side. For one of my projects, I used a small, 45 degree dovetail cutter to deburr the inside-ceiling corners of the slot. I designed some parts with t-slots a couple of years ago that I could cut more aggressively than usual by milling the max width from the back side, leaving a .5-1.0" connecting section every 4-5 inches that had to be finished with a real t-slot cutter. This permitted me to hog out about 75% of the t-slot and just use the t-slot cutter for a an inch or so instead of for the full 12" or so of the slot I was cutting (this was a Sherline table sized t-slot). The only part of a t-slot that is used is the ceiling, so this method worked well for my application. Fred Smith - IMService http://www.imsrv.com ------- Re: How do I machine a T-slots and dovetails? Posted by: "Tom & Judy Bank" trbank1x~xxverizon.net Date: Wed Jun 22, 2011 9:04 am ((PDT)) Another way to do it in aluminum is to mill out the center slot and then do the T part with a Dremel flat edge cutter in six passes. Start with two passes down the center to get the required depth; then two passes over to the one side and two over to the other. Works, and I've done it, but not the way to go for a production shop. Regards, Tom Bank ------- Re: How do I machine a T-slots and dovetails? Posted by: "Ben" bens_groups2003x~xxyahoo.com Date: Wed Jun 22, 2011 3:20 pm ((PDT)) Hello all. Is it fair to say that a woodruff cutter is the same as a T-slot cutter? Regards Ben ------- Re: How do I machine a T-slots and dovetails? Posted by: "JERRY G" chieftoolmakerx~xxearthlink.net Date: Wed Jun 22, 2011 3:34 pm ((PDT)) No, or else there would not be two different names and /or applications. Woodruff cutters are used mostly on shafts to make seats for woodruff keys to drive pulleys and/or gears. T slot cutters form a slot to contain t nuts. Jerry G (Glickstein) P.S. Say, that is a good idea! I think I will post the question on my MEworkshop Group to see what response I get. ------- Re: How do I machine a T-slots and dovetails? Posted by: "Ben" bens_groups2003x~xxyahoo.com Date: Wed Jun 22, 2011 3:58 pm ((PDT)) Ahh ok, I though it was just a different name for the same thing like a UK vs US difference or something. I did notice in my book, the Amateur's lathe by Sparey, that he writes that woodruff cutters are used for cutting slots into shafts for keys but are mostly (!) used for cutting T-slots. That is why I was wondering it is is just the same thing with a different name. Regards Ben ------- Re: How do I machine a T-slots and dovetails? Posted by: "Steve Wan" stewanx~xxgmail.com Date: Wed Jun 22, 2011 7:03 pm ((PDT)) Hi Ben: Me again! T-slots are easy to mill on aluminium plates. I just finished making a 10" tee slot table for my monster mill last week. Only need a 6mm slot drill and a tee slot cutter of that same 6mm shank. Mill to actual dept and use tee-slot to open up the side grooves of 3mm width. Remember, no coolant at all, dry milling and a hand-held air pump to blow away the chips. Coolant will bind the cutter easily in those tight milling situations. As for dovetail cutting, I don't believe in getting a dovetail cutter unless the bevel is shallow. I would prefer using an angle vise. Those of cast iron made with angle scale at the side. Sherline angle vise is ok but the mill distance is restricted. Simply set the angle by looking at scale or use a digital angle meter. Always check with the mating part before mass producing in pairs. Hope these help again. Steve-S'pore ------- Re: How do I machine a T-slots and dovetails? Posted by: "Ian Newman" ian_newx~xxyahoo.com Date: Thu Jun 23, 2011 7:20 am ((PDT)) Hi Ben, Woodruff cutter and Tee-slot cutters are similar but not the same: Tee-slot cutters have a reduced parallel shank above the cutter which is small enough to fit in the slot of the Tee slot - see here: http://www.chronos.ltd.uk/acatalog/info_SCT071B.html A Woodruff cutter does not have a parallel reduced shank, but has a radiused reduction from the full shank diameter towards the cutter -- see here: http://www.chronos.ltd.uk/acatalog/info_WFF2.html This gives added strength to the Woodruff tool (or rather -- it weakens the tool to a lesser extent when compared to the Tee-slot cutter). Also, Woodruff cutters come in sizes to match standard key sizes designated by a number or letter code -- see here for the standard Imperial sizes: http://www.oldengine.org/members/diesel/Tables/Key6.htm or here for the metric equivilent: http://www.roymech.co.uk/Useful_Tables/Keyways/woodruff_keyways.html Ian ------- Re: How do I machine a T-slots and dovetails? Posted by: "Des Bromilow" desbromilowx~xxyahoo.com Date: Thu Jun 23, 2011 6:12 pm ((PDT)) Not the same, but in some production machines, a woodruff cutter has been used to make the T-slots (think Taig/Peatol) -- to learn what a Woodruff cutter is used for, google "woodruff key" and you will learn The two cutters look similar and are designed to cut on the periphery of the "disc", but main differences will include dimensions for the disc (diameter and width), and the "neck" which in the case of T-slots determines how much meat is left above the slot. All T-Slots and Dovetails are traditionally milled in the following sequence: Determine dimensions. Mill out narrow portion (Slot width and depth, or dovetail narrow portion and depth) with suitable finishing allowances. Then select appropriate "profile cutter" (T-Slot, or Dovetail) and mill out the undercut portion. A dovetail can sometimes be cut in multiple passes, whereas traditionally a T-slot is cut in one pass. You can make your own cutters based on materials, and tooling... I've seen photos of T-slot cutters ground up from broken drill bits, and I've used a dovetail cutter made the same way. There are other ways to cut dovetails including angled milling, flycutting, and shaping -- I've done one with a slitting saw into an angled piece of stock, but I allowed for the arbor in the design -- not pretty but it did work. As others have mentioned, built up methods are also an option. Des ------- Re: Creating a datum or reference on a casting [Min_Int_Comb_Eng] Posted by: "lakec_ah" Lakecx~xxearthlink.net Date: Mon Aug 29, 2011 1:00 pm ((PDT)) "hcrotalus" wrote: > Hey group, I am hoping someone can help me find a article on how to set up a datum or reference line on a casting from which to machine from. What's the process? I thought that I recently seen an article on this subject but now I can't find it. Does anyone remember seeing this article? Somewhere? Thanks Todd < In my limited experiance, the casting tolerances are way bigger then my machining tolerances, so any form of datum is usually the first thing machined into a casting. I usually pick a somewhat flat surface and machine it flat to create a datum, after averaging out how much my casting is off in various directions. You can leave tabs and other places in the casting to put a datum, but I don't trust the casting to provide them. Jeff ------- Re: Creating a datum or reference on a casting Posted by: "ED MAISEY" holmes_ca_2000x~xxyahoo.com Date: Mon Aug 29, 2011 1:46 pm ((PDT)) If you need the centre line of a cast hole make a wooden plug and whack it in, more detail, please. Edmund ------- Re: Machinable Wax Recipe [sherline] Posted by: "Gerald Feldman" gfeldman2904x~xxpacbell.net Date: Fri Sep 9, 2011 1:28 pm ((PDT)) For those looking for a recipe for machinable wax, here is a link to one. Other information is available using your search engine. http://www.weaponeer.net/forum/uploads/dcorb/files/2009-02-23_174227_mach inable_wax.pdf Jerry F. ------- Re: Normal vs Climb Milling [sherline] Posted by: "Ian Newman" ian_newx~xxyahoo.com Date: Tue Dec 20, 2011 7:40 am ((PST)) Curt Givens wrote: > Just about the time I think I've got my head wrapped around the concept of climb vs normal milling something will happen that makes me start wondering all over again. I've probably read Joe Martin's treatise on the subject at least a dozen times, think I "understand" then something happens. So I guess I need a really simple explanation. The Sherline mill turn clockwise viewed from above. With a piece of stock mounted in the vise is it right to left or left to right that is "normal" and is it front to back or back to front. Movement of the work piece. Does it matter if the end mill has its full diameter working or just part of it? Does it matter if it's on the front edge or back edge of the stock when it's removing metal? Am I right that if you are cutting a slot you are actually normal milling on one side of the slot and climb milling on the other? Or do I just totally not understand any of this? < Hi Curt: The terms "climb milling" and "normal milling" lose their intuitive meanings when applied to end milling. In the case of climb milling (or down cutting) the motion of the cutter tends to pull the work further under the cutter - the chip starts with a thick beginning and gets thinner as the tooth cuts towards the finished surface. This gives a smoother cut and a higher quality finish but the pulling action will take up backlash in a worn machine and cause sudden deep cuts which can damage work or cutter. Normal milling (or up cutting) pushes the work away from the cutter. The chips start thin and get thicker as the cutter rotates. This means that at the start of a cut the tooth is making a very thin cut and tends to rub rather than cut the work - this gives a less smooth finish to the surface. To translate the above into motion of the work: If you are normal milling, the cutter should cut with its right hand side when the work is moving away from the operator and the left hand side when the work is moving towards you. Width of cut: There are two types of end mill - in the USA these are called end mills and centre cutting end mills (in the UK they are called end mills and slot drills). Despite its name, the end mill is not designed to cut with its end (surfacing) - it is designed for profiling (cutting with its side). Slot drills have two or three flutes and can cut across the whole width of the cutter (i.e. they can cut a slot). The end mill (with four or more flutes) should not be used to cut a width greater than 1/4 of its diameter per pass. To understand the reasons for the above recommendations imagine a four flute cutter cutting a slot (so it is cutting the full width of the cutter). Picture the plan view of the job, the cutter rotating clockwise and call the direction of the slot being cut the "front" of the slot. As one of the cutter teeth cuts away the front of the slot, it will tend to bend the cutter to the left (looking at the plan view) and push the left hand cutter tooth into the side of the slot. This causes a very rough, lumpy and poor quality side to the slot and will place so much stress on the tooth tip that it is likely to break - this is why you should not cut a slot with a end mill (or if you do, use a cutter smaller than the width of the slot that you wish to cut and cut each side of the slot separately). The two flute slot drill does not suffer from this problem as when the front of the slot is being cut and the cutter flexes, there is no other tooth in contact with the slot sides. The advice to limit the width of the cut to less than 1/4 of the cutter diameter is to minimise the sideways flexing of the cutting tool and the associated problems. If you must surface with an end mill, remove the fragile tooth points by stoning a slight bevel on the tip of each tooth - it only needs to be very slight (see picture in the album "End Mill Tooth Chamfer"). Ian ------- Re: Normal vs Climb Milling Posted by: "shipmodelmaker1931" shipmodelmaker1931x~xxyahoo.com Date: Tue Dec 20, 2011 7:52 am ((PST)) Hi Curt, Contact me off list. I have a few pictures that will explain your concerns, (each one worth a thousand words) without filling your eyes and mind with confusing info, hard to grasp. Regards, Jerry G (Glickstein) chieftoolmakerx~xxearthlink.net Open 24/7 :) ------- Squaring a long piece of stock [taigtools] Posted by: "Shane Adams" adamsch1x~xxyahoo.com Date: Tue Mar 20, 2012 1:53 pm ((PDT)) Hi All - How would you go about squaring a long piece of stock: 1/2" x 2.5" x [6-10"] Would you just use a regular mill vise and square normally? Would you put supports on the parts that hang outside the mill? Shane ------- Re: Squaring a long piece of stock Posted by: "Stan Stocker" skstockerx~xxcomcast.net Date: Tue Mar 20, 2012 5:06 pm ((PDT)) Hi Shane, If your vise can hold the piece flat then you can proceed as your would for shorter work. Let just enough of the work extend from the vise to cut. The long tail extending from the vise shouldn't be an issue unless you start having really long pieces to square. If your vise doesn't have the clamping strength or rigidity for the work you can clamp the work to the table with supports. If you have a number of parts to make you can set up reference blocks to make swapping to the next piece quicker. Take care, Stan ------- Re: Squaring a long piece of stock Posted by: "alighazizadeh" alighazizadehx~xxaol.com Date: Tue Mar 20, 2012 6:30 pm ((PDT)) Hi. To square up any piece you will have to establish a datum to work from, fly cut a surface to get rid of imperfections and then flip the piece over on a set of parallels to fly cut the other side. Once this is done change over to an end mill and machine the sides square without disturbing the piece after fly cutting, once one vertical side is milled you can flip it on its side and use a try square against the milled side to bring it to true vertical and then mill the other verticals; if you keep it tight against the square you can get a very reasonable squared piece so long as your mill and the vise are properly trammed. Regards, A.G ------- Re: Squaring a long piece of stock Posted by: "Stan Stocker" skstockerx~xxcomcast.net Date: Wed Mar 21, 2012 4:29 am ((PDT)) Argh! For some clueless reason I misread your message as wanting to square up the END of the stock, not square it up all over. Please disregard my flat out wrong earlier response if you intend to square it up all over. You will need to decide how to hold the work, using a vise with the end hanging out isn't going to work very well :-) How you approach the job depends on the tooling available, and the starting shape of the workpiece. The largest flat faces need to be fly cut or leveled with overlapping passes of an endmill. You might want to make a nest style vise such as used by "Tryally". While the Tryally stuff is for sherline, it can be made in any size. He extended the floating style mill vise to make an adjustable nest. Once at least one of the faces is flat, clamp it down over parallels (square tool bits are good, just don't hit them with the cutter) and clean up the two long sides. You may have to shift clamps as you work. Square the ends at the same time, so the sides and ends will be square and parallel to the accuracy of the machine. Tryally vise pics at: http://tomwade.me/tw/machinist/slim_vise/other_sv.php Video at: www.youtube.com/watch?v=anxkL8bPLUw There are plans around somewhere, but a quick google didn't find them. Pretty self explanatory in any event. There are also homemade or purchased MiteeBite style edge clamps that can be useful for these sorts of jobs when combined with a tooling plate or purpose made holding fixture. Depending on the stock the order of operations can change somewhat. If one face is very close to flat you might just flatten it on a surface plate with silicon carbide paper and kerosene as a lubricant. Having one of the faces flat from the get go makes the rest of the operation go very smoothly. If the stock is so far from flat that you can't lap it then you have to use shims or whatever works to get the work to sit without rocking before clamping it down. If the finished part will have through holes, don't overlook the possibility of drilling the holes first, even undersized to allow final accurate boring, and using the holes for clamping studs. Hope this is more useful than my earlier response! Stan ------- Re: Squaring a long piece of stock Posted by: "alighazizadeh" alighazizadehx~xxaol.com Date: Wed Mar 21, 2012 11:14 am ((PDT)) Hi Shane, It is not difficult to do, have a look at the link below from this guy in Brazil and you will get the idea. http://www.youtube.com/watch?v=YsLhXwt8pX0 Regards ------- Cutting blind slots [taigtools] Posted by: "Paul J. Ste. Marie" taigx~xxste-marie.org Date: Sat Aug 4, 2012 9:29 pm ((PDT)) More adventures in the land of slot cutting: Having given up on drill-point mills, for the last two go-arounds I've been taking multiple passes with a conventional endmill--first plunging a cutter-cutting mill, and then by drilling a pilot hole at each end of the slot to avoid the center-cutting issue. Neither approach has been totally satisfactory. I've been getting a "stair-step" effect in the slots--the top 0.1" or so is about 0.010" wider than the next 0.1", and so on to the bottom of the slot, which is pretty much on size. I was initially blaming some side-to-side drift for this, but it happens even when the mill carriage is quite securely locked in place, and it's symmetric--both sides of the slot show the effect. Oddly, it also gets worse when I take shallower cuts. Taking cuts 0.050" deep show more of an effect than cutting 0.100" deep (this on a 1/4" wide slot). Any ideas? It's quite annoying. It's not the mill wearing down--I was using a TiN coated endmill and didn't see that sort of wear on the edges. ------- Re: Cutting blind slots Posted by: "ED MAISEY" holmes_ca_2000x~xxyahoo.com Date: Sat Aug 4, 2012 9:33 pm ((PDT)) Use a smaller slot or endmill if possible, Edmund ------- Re: Cutting blind slots Posted by: "Michael Fagan" woodworker88x~xxgmail.com Date: Sat Aug 4, 2012 10:18 pm ((PDT)) When you rough a slot and the cutter is taking passes on both sides of the slot at the same time, deflection is likely. Use a 3/16" endmill and take a 30 thou cleanup on each side of the slot at full depth. Climb mill if your machine and setup is sufficiently rigid. ------- Re: Cutting blind slots Posted by: "Ian Newman" ian_newx~xxyahoo.com Date: Sun Aug 5, 2012 1:12 am ((PDT)) Hi Paul, Before I start a word about my terminology - I'm in the UK and in this part of the world an end mill is never able to centre cut, what you call a centre cutting end mill we call a slot drill. Slot drills usually have two (sometimes three) flutes, end mills have four or more. For slot cutting you should never use an end mill - the four flutes make it almost impossible to cut a smooth side to the slot. To get a idea of the problem, imagine a four flute cutter cutting a slot (so it is cutting the full width of the cutter). Picture the plan view of the job, the cutter rotating clockwise and call the direction of the slot being cut the "front" of the slot. As one of the cutter teeth cuts away the front of the slot, it will tend to bend the cutter to the left (looking at the plan view) and push the left hand cutter tooth into the side of the slot. This causes a very rough, lumpy and poor quality side to the slot - this is why you should not cut a slot with a end mill (or if you do, use a cutter smaller than the width of the slot that you wish to cut and cut each side of the slot separately). The two flute slot drill does not suffer from this problem as when the front of the slot is being cut and the cutter flexes, there is no other tooth in contact with the slot sides. The usual recommendation is to limit the width of the cut for an end mill to less than 1/4 of the cutter diameter of the cutter, thus minimising the sideways flexing of the cutting tool and the associated problems. Attempts to cut both sides of a slot at the same time with an end mill often results in the corner of the tooth chipping off the cutter (due to the flexing/digging in problem) - this can be avoided by stoning a small bevel on the tip of each tooth. It need not be much, just 20 to 30 thou or so. All the best, Ian ------- Re: First time cutting metal [taigtools] Posted by: "Will Schmit" anchornmx~xxyahoo.com Date: Tue Feb 19, 2013 5:48 pm ((PST)) February 17, 2013 Rupert wrote: > Not really. The Taig is an addition to my manual mill. I got into CNC about a 1 1/2 years ago building a JGRO router table which gets a lot of use. I got a used CNC Taig last fall which I'm still leaning how to use. So far, I've only cut MDF on it. I figure it's time to use the Taig for what it was designed for- cutting metal. Besides, I'm finding this CNC stuff kind of fun going from a CAD drawing to watching the machine produce the finished product. < Rupert, I don't want to lead you astray (because my set-up is kind of unconventional), but the problems I encounter with 1/8" bits is deflection. There is a table in the machinist's handbook to identify the cut per pass. In theory, every time a flute passes, it should take out a known amount of material. The feed-rate should be advancing the tool at a rate in which it will be constantly taking the same amount of material. Because I am gun-shy about deflection, I say cut slowly, with a slowly rotating bit, and watch your chips. Your ears will tell if the bit deflects (chatters or sings), and your eyes will see a steady flow of well formed chips. Buy extra material, and experiment -- and sneak-up on the sweet-spot. ------- Milling Project [SherlineCNC] Posted by: "Thomas" tomdeanx~xxspeakeasy.org Date: Fri May 17, 2013 7:00 pm ((PDT)) I have a Sherline 4400 lathe and 2000 mill, both with DRO. I am not very skillful... Sorry, this is long and most likely wrong. I need to make an aluminum plate, similar to http://www.pierplates.com/products_2520.html. The installation diagram has some detail. Rather than purchase and modify this plate, I thought why not make it myself for 2x$ + 2xtime? I have 12" square 6061 AL in several thicknesses. If I can do it, onlinemetals likes my $. I have a rotary table. My plan is to practice on a thinner piece. 1. Drill a 3/8" hole in the center of the work piece. This is the reference point. It will later be opened to 1/2". 2. Attach the workpiece to the rotary table with a 3/8" bolt. 3. Mark 4 points at 90 degrees, within the diameter of the table for #10 screws. The initial position is not critical. These are 'milling marks' to firmly attach the workpiece to the rotary table. Remove the workpiece, drill the 4 holes for the #10 screws. 4. Mount the rotary table on the mill table. Zero the DRO to the center of the rotary table. 5. Mount the workpiece to the rotary table, using the 3/8" bolt and 4 ea #10 screws, washers and T-nuts. Use a 3/4 end mill (sic). Do everything 2x with 3/8 end mill. 6. At a radius of 7-1/4 inches, cut a 20 degree arc half way through the workpiece. At a radius of 7 inches, cut a 20 degree arc through the workpiece. At a radius of 6-3/4 inches, cut a 20 degree arc half way through the workpiece. I have exact numbers for each pass. 7. Rotate 120 degrees and repeat step 6. 8. Rotate 120 degrees and repeat step 6. Are there any gross errors in my plan? I have some drawings with more exact dimensions. This is the start of my plan. Most likely, when I finish, or, before I start, I will do a CNC conversion, like I have discussed before. ------- Re: Milling Project Posted by: "jowhowho" jowhowhox~xxyahoo.com Date: Fri May 17, 2013 9:18 pm ((PDT)) General principle: do as much as you can without removing and remounting the part. Make sure the planes of the XY table and the rotary table are perpendicular to the Z axis and the spindle. Play around using a large diameter fly cutter if you thing they are already aligned. You might be surprised. If you use a tool plate you can fasten your part with screws from underneath and leave it fastened until it is done. You'll also be able to drill and mill all the way through the part (as long as you don't run into your fixture screws. Sherline sells a round tool plate for the rotary table, or you can buy some MIC-6 and make your own. If you mill the center hole by rotating the rotary table, you'll be guaranteed it is concentric with the table and subsequent features. You may want to fly cut the material if you are using 6061. Go for CNC for sure, but you can do a lot with a rotary table on a mill. Justin ------- Tool Path Question [SherlineCNC] Posted by: "Thomas D. Dean" tomdeanx~xxspeakeasy.org Date: Mon May 20, 2013 8:35 pm ((PDT)) I have to cut a 7/8 inch wide 20 degree arc through a 1 inch 6061 blank. I will mount the work piece on the rotary table with a 3/8 bolt through the center and 4 #10 screws and T nuts. I plan to use a 1/4 inch end mill. Should I do something like use a twist drill to remove most of the material and finish with an end mill? Tom Dean ------- Re: Tool Path Question Posted by: "jowhowho" jowhowhox~xxyahoo.com Date: Mon May 20, 2013 10:57 pm ((PDT)) You said you don't have CNC yet, so ramping in to a pocket is not easy for you. You could use a center cutting end mill to plunge, or you could drill one hole in each pocket. Even with a non center cutting end mill, you can plunge a teeny bit, mill a path longer than the radius of the mill, plunge a teeny bit, and mill back to the original position. Repeat as needed. You should stick some scrap on the mill and make chips. ------- Re: Tool Path Question Posted by: "Martin Dobbins" trainnutzx~xxyahoo.com Date: Tue May 21, 2013 10:04 am ((PDT)) Hi Tom, A drill will remove material faster than milling, so it depends on how much time you've got/want to spend on the project. If you decide to mill it without drilling it, a two flute endmill running at high spindle speeds with light cuts will be the best bet on a slot; the largest endmill that will fit in the slot and leave some room for finishing will work better than using something as small as 1/4 inch end mill. Martin ------- Re: Tool Path Question Posted by: "KM6VV" KM6VVx~xxSBCglobal.net Date: Tue May 21, 2013 10:37 am ((PDT)) You can certainly do it on a rotary table. You have CNC? Then you could just mill the pocket. A little more work (normally you have to calculate by hand unless you have a 4-axes CAD/CAM package) but you can just just mill the pocket, or if it's a through cut, do an internal contour, and then you don't have to hog out all the material when using a 1/4" endmill. You don't have to use the rotary table, the CAD/CAM program can calculate it for you. Without CNC or the CAD/CAM package (manual calcs), the rotary table will simplify the cuts. Even with CNC, I still use my rotary table to make flywheels and to trim the 5" disks (1/8" thick) that I make for my robots. I wouldn't use a twist drill to remove material, unless you are manually drilling stock. Twist drills are not made to cut on their sides, just straight down. Alan KM6VV ------- Re: Tool Path Question Posted by: "Thomas D. Dean" tomdeanx~xxspeakeasy.org Date: Tue May 21, 2013 11:10 am ((PDT)) > Twist drills are not made to cut on their sides, just straight down. I know that. I was thinking of drilling holes through the material with a twist drill, would be faster to remove lots of the material and not be using an expensive end mill. Tom Dean ------- Re: Tool Path Question Posted by: "KM6VV" KM6VVx~xxSBCglobal.net Date: Tue May 21, 2013 11:29 am ((PDT)) I figured you might. I hate "cleaning up" the hole when I need to resort to that method. I just take it a little slower, and let the CNC do the job. Alan KM6VV ------- Finger Dimple for a radio tuning knob [taigtools] Posted by: "kiheiman_98" kiheimanx~xxq.com Date: Fri Jul 12, 2013 3:34 pm ((PDT)) I would like to add a finger dimple to a ham radio tuning knob. This would allow one to quickly spin the knob across the frequencies on the radio by using their finger to engage the dimple. I can machine a piece of 5/8" OD aluminum stock without any problem and I can drill the 1/2" hole for the dimple. I am not sure how I could get a nice "cup" like finish inside the hole. Kind of the reverse of rounding off the end of a piece of stock. Anyone have any ideas? ------- Re: Finger Dimple for a radio tuning knob Posted by: "Yi Yao" yix~xxyyao.ca Date: Fri Jul 12, 2013 3:57 pm ((PDT)) Do you have a ball nose end mill? It seems like the right tool for the job. ------- Re: Finger Dimple for a radio tuning knob Posted by: "Clint" kiheimanx~xxq.com Date: Fri Jul 12, 2013 4:07 pm ((PDT)) I do not have one, but could get one. I wondered if that would be the solution. Did not know if it would create a smooth finish. ------- Re: Finger Dimple for a radio tuning knob Posted by: "Yi Yao" yix~xxyyao.ca Date: Fri Jul 12, 2013 4:38 pm ((PDT)) Yes, its pretty easy to get a smooth finish with a ball nose end mill. Remember to rough it out with a square end mill first. You can also make your own cutter if you have the patience and experience to do so. Dean shows how: http://www.deansphotographica.com/machining/projects/mill/vise/vise3.html Scroll down to the 5th picture. He starts making a ball nose cutter there. ------- Re: Finger Dimple for a radio tuning knob Posted by: "Rupert" rwenig2x~xxxplornet.com Date: Fri Jul 12, 2013 4:38 pm ((PDT)) A ball nose end mill will leave a very nice finish. This can be done in a lathe also. We had to use the hand method using a normal turning cutter with a small radii to shape a ball and socket in school many years ago. The school project was the ball and socket on a small screw jack. Rough cut the dimple with a drill or machine it. Then shape a HSS cutter to a 1/4 ball shape and use it to finish the dimple. Works quite well but both lathe axes have to be worked together. Rupert ------- Re: Finger Dimple for a radio tuning knob Posted by: "Will Schmit" anchornmx~xxyahoo.com Date: Fri Jul 12, 2013 6:15 pm ((PDT)) It really depends if you are making one or many. I would make it on a lathe, then use the tailstock to hold a simple carbide router bit. I would also polish it with 600 wet-or-dry paper, then crocus cloth. If I were doing more than 10, I would just burnish them in the tumbler. ------- Re: Finger Dimple for a radio tuning knob Posted by: "Shawn Woolley" shawnwoolleyx~xxmac.com Date: Fri Jul 12, 2013 5:12 pm ((PDT)) Ive done that quite a bit for guitar amps I typically use a starter hole with a standard mill then finish it with just a fine round ball grinding stone -- slowly dropped down into the piece until it reaches the depth you want. Depending on the stone, you can get these like glass. ------- Re: Finger Dimple for a radio tuning knob Posted by: "Yi Yao" yix~xxyyao.ca Date: Fri Jul 12, 2013 6:12 pm ((PDT)) I've tried that too. I gave up after the aluminum totally clogged up the abrasive stone. ------- Re: Finger Dimple for a radio tuning knob Posted by: "Caparo" caparox~xxsaltmine.org.uk Date: Sat Jul 13, 2013 1:36 am ((PDT)) Hi, if I have to use a grinding stone on any soft material, I pre-clog the stone with soap (hard bar used for clothes washing or industrial bar soap for mechanics I find are best. Ladies' hand soap tends to be too soft for the job but can be used if re-application is not a problem. TTFN Caparo ------- Re: Finger Dimple for a radio tuning knob Posted by: "Pierre Coueffin" pcoueffinx~xxgmail.com Date: Sun Jul 14, 2013 9:48 am ((PDT)) To take tool marks of a dimple like that which has already been cut, I've sometimes used a wooden ball that fits the hole with a stick glued into one side, and an abrasive paste on the drill press. Valve grinding paste is a pretty good way to start polishing. You can get sub micron diamond pastes online that will let you polish up a hemispherical reflector for optical work if you want to put in the effort. Use a fresh tool and clean thoroughly every time you go to a finer grit. ------- NOTE TO FILE: This next conversation started about milling on a lathe but soon switched to milling tips that were fairly generic (for any dedicated milling machine, or any milling attachment for any lathe) and then switched to a discussion of milling cutters. Milling using a vertical slide on an ML7 [myfordlathes] Posted by: garthnx~xxpbt.co.za garthn444 Date: Wed Dec 25, 2013 4:13 pm ((PST)) Hi fellows, I'm trying to mill a 10mm deep slot in mild steel, 14mm wide, using an 8mm slot drill. Not working well at all -- actually, no idea of how to get this right. Should I cut very shallow depths, and at what RPM? lubricant? and cut the extra 6mm the same way? really unsure... Thanks Garth ------- Re: [myfordlathes] Milling using a vertical slide on an ML7 Posted by: "silverfoxccx~xxtiscali.co.uk" Date: Wed Dec 25, 2013 4:35 pm ((PST)) Garth, That was my m.o until I got more slot drills. I think my mill is stuck in either 255 or 500 Rpm. Had no problems at all since using plenty of cutting oil, got better results. Ron ------- Re: Milling using a vertical slide on an ML7 Posted by: "Andrew Curl" methuselahx~xxntlworld.com Date: Fri Dec 27, 2013 1:45 am ((PST)) Start in the centre of where you want the slot. A rule of thumb is to go half the diameter of the cutter deep, per pass. As you develop a feel, you'll be able to judge this sort of thing quite easily. Take the first pass, then move the slide up and then down, locking it, and taking second and third passes ("X" axis) close to the finished dimension, then take to full depth. For finishing to width, assuming that you've left only about ten thou., set the slide, lock it and climb mill. Usually you should feed the work against the rotation of the cutter, when removing small amounts climb milling will leave a better finish. Make sure that the vertical slide is locked whenever possible. Appropriate cutter speed would be at least 600 rpm; industry would go faster; but as usual, you cannot go too slow if a steady feed can be maintained. Lubrication when milling is a bit different to turning, in that a drip can or brush doesn't deliver enough fluid to wash the chips away (what you ideally want) and can actually hinder the process, so it's your call. I do almost all of my indoor milling dry, unless I'm working something sticky, like aluminium. Cutter life is shorter, but having the chips sticking to the flutes can shorten cutter life still more. Wear some goggles when milling. You are producing shards and splinters which you really don't want in your eyes, and if things go really wrong, snapped cutters can take eyes out from the other side of workshops too. Don't wear gloves near rotating machinery ever. Andrew UK ------- Re: Milling using a vertical slide on an ML7 Posted by: garthnx~xxpbt.co.za garthn444 Date: Fri Dec 27, 2013 3:36 am ((PST)) I am taking off .2mm at a time. If I try .5 or 1, there is serious vibration. I'm using my stepper motors to drive the lathe, I've tried cross slide speeds between .5mm and 2mm per second. Something I'm missing....or perhaps milling steel is just not something easy on the lathe/slide? I also don't see any method of locking the vertical slide -- should there be a bolt or something? (I have an original swivelling slide.) ------- Re: Milling using a vertical slide on an ML7 Posted by: "Andrew Curl" methuselahx~xxntlworld.com Date: Fri Dec 27, 2013 4:23 am ((PST)) Garth, small cuts are the ones most likely to take the edge off! For infeeds, I would suggest 0.15 or 0.2mm -per rev-. The myford slide I have is off a 254 (a biggun) but these things usually have a socket headed screw or two along the same side as the gib screws. Even the small ones. At a push, nip one of the gib screws up instead, and add locking bolts to your "to do" (with some urgency) list. Make sure that your cross-slide and your carriage are adjusted well, too. You can lock the carriage if necessary. Milling steel isn't as easy as brass or ally, but if your cutter is sharp, it shouldn't really represent a problem. Is your cutter in good order? Where did you get the steel would be another good question. Are you sure you haven't sourced some b*st&rd hard stuff out of someone's scrap bin? (As an aside, I wouldn't ordinarily mention this, but I have accidentally run cutters backward before now; they work remarkably well, considering -- what is your rig? Overhead drives are great for fluffing rotational direction.) Andrew UK ------- Re: Milling using a vertical slide on an ML7 Posted by: garthnx~xxpbt.co.za garthn444 Date: Fri Dec 27, 2013 4:45 am ((PST)) Hi Andrew. By .2mm a rev - at 1200RPM, would that be 4mm per second? Wow....perhaps that is the whole problem, I'm feeding in far too cautiously? (I calculated 1200 from Tubal Cain's book "Milling operations in the lathe" - (3.8)x(100ft/minute for free cutting MS) / (cutter diameter in inches). The cutter is a brand new 8mm slot drill -- it's a good quality (I think a Somta). The steel is free cutting from a reputable firm here -- it turns great. Also good quality... The lathe (ML7) is running in normal direction -- but as I am cutting a slot, the teeth would be cutting both against and with the movement of the work piece. No sign of any locking bolt -- I must add that. In the meantime, I am clamping to stop it moving -- seems to work fine (I wrecked one piece before I realised it was moving). Regards Garth ------- Re: Milling using a vertical slide on an ML7 Posted by: d.j.wilsonx~xxmac.com Date: Fri Dec 27, 2013 10:12 am ((PST)) On my slide, two of the gib strip adjustment screws are allen bolts, that I tighten up to lock the slide. ------- Re: Milling using a vertical slide on an ML7 Posted by: "Alan Moore" a.j.moorex~xxbtinternet.com Date: Fri Dec 27, 2013 12:31 pm ((PST)) Hi Garth, I think you are in the process of discovering why people buy milling machines. Trying to mill in the lathe with a vertical slide is a pain -- whatever you do, it is almost impossible to hold the work rigidly enough to avoid chatter. While I would hesitate to disagree with anyone as expert as Andrew, my experience has been that you can throw away all the normal guidelines of speeds and feed rates when milling in the lathe. It is just not rigid enough to take the strain. Regards, Alan ------- Re: Milling using a vertical slide on an ML7 Posted by: "Andrew Curl" methuselahx~xxntlworld.com Date: Fri Dec 27, 2013 4:02 pm ((PST)) Alan, I'm not an authority! I just write about what has worked for me. Drummond fan as I am, I eventually bought a MkII BCA miller. The chief problem, milling in lathes, as you quite rightly pointed out, is rigidity, or put differently, slideway area. Locking off all unnecessary slides helps, and a lot of work can be done this way if no other machines are to hand. Just got to take it easy. To this day, some of my most complex milling jobs were done on my lathe. It just takes a little more patience! Andrew UK ------- Re: Milling using a vertical slide on an ML7 Posted by: "Alan Moore" a.j.moorex~xxbtinternet.com Date: Fri Dec 27, 2013 7:00 pm ((PST)) Andrew, One other comment. If you absolutely have to mill in the lathe and you have one of the vertical slides which can be swivelled in the vertical plane, it is worth while drilling the base and putting in two taper pins or shouldered bolts to hold it accurately at right angles to the bed (you do 90% of your milling in this position). If you rely totally on the single bolt clamp you can find that machining forces will cause the slide to creep round to some angle and ruin your cut. How do I know this? Regards, Alan ------- Re: Milling using a vertical slide on an ML7 Posted by: stephen_vollerx~xxhotmail.com Date: Sat Dec 28, 2013 8:58 am ((PST)) If it's no good, you have to wonder why Myford persisted in selling the vertical slides. I appreciate it's not an ideal setup but we can't all run to a dedicated milling machine, be it on cost or room available basis -- I include myself in those scenarios. I have yet to try milling using my ML7, but have a double swivel vertical slide so will be giving it a go in due course. I am happy to take lighter cuts if it means I can achieve the result I desire. If it doesn't work out I guess there is always the option of selling the double swivel vertical slide again as they seem to fetch good money. Unfortunately I don't think a dedicated mill is viable for me but who knows what the future holds. Regards, Steve V ------- Re: Milling using a vertical slide on an ML7 Posted by: "Bob Hamilton" bobx~xxhamilton-bob.freeserve.co.uk Date: Sat Dec 28, 2013 10:00 am ((PST)) I have never used the vertical slide that came with my machine and would not consider myself to be even good with a miller, let alone expert. I would however offer some advice to anyone just “having a go” Probably the first thing to watch out for is the cutter grabbing and pulling into the cut. Climb Milling may indeed give a better finish as somebody suggested (I can’t say yay or nay to that) but is fraught with danger. I would always cut against the direction of travel, not with it. Small cuts may (or may not) cause cutter wear, but how much milling are you doing?? Lots of coolant / lubricant is doubtless desirable, as a makeshift device try compressed air to clear the cuttings. Never expect to get a perfectly sized slot with a single cut, expect to open it up with cuts to the sides. Wherever possible have the relevant slides either locked or at least tightly “nipped”. These machines are really quite amazing little things and very capable in the right hands, but lots of care is needed to get good results. I’m sure that nice modern CNC stuff works perfectly with only a degree in I.T. required to make them perform. I’m a “very old school” pre CNC guy. In fact as I am writing, it came back to me that some of the very old lathes that we had were fitted with screws on the cross slide that required the handle to be turned “WRONG WAY” that is counter clockwise to “go in”--------Can you imagine how many cock ups there were using them. Anyway, enough of all our yesterdays. Good luck -- just go steady. Bob ------- Re: Milling using a vertical slide on an ML7 Posted by: "David Littlewood" davidx~xxdlittlewood.co.uk Date: Sat Dec 28, 2013 6:27 pm ((PST)) Bob Hamilton writes > Never expect to get a perfectly sized slot with a single cut, expect > to openit up with cuts to the sides. This is certainly true if you use a 4-flute end mill, but if you use a 2-flute slot drill the resulting slot should be pretty well spot on, at least I have found it is when I've done it. This is all to do with the presence or absence of sideways thrust on the cutter, and this job is, after all, what slot drills are designed for. David Littlewood ------- Re: Milling using a vertical slide on an ML7 Posted by: garthnx~xxpbt.co.za Date: Sun Dec 29, 2013 5:18 am ((PST)) I found the slots to be quite neat - using a two flute slot drill. My concern now is speed and vibration - I think this is too much to expect from a vertical slide. I've made 2 parts out of 12 that I want (for a QCTP). Can a slot drill be sharpened? Is an 8mm slot drill overkill? Should I cut multiple times with a smaller slot drill? ------- Re: Milling using a vertical slide on an ML7 Posted by: "Andrew Curl" methuselahx~xxntlworld.com Date: Sun Dec 29, 2013 5:43 am ((PST)) Slot drills are for slots, they can be used for profiling, endmills are really for profiling only, they certainly cannot be used for plunging. Slot drills can be resharpened, the end faces can be done off-hand if you have a good eye, the flutes require a special machine- a T&C grinder. These can get expensive, or you can make your own, like the "Quorn" the "Stent" and others. 8mm should not be an overkill, but there are these wonderful three flute cutters that can profile and plunge called FC3s. They are only made to a maximum of 1/4" or 6mm, they are solid cobalt, and the idea of them is that they are so cheap (for industry) that they are not actually worth resharpening -- they are also known as throwaway cutters. I use them a lot! The smaller diameter means higher rotational speeds and more passes -- that's all. Their shorter length (read: minimal overhang) helps rigidity. They can be had with extra length flutes, ball noses and such, just like their bigger brothers, and can offer the best of both worlds. If you have more money, Clarkson make their "Premium" 3 flute cutters too. They have the same 3-flute configuration, but come in bigger sizes, with the usual threaded shanks instead of a clamping flat. It's worth noting that half the reason that the "Quorn" was designed was to resharpen FC3s after all. Andrew ------- Re: Milling using a vertical slide on an ML7 Posted by: stephen_vollerx~xxhotmail.com stephen_volleruk Date: Sun Dec 29, 2013 7:18 am ((PST)) Thanks Bob, I will go carefully, and of course you can only learn by trying. Regards, Steve V. ------- Re: Milling using a vertical slide on an ML7 Posted by: johnx~xxstevenson-engineers.co.uk Date: Sun Dec 29, 2013 5:07 pm ((PST)) Andrew, Not so fast, what you are quoting is classic Chapman but things have moved on and the manufacturers haven't kept to any standard. You can now get center cutting 3, 4, 5, and 6 flute 'end mills' or if they are center cutting should they be called slot drills? Doesn't help that they call they different names on the same page of the catalog!! I took a chipped 20mm carbide end mill in for resharpening, it was the classic one with the hole in the centre. When it came back it was center cutting, no hole and one flute over center. These new 5 and 7 axis tool and cutter grinder have rewritten the book, only problem is there hasn't been any new books for 50 years ------- Re: Milling using a vertical slide on an ML7 Posted by: "David Littlewood" davidx~xxdlittlewood.co.uk Date: Sun Dec 29, 2013 6:38 pm ((PST)) johnx~xxstevenson-engineers.co.uk writes >You can now get center cutting 3, 4 5, and 6 flute 'end mills' or if >they are center cutting should they be called slot drills ? The problem with this is that if the cutter has more than two flutes, there will be a sideways force on the cutter edge as it removes metal, so the extra teeth at the side will remove some metal, so the slot will be displaced slightly. This displacement will depend slightly on the speed and depth of cutting, and drastically if you traverse in the reverse direction. The effect has nothing to do with the presence or absence of a centre cutting tooth. The result is always, to a greater or lesser extent, a slot which is over-width, displaced, ragged, or all three. With a two flute cutter, there is no cutting tooth in contact with the side wall when the sideways force is applied, so these problems do not exist. This was explained very clearly by G H Thomas in his "Workshop Manual". David Littlewood ------- Old Kit, New to operating it?? [myfordlathes] Posted by: "Bob Hamilton" bobx~xxhamilton-bob.freeserve.co.uk Date: Mon Dec 30, 2013 1:38 am ((PST)) While I certainly have no argument with the positives / negatives of obtaining accurately sized slots using slot drills against end mills. My comments were really aimed at someone with possibly limited experience and with old / unfamiliar kit. I have found that people that know "THINGS" and this covers a multitude of "THINGS" forget that newcomers find "Everything difficult"---------Myself included. Mistakes are often made in the final stages of making "THINGS" and slots for keys are a classic. It would make sense to me, to test run a cutter and size up the result if unfamiliar with.the setup, but failing that, an undersized cutter will allow some "adjustments" to be made. I think that my background has generally been with old machines that were often far from accurate and a large amount of operator input was required, so the above would be the sort of thing that was required all of the time. Not quite here yet, but-------Happy New Year to one and all. Bob ------- Re: Milling using a vertical slide on an ML7 Posted by: "Andrew Curl" methuselahx~xxntlworld.com Date: Mon Dec 30, 2013 8:16 am ((PST)) True enough, John. I like to think my references are a bit more recent though! I have the Caxton books (A.W.Judge c.1948) but I was thinking more along the lines of my Buck and Hickman/ Cromwell Tools catalogues, and the cutters I tend to buy and use, which are a bit more up to date. Please bear in mind that when I use my lathe or my BCA, I seldom use more than a 5/8" diameter cutter (the BCA can't hold a threaded shank bigger than 3/8") although I do use shell mills upto 2" on the Drummond. For facing. Whilst I have seen a 6-axis Walter CNC grinder in action (frightening!), cutters of those sorts of sizes and numbers of flutes are hardly applicable to little machines. I have a couple of half inch six fluters, but to give an idea of their age, thay are on morse taper shanks, too. They're new-old-stock as well, boxed and labelled as such, and not modified reamers. I am still not convinced that a six or seven flute endmill, regardless of the gashing applied can truly plunge without an awful lot more pecks that a two flute slot drill, either. I save the "big" stuff for my Bridgeport. Even then not that big- when you've served your time with Parksons, they seem pretty whippy! Andrew ------- Re: Milling using a vertical slide on an ML7 Posted by: garthnx~xxpbt.co.za garthn444 Date: Tue Dec 31, 2013 5:23 am ((PST)) I'm having much more success with a smaller (5mm) slot drill than the 8mm. Same design, two flute. When I bought it I asked for the technical specs for cutting and am using those, 1800RPM and feed of a little more than 1mm per second (for free cutting MS). I am managing 1mm depth, 2 causes too much vibration, but 10 passes x 4 (to get 10mm x 14mm) is a lot better than 100 x 2. I'm unsure exactly of how to lock the slide -- I don;t see locking screws on any of the photos I have found of vertical slides. Locking the screw means that the backlash is still a factor. I don't want to start drilling holes in the slide until I'm sure about this... ------- Re: Milling using a vertical slide on an ML7 Posted by: "Bob Hamilton" bobx~xxhamilton-bob.freeserve.co.uk Date: Tue Dec 31, 2013 8:26 am ((PST)) Can you just nip the slide adjustment a bit more than normal on both the lathe and the vertical slide. Also have the feedscrews adjusted neat so as to remove as much backlash as possible Are the lathe headstock bearings OK.??? Plenty of lube to help with any play. Put a DTI on the chuck and a bit of timber underneath as a lever to test. I’d have thought an 8mm cutter used a bit gently would have flown through free cutting mild steel. 1800 rpm does seem a touch fast to me, but that should help in other ways. What is it that you are trying to make?? Bob ------- Re: Milling using a vertical slide on an ML7 Posted by: garthnx~xxpbt.co.za garthn444 Date: Tue Dec 31, 2013 9:15 am ((PST)) I suspect my main problem is that although my machine vice (mounted on the verticle slide) is fairly heavy (good), it has considerable overhang (bad). There is just a lot of vibration. I've tightened up all gib strips as much as I can without them jamming. My main bearings are good, I reshimmed a while back and there is no detectable play. I'm making these http://homews.co.uk/QCTH2-04.pdf The precision is not a great factor -- they are coming out alright, just taking a long time to mill. ------- Re: Milling using a vertical slide on an ML7 Posted by: "Kevin" tadpolex~xxbtinternet.com klokenz Date: Tue Dec 31, 2013 9:47 am ((PST)) Hi Garth, I use my vertical slide fairly often for milling operations, though always on a rather small scale. For removing much metal you have to take it gently, as you've found. The vertical slide enables you to do milling operations in the lathe, but doesn't convert the lathe into a milling machine! The standard Myford vertical slide doesn't have locking screws as such, so yours isn't missing anything. Regard the vertical adjustment as a means to set the workpiece to the required height _between_ passes of the cutter. Since it will not be used _during_ a pass the gib adjusting screws can be nipped up tighter. I used to just nip up one of them, leaving the others to take care of free movement when I needed to move up or down. Later, for many years, I used to fit a small G clamp to secure the two main parts to each other. As I recall I had a small shaper spacer to go under one jaw. It did not look at all elegant, but was very practical! Later I got around to fitting a single locking screw. It's an M4 socket head screw that presses on the gib. I would not want to use anything larger as it goes into cast iron, and I worry about applying too much "wellie" and spliting part of it out. Maybe I'm worrying unnecessarily, anyway the M4 serves my light duty needs. Sometimes, in fact often, you can do without the vise. As an example, make up a piece of 25mm square with a couple of holes near the ends for Tee screws to clamp it firmly to the vertical slide. Then fix the workpiece to that with toolmaker's clamps, or by putting screws directly into it. Regard it as disposable, though it will last for many jobs. Even better if the work allows is to clamp directly onto the face of the vertical slide. Kevin, NW England, UK ------- Re: Milling using a vertical slide on an ML7 Posted by: "Cliff Coggin" clifford.cogginx~xxvirgin.net Date: Wed Jan 1, 2014 3:30 am ((PST)) My ML7 vertical slide has three gib locking screws in addition to the three adjusting screws, though whether they are original or fitted by the single previous owner I know not. Despite that, the whole assembly is much too flexible for serious milling operations. I have milled brass and aluminium in it after a fashion, but don't entertain the idea of milling steel. Cliff Coggin Kent UK ------- Profiling hot rolled steel plate [TAIGTOOLS] Posted by: "Kyle Setchel" kylesetx~xxgmail.com Date: Sat Feb 15, 2014 2:40 pm ((PST)) Hi. Long time group stalker, first time posting. FYI, I'm a computer guy, who is learning machining, and still very much a newbie. I'm a hobbyist with a taig cnc mill running mach3. I'm profiling some 2D parts out of 3/16ths hot rolled steel plate. I think I'm looking for recommendations on end mills, and probably DOC, speeds and feeds. The edge finish isn't important.. here comes observations! I've been using 4 flute square endmills solid carbide (11/64 diameter) with using the max spindle speed for the taig pulleys. I find that it just generates way too much heat, and manually applied oil requires too much attention, as I have to apply it constantly. I'm making DOC of 0.015" and doing 1.5 IPM plunge and 3 IPM feed rate. I find that I can get away with slightly higher feed rates when doing straight lines. I'm constantly blowing away chips as well. It just gets really hot (150F with the infrared gun), and I think it is heating up the headstock and causing it to grow and that moves the endmill so that it isn't perpendicular to the stock anymore, thus causing the cutter to work harder, and generate sparks and more heat. Vicious cycle I tell you! What do I do? Use different cutter, RPM, speeds and feeds or what? I don't want to constantly apply lubricant through the whole job if possible! Thanks in advance guys! Kyle from Atlanta, GA ------- Re: Profiling hot rolled steel plate Posted by: luv2bsailinx~xxyahoo.com Date: Sat Feb 15, 2014 4:49 pm ((PST)) Lighter cut, lower RPM, faster feed. ------- Re: Profiling hot rolled steel plate Posted by: "Don Rogers" Donx~xxCampbell-Gemstones.com Date: Sat Feb 15, 2014 7:37 pm ((PST)) It's been a number of years, decades actually since I've cut hot rolled steel. I seem to remember that it was best to skin it first, IE take a light cleanup cut with a fly cutter on both sides, or in our case in the big Tool and Die room, over to the surface grinder and skin it. The reason to skin it was that enough carbon was picked up during the heating and rolling to put a very thin case hardening on the steel. Second observation, I would not use carbide mills, but rather HSS ones, the fresher the better. Check the feeds and speed chart and software for the chip loads and speeds. Any time you are generating sparks, it is time to quit cutting and 1. check the tram of the mill, and 2. replace the mill, it is shot. There are a lot of hot rolled steel types. If I remember right, most tool steel is hot rolled. So is boiler plate. Two quite different animals. If it is tool steel, or a type of steel that you can heat and quench harden, then with the heat you are generating, that is causing sparks to result, it is doing an effective job of hardening the surface of the steel as you are cutting it and the next flute that enters the cut is now trying to cut hardened steel. The next revolution, the dulled cutter now generates more heat and as you continue cutting. Boiler plate is basically a mix of steel scraps as I was told on my apprenticeship. I know that drilling and tapping was a real hit or miss event. Lots of dulled drills and broken taps in the process. You should also consider a coolant. It is a problem on the Taig as there is no gutter on the table, but it can be done. Something like a cool mist can help. Don ------- Re: Profiling hot rolled steel plate Posted by: "Stan Stocker" skstockerx~xxcomcast.net Date: Sat Feb 15, 2014 7:59 pm ((PST)) Hi Kyle, Drop the spindle RPM way the heck down. You can bring it up later, but I'd try playing in the 600 to 1100 RPM range to work out the process. Next, increase your depth of cut. I'm pretty sure you're rubbing and recutting chips more than you're removing metal from the plate as things are now. Listen to the machine. If your machine allows pure manual use, play around and get a feel for the spindle speed and depth of cut. If you want to calculate chip loads and such using machinery handbook or other calculators/tables that's great, but remember those tables are for industrial applications with spiffy stuff like flood coolant and big rigid machines. I expect to drop to around 50% of the calculated feed rate OR DOC and spindle speed with lighter machines. Not to be too repetitive, but LISTEN to your machine. It will tell you if it's being strained or not cutting consistently once you learn to listen. You mention 1.5 IPM plunge. Most 4 flute end mills aren't end cutting, they can't plunge. Sure you can lower them into an edge up to the width of the end edge, but the center of the end mill doesn't end cut. There are end cutting 4 flute mills, they will have one pair of edges that meet in the center like a standard 2 flute style, the others will stop clear of center. Most 4 flute mills have all the edges stop before center. You can profile and pocket with ramp down, but you can't plunge or poke holes :-) Hot roll can be interesting to cut if the mill scale is on the plate. Most purchased from suppliers is descaled, but sometimes it's nasty stuff. The cut quality may not be functionally important for the part to work, but it tells you whole lot about how well your machine is working. Cast a really careful eye over the endmill, it sounds like the thing may have been damaged a bit, or not all that good to start with. Merely being carbide means little, being GOOD carbide means something. You can do great work on an OK mill with quality endmills, but plop an interstate HSS or some "quality import carbide for $4.00" budget endmills into the spindle of a super fine heavy duty mill and watch the cut quality go in the toilet. Get a tip proof container and fill it with good cutting oil. Use a flux brush and lay a layer of oil over the cut area. Use a chip brush to clear swarf as it builds up, recutting chips is rough on finish, wastes spindle power, and wears the cutter. Use the flux brush to add oil as needed. Listen to changes in the sound of the cutting action. Flood cooling is a mess, many won't use mist for health reasons, but some lubricant is just a requirement when machining steel. Particularly low carbon possibly mystery origin steel like the "made in one or more of the following countries" on the racks at Lowes or Home Depot. And some steels just look like rats with carbide teeth gnawed on it no matter what you try. Good luck, Stan ------- Re: Profiling hot rolled steel plate Posted by: "Larry Guthrie" yrralguthriex~xxgmail.com Date: Sat Feb 15, 2014 7:57 pm ((PST)) Cold rolled steel produces better surface finish, better dimensional stability and work hardens the surface. Hot rolled steel has a poor surface finish and I don't believe it hardens the steel. It is also not stable dimensionally. If you take a surface cut on one side of a flat the hot rolled will tend to cup. ljg ------- Re: Profiling hot rolled steel plate Posted by: "Stan Stocker" skstockerx~xxcomcast.net Date: Sat Feb 15, 2014 8:15 pm ((PST)) Hi Larry, If the cold rolled is annealed and normalized this doesn't apply, but it's usually cold rolled that turns into a pretzel when you slab off one side and leave the original rolled surface opposite. Hot rolled is pretty stress free stuff, it isn't squeezed and squished like CRS. Not pleasant to work in most cases, but fairly stable. Take care, Stan ------- Re: Profiling hot rolled steel plate Posted by: "Mike Rehmus" editorx~xxmodelenginebuilder.com Date: Sat Feb 15, 2014 8:09 pm ((PST)) Try a 3-flute end mill, it cuts smoother than a 2-flute but doesn't drag the chips around like a 4-flute cutter. If you have shop air, just blow onto the junction of the cutter and the work. It will keep things cool and blow away a lot of the swarf. Or use a very light mist of coolant if you want that help in keeping the cutter in better condition. I found a continuous air blast to be most effective. Hot rolled steel doesn't distort as will cold rolled steel because the surface has not been work hardened by rolling it cold. But you said you are profiling which cuts around the edges, not on the general surface of the work so that should not be a problem regardless of the type of steel as long as your sections don't get too small. If you are moving the head on the mill, then you are pushing too hard. Blue, hot chips are OK but sparks mean you are cutting too fast. Best regards, Mike Rehmus Editor, Model Engine Builder (TM) Magazine www.modelenginebuilder.com Log onto our Web site and sign up for our free newsletter. ------- Re: Profiling hot rolled steel plate Posted by: "Don Rogers" Donx~xxCampbell-Gemstones.com Date: Sun Feb 16, 2014 2:21 pm ((PST)) The Taig Z axis ways are made from hot rolled steel. Cliff and I had a talk about it one day as I found my original way had developed a twist. The wide piece. I had ordered a new one and it was actually worse than the first. You could see where they had Blanchard ground the scale almost off and some of the finish grind didn't clean up OK. I had a 0.004" Curl in the first two inches. Cliff quickly sent me a replacement which was dead on. In the conversation, he mentioned that they use the hot roll because it is more stable, but less expensive than normalized steel would be. He also mentioned that it was all but impossible to get the ways exactly flat, but they should pull flat when tightened down. Makes sense when you consider that they are held down on a magnet table to surface grind them and a slight warp will be pulled flat, but when you turn off that magnet, the warp will come back. Flip the metal over and clean the other side and the same thing happens again. To some extent. Don ------- fly cutting cast iron [SherlineCNC] Posted by: nilrodsx~xxyahoo.com Date: Tue Mar 25, 2014 9:13 am ((PDT)) Been lurking for a while and thought I would throw this one out to see what others are doing. I was fly cutting some cast iron the other day and ran into some issue and wanted to see how everyone else was doing it. The speeds and feeds on sherlines site seem to be quite different for insert vs regular fly cutter, at least what I could find. Setup is a A2Z CNC monster mill with a fly cutter (not insert one) with carbide lathe bit. I was running about 1/4 speed and about 3in/min feed rate and about .004 depth of cut per pass. When it was just taking off a few spots here and there it was fine, but when it got down to doing the full area it started to shake like crazy and I had to increase speed quite a bit to get the vibration to stop. I was able to get it finish but the finish was not great like I see on other materials. I tried adjusting speeds and feed rate a little but didn't help much. What sort of speeds and feeds are others using to fly cut on cast iron? Any thoughts would be helpful. Thanks, Chris ------- Re: fly cutting cast iron Posted by: baboonhead11x~xxyahoo.com Date: Wed Apr 2, 2014 3:52 am ((PDT)) Assuming your workpiece is tightened, yeah it could just be due to the fact the machine isn't very rigid. I'd probably try keeping the feeds and rpm the same and lighten up a bit more on the depth of cut. Also, you may be having your fly cutter too far out (large radius) so you may want to play around with the feeds and speeds? ------- Re: fly cutting cast iron Posted by: nilrodsx~xxyahoo.com Date: Wed Apr 2, 2014 9:33 am ((PDT)) Ok. that is kind of what I was thinking too, it is a little more rigid than a std sherline mill, but not that rigid you're right. The material was definitely tightened down. There was no movement of it at all while cutting. As for the radius I think it was only out about 1 1/2- 2" on the radius, so not too large. Anyway thanks for the thoughts. I figured I would just see what others had run into. ------- Re: fly cutting cast iron Posted by: russellcupanx~xxyahoo.com Date: Wed Apr 2, 2014 3:49 pm ((PDT)) Chris, here are some things that may need to be considered. I'm guessing at some of these, as they were not mentioned in your original posting. Don't use any cutting fluid or coolant. That means things are going to get dusty/dirty so you may want to think about positioning the nozzle of a shop vac near where the cutting action is taking place. Get below the "skin" of the casting as quickly as possible. If the castings are generous enough, you could try to get to good material by removing the skin with a belt/disk sander. If that's not practical, increase the depth of cut as much as possible. As deep as .05 inch on the first pass if you can. Depending on the quality of the casting, there could be sand still imbedded near the outer surfaces, so that's why you want to go deep. With a single point tool and a cutting diameter of 2 inches, the feed rate may need to be around a half inch per minute, and the spindle speed at around 1/2 on the dial. That would keep the chip load fairly light. You mentioned a poor finish on the part when done. It's possible the carbide on the tool bit got chipped when the .004 deep cuts were being made through the skin of the casting. I hope this helps. It's been a long time since I milled cast iron. There are reference materials and charts that give you the cutting speeds of various materials and the chip load that the cutter should see. The charts allow for cutter diameter and the number of flutes on the cutter. On our small machines, chip load should probably be limited to .002 of an inch. Russ (another lurker) ------- Re: fly cutting cast iron Posted by: nilrodsx~xxyahoo.com Date: Wed Apr 2, 2014 4:06 pm ((PDT)) Russ, Good thoughts. I did forget to mention I wasn't using any coolant, not for cast iron. Yeah it was messy. It was an odd one since I was milling a boss about 1 1/2 inches tall off a casting. Actually I started with about .003 DOC and the finish did look better, but I was still probably running too high a feedrate. Everything I kept reading kept saying to have a fairly heavy chip load while fly cutting and increasing it did remove the material faster so I kept going. Sounds like I may have been doing it closer to right when I started, just too fast. I had run the calculations off the machinist reference but I know those are meant for larger machines and they always come out so high I could never use them on my small mill. The recommendations were so different on the sherline site for the plain fly cutter vs the insert one and what I had was kind of in between (had carbide bit but larger radius). I checked the tool bit and didn't see any chips, thought the same thing myself when I really start hogging material. Just nice to bounce ideas of some other folks to see their experiences. Hopefully this will help someone else down the line. Thanks ------- Re: fly cutting cast iron Posted by: baboonhead11x~xxyahoo.com Date: Wed Apr 2, 2014 5:04 pm ((PDT)) I haven't fly cut cast iron specifically, but I've done so on a wide variety of steels and plastics and yes there were 1 or two cases of manually doing it where I was overly aggressive trying to hog material and the cutter got stuck where the spindle stops spinning because it doesn't have enough power. The spindle simply doesn't have enough power like you would expect in a proper machine. The fact it's not rigid means while it could do some cuts, it vibrates a lot, because the cutter really isn't doing full depth cuts since it's flexing around. So while you're meant to go low feeds and speeds, you just don't have that torque to make the cut according to what tables say. Really I found either you reduce depth of cut, and basically work on cutting the work hardened area (which the carbide can handle anyway), or you can maybe try to spin the rpm faster and lighten up on the feeds so get finer swarf. So to sum up my experience, the spindle is not powerful enough and the machine not rigid enough to really hog material, particularly when you are using the large fly cutter with the large radius that provides a much larger countering torque to the motor's applied torque. You can maybe use the carbide insert cutter and get better results. Or if you stick to the large diameter fly cutter, my solution was to lighten the depth of cut basically. For some steels and stainless that work hardens, I still just let it cut low depth and basically work the work- hardened area (carbide tips can handle it). There was no other alternative because the machine isnt able to undercut the work-hardened area for those stainless steels. Granted, cast irons don't work harden so at least you don't have that issue to worry about yet! ------- Re: fly cutting cast iron Posted by: baboonhead11x~xxyahoo.com Date: Wed Apr 2, 2014 5:07 pm ((PDT)) Oh, another way to tackle a better finish will be not doing full face engagement. I do something around 60% radial engagement and then finish the whole surface off that way. Rather than take on the whole surface with one facing pass. BTW, if you don't have the carbide insert cutter, you could also try to lower the radius of your bar fly cutter by shifting the carbide tipped bar backwards a little. If you reduce your cutting diameter, your machine's torque can better handle cuts. ------- Problems with Vibrations [SherlineCNC] Posted by: pramodishax~xxyahoo.com pramodisha Date: Mon Jul 28, 2014 12:38 am ((PDT)) Hello Friends, I am based in India and am using sheline CNC lathe as well as CNC Milling Machine. I have mounted the lathe on a small computer table while mounted the Mill on a table made from steel angles and plywood top. My workshop is on the 3rd floor and the problem is that I get vibrations and sometimes while using a big cutter (6 mm), the vibrations create quite bigger noise and vibrations on the floor, which even goes to the people living just the floor below me. I cannot lay foundation on the floor. So what alternatives do I have? Shall I use anivibration pads just between the machine and the plywood top of the table? If yes, then how to keep the machine leveled and straight? Please suggest alternatives. I would also appreciate suggestions for lessening the lathe vibrations also. Also suggest whether using counterweight for the Z-Axis be mush useful? Thank you all for reading my post and Thank you in Advance for helping me out. Pramod Agrawal ------- Re: Problems with Vibrations Posted by: "Mike Bauers" mwbauers55x~xxwi.rr.com Date: Mon Jul 28, 2014 12:56 am ((PDT)) Welcome, Pramod, May I suggest placing the anti vibration pad on the surface of your plywood tabletop and mounting your mill on another piece of plywood that rests upon the mat? Your metal legs are possibly transmitting the vibrations as well. You may wish to make some sort of wooden cups to place between the legs and the floor and line either the inside or the base of the cups with thick felt to further dampen the vibrations. Mike Bauers ------- Re: Problems with Vibrations Posted by: "Rex Burkheimer" burkheimerx~xxgmail.com Date: Mon Jul 28, 2014 5:17 am ((PDT)) I would say if you have vibrations at that level, you should revisit your feeds and speeds. Besides the issues mentioned, that can't be good for your machines. Assuming you are working within the limitations of your tools, the best way to reduce vibration is with mass. If your table will support it, consider adding a slab of steel under the machines. You could also pour a small concrete pad on top of your bench, and possibly at the base too. Level is secondary, especially in these small machines. It is useful for some setups on the mill, but has no real effect on the accuracy. Rex B - DFW ------- Re: Problems with Vibrations Posted by: jowhowhox~xxyahoo.com Date: Mon Jul 28, 2014 12:05 pm ((PDT)) My machines are mounted on 3/4" aluminum plates. The mass and stiffness of the aluminum eliminates most noise and vibration. I also have very heavy work bench tops -- 2-1/2" of plywood and Masonite. If you don't have big chunks of aluminum, try a few layers of plywood. Rubber feet help too. The most efficient way to help the motor lift the weight of the head is with a spring. A counterweight would double the mass and stress the screw and motor during acceleration. You might also want to balance the head with a long, rigid moment arm so the accelerated head doesn't try to rotate on the ways and bind them. The center of gravity of the head, optimally, should be near the ways. The longer the moment arm, the less it has to weigh. If you solve the imbalance and weight issues half way, or so, you can get a big improvement without too much work. Start conservatively -- most people get by with nothing but proper lube and adjustments. ------- Re: Problems with Vibrations Posted by: "toolznglue" toolzngluex~xxsbcglobal.net Date: Tue Jul 29, 2014 6:03 am ((PDT)) Rather than a piece of plywood, I use two pieces of 3/4" MDF glued together to form a 1 1/2" thick base. The piece I use for the lathe is framed in oak hardwood - the hardwood glued to the 1 1/2" sides of the base prevents oil from getting into the MDF - and covered with a laminate (trade name is Formica - there are others). The hardwood sides and MDF bottom are varnished to protect them from moisture and oils. For the Mill, construction is the same except that the top is covered with a piece of 0.032 inch thick steel. The steel provides a magnetic surface to hold the magnetic chucks used to hold dial indicators, etc. The cabinets are sized for the Sherline products (2000 mill & 4400 lathe) and have space to hold either tools or raw materials. The mass of the raw materials or other tools helps to provide additional mass to dampen any vibrations. Jerry Jankura So many toys.. So little time. ------- Why the general lack of full enclosures? [SherlineCNC] Posted by: baboonhead11x~xxyahoo.com baboonhead11 Date: Mon Dec 8, 2014 10:54 am ((PST)) I've been scrolling through the pictures and videos of related setups from people. Some people have really nice setups and workshops worthy of envy. But one thing I noticed is very few have full enclosures for their CNC mills. For a manual mill or lathe, I understand as you need to get your hands in there to crank wheels. For CNC, why not have the enclosure to keep dust in and noise down? I remember the first thing I got setup before I did any machining work was a full enclosure. I even had a period of downtime because I was still constructing the enclosure as parts arrived while the enclosure was not completed. From the get go I couldn't tolerate swarf and chips flying everywhere. Also, the noise can be kept down when the enclosure is closed so its more tolerable in the room, and it may even help those once in a while tool or part fly-offs from hitting you if it ever happens by accident. Why not build a full enclosure? One can build it out of wood for maybe less than $100 worth of materials. More if you add transparent windows using say acrylic. I would say the main benefit is still keeping dust in, particularly the small particulates that you otherwise breath in. It can't possibly be healthy breathing in too much aluminum, steel, brass or wood dust. For example, I've done some machining on brass with steps involving fly cutting, or sawing, which generates fine dust particles. After a machining operation, I often leave the mill to settle for a while before opening the enclosure to change tools or vacuum the workspace. Sometimes I can find dust particles on top of the spindle assembly where there is no line of sight for dust particles to spray from based on the trajectory of the cutting tool. So it demonstrates that dust particles get suspended in the air and finally settle everywhere. Which means without a full enclosure you're surely to have dust all over the workshop, or if you are near it, you are breathing it in. Fully enclosure is as important as sharp tools and a well trammed mill I think. ------- Re: Why the general lack of full enclosures? Posted by: jferg346x~xxyahoo.com jferg346 Date: Mon Dec 8, 2014 2:29 pm ((PST)) I just got my 2000 cutting metal after a summer of fussing with a lot of other things. I bought it with the steppers and then put the controller together with Probotix electronics, an old pc, and LinuxCNC. Works great but I can see i'm going to need a mister and then some way to confine the mess. I do use the hand-wheels to set up the initial fix, so I'm trying to decide how big to make the enclosure. My thought was that top, back, and sides would be hexcore with some sort of hopefully impervious skins and front polycarbonate, either sliding panels or hinged. It also occurred to me that i could make it with tracks so it could be put together after i had the machine ready to go. Maybe that's nuts. I have limited space and have to move the machine out of the way when I'm doing something else so the enclosure would be taken apart first, then the mill which is mounted on a piece of finish plywood and gets moved to on top of tool cabinet - out of the way. I have plenty of time, so production efficiency isn't an issue. I guess I'm going to end up inventing what I need, probably mocking it up with cardboard, then plywood, then the real stuff. I had thought of leaving hole in the top for the z-axis and in front for the y-axis and then making the box wide enough to enclose the full x-axis travel. I suppose I've got the same question BB-Head is asking, what has everyone else done? John ------- Re: Why the general lack of full enclosures? Posted by: baboonhead11x~xxyahoo.com baboonhead11 Date: Mon Dec 8, 2014 4:05 pm ((PST)) Your 2000 series is larger so you have to account for that based off the dimensions and maximum X (table) and Z travel (spindle motor) accounting for steppers and wheel etc. Anyway my mill enclosure is 31" X 25" X 18.5" and its just perfect for the entire travel with hand wheels and the size of stepper I have and I can still have space to manually crank. Why leave a hole on the top? I think the enclosure should do two main things: (1) keep dust in and (2) keep noise down. If you have any holes, you're not keeping dust in, other than the big chips but sometimes it's the tiny dust particles that is the health hazard. And it certainly won't keep noise level down. I have mine in a wooden frame with high strength thick acrylic pieces on all but the front side. They are permanently fixed to the frame. Then I have a magnetic latching front door that is polycarbonate. So basically I can see in from all directions. If I were to make improvements should I have extra money (I don't) or time (I sometimes do), then I want to put sound insulating material as a secondary enclosure to isolate the machining noise better. I would also like to add an internal HEPA air filter that I can switch on to filter the internal air for a while before I open the enclosure so that suspended dust particles don't escape into the room when I open the doors. Again, I found machining dust is a huge issue. Its obvious when you see machining dust settle on top of the spindle assembly and on the Z axis steppers. Shows how they can really flow around. Wouldn't like that flying around the room or be breathed in. One thing you have to keep in mind also, is the mill enclosure also thermally insulates the mill too. So you will find after machining for a while that the internal temperature is a lot warmer than the outside room temperature. Can be a good thing during the winter and bad for the summer as the head adds on top to make the machine work in a higher temperature environment. ------- Re: Why the general lack of full enclosures? Posted by: jowhowhox~xxyahoo.com jowhowho Date: Mon Dec 8, 2014 6:54 pm ((PST)) I can't speak for everyone, but for me it would be a waste of effort, time, and space. Any other critical observations? ------- Re: Why the general lack of full enclosures? Posted by: "Janet Ferguson" jferg346x~xxyahoo.com jferg346 Date: Mon Dec 8, 2014 8:14 pm ((PST)) BB-Head,You make good points. I doubt if I'm going to do anything with brass, but confining the mess is worth the effort to me. If i can keep the noise down, that would be a help. Shop is in the private garage which came with our apartment and my agreement with the property manager is as long as no-one complains, I can do whatever I want. My approach to this was to visit the people in the adjacent units, tell them what i was doing, that I'd run only during the day, give them my phone number and tell them to call me any time that they were annoyed with it and i'd stop. I've found that when you do this, no-one ever complains. They just want to know that their use of their own homes is being respected. I like the idea of the acrylic panels, although I've been thinking of using 1/4 inch gator board for the back and sides and polycarbonate for top and front. I like the idea of a fan, maybe with some baffles. I think I'll measure this up and see what it will look like. I can get Gatorboard locally, but am likely to have to order the corner channels. thanks for your thoughts. John ------- Re: Why the general lack of full enclosures? Posted by: "Hannu Venermo" gcode.fix~xxgmail.com hvenermo Date: Mon Dec 8, 2014 9:00 pm ((PST)) We have a wide range of needs, jobs, work we do and resources. Full enclosures are very useful if you use coolants, and actually produce stuff, commonly, on your equipment, especially with cnc. CNC use tends to be stuff that takes a long time, because you can run jobs that manually most won't have the hours or will to spend standing at the work. The large majority don't use coolants. From looking at the work done, it also seems obvious the large majority work with models and alu/brass as the materials of choice. These have little airborne contaminants. My stuff is in steel, and industrial, so for me I belong to the very small, maybe under 1%, of minority who: -make stuff commercially -use commercial quality (and cost) CNC kit -need to produce stuff efficiently as otherwise it is not worth it -have to dedicate the space, time, power and resources to be able to do the above. When I made some brackets, for example, I produced about 1 kg of steel swarf. In the dedicated garage, the flying stuff is an irritation, and needs sweeping. Better chip shields will need to be installed. In the list of increasingly desirable order: Coolant, shielding, power, rigidity, accuracy, toolchangers. And they need lots of resources and time if you want to do them so they really work for their intended purpose. In my case: My brackets are in 15 mm or 5/8" inch thick tool steel (F1 calibrado in spain). 150 mm wide. They hold my new servos, for a demonstration industrial lathe retrofit and a demo scratch-built industrial CNC minilathe. The brushless servos are set up with 0.3/0.6 micron step resolution, 10.000 counts per rev brushless, 300.000 kHz, with 30/25 mm thick ballscrews (4/5 mm rise at 1:2 transmission), 220 V, 750 W power. I use an industrial-quality ethernet based CNC controller, at 4 Mhz, and 24 V DC IO with proper limit switches. I will be likely putting in optical home switches, and use an encoder- based spindle index. The spindle servo drive is a 2.5 kW power, AC brushless servo. Just wiring up the controller takes about 3 days, with about 200 connections with DIN rail mounts, ferrules, 24V power supplies, relays, wires, drawing schematics, and about 300€ in bits and pieces. Getting everything done so it works takes about 3 weeks, full time. Issues appear with noise (4 Mhz speeds are noisy), differential signals wiring for servos, MPGs, feed rate overrride, spindle speed override, light towers, hard-wired control panel, cable management. The only benefits on the new lathe(s), 2 of, are more accuracy, more rigidity, more power, and 2 or more toolchangers, and possibility of 2 or more spindles, per lathe. The home switches are more accurate. The spindle index (with an encoder) is more accurate, and the main spindle runs as a full C-axis. The free-running servo spins to 3000 rpm in 0.3 seconds. In use this will be about 0.5 seconds (with a 50 kg carriage). 2.4 Nm continuous, 3x or 7 Nm peak. My stuff is equivalent to the 50.000-100.000 $ commercial turning centers, at 5000 kg mass and 3x2x5 m in size. At 1/10 the mass, 1/10 the power, and 1/3 the cost. They will produce things like very high quality screws, hand tools, and CNC bits. Examples are optronics like optical translation stages, 0.25 mm / rise or 0.5 micron resolution screws, laser equipment mounts. Titanium hand tools, drill bushings, 2 micron gage pins. Accurate, small stuff. Commercial equivalents to stuff I build are HAAS turning centers in bigger and more common stuff, or a Schaublin CNC lathe in the small stuff. hanermo (cnc designs) ------- Re: Why the general lack of full enclosures? Posted by: baboonhead11x~xxyahoo.com baboonhead11 Date: Tue Dec 9, 2014 4:46 am ((PST)) The main advantage of CNC even to the novice or hobbyist not doing commercial work is the ability to get complex shape. There are dimensions and 3D or even 2.5D geometries that you simply can't manually produce and require a CNC to coordinate the axis precisely. Oh so you use your sherline for commercial stuff? I actually don't have coolant system setup either. My enclosure is purely to keep the dust in. ------- Re: Why the general lack of full enclosures? Posted by: "Janet Ferguson" jferg346x~xxyahoo.com jferg346 Date: Tue Dec 9, 2014 5:10 am ((PST)) BB,Complex surfaces were my reason to go to CNC, and also the reduction in the amount of tooling needed to make simpler things. i was getting ready to buy an indexing head, and then realized that i didn't need it for the things I'd had in mind since i can do same thing with different setup with CNC. Did you buy the 10,000 rpm pulley for your Sherline? I didn't and so have to use really slow feeds when I'm cutting with 1/8 end mill. I probably don't understand the thing, but it looks to me like I really need positive way to clear chips and keep cutter lubricated and the runs take a long time, so mister and enclosure seemed way to go. best, John ------- Re: Why the general lack of full enclosures? Posted by: "Elizabeth Greene" elizabeth.a.greenex~xxgmail.com Date: Tue Dec 9, 2014 6:27 am ((PST)) I have a Spectralight Mill that came in an enclosure, and I like it very much. I cut glued-up sheets of insulation foam for lost foam casting and to prove parts before cutting wood or metal. The enclosure traps the foam fuzz and sawdust, keeps the cats away, and catches bits/hex wrenches when I (inevitably) drop them. ------- Re: Why the general lack of full enclosures? Posted by: burkheimerx~xxverizon.net ar1911 Date: Tue Dec 9, 2014 9:03 am ((PST)) I have had two Sherline CNCs. Both were teaching mills from Denford and Lab-Volt. They came with nice steel enclosures and acrylic doors. Lots of those around, usually going for a song. I've even seen the enclosures separately for close to scrap price, but it's been a while. Rex B - DFW ------- Re: Why the general lack of full enclosures? Posted by: baboonhead11x~xxyahoo.com baboonhead11 Date: Tue Dec 9, 2014 7:05 pm ((PST)) The other benefit of the CNC is the press and go. One still needs to hang around just in case something goes wrong to hit the stop switch, but you don't need to physically be there all the time while it is machining. With manual machining your attention is glued to the task at all times. That's another advantage I like about it. I don't have the higher RPM pulley setup. I find I don't need it. Like you said, you can just adjust feeds and speeds. Often that just means slower machining feeds which are probably better for the leadscrews and accuracy anyway as the steppers can't rotate that fast anyway and will lose steps with higher rotational velocities. I don't have a mist system either. On the to do list but time and budget never allowed for it yet. The stuff I machine can be machined dry most of the time. I find a shopvac and some physically applied oil is often sufficient. ------- milling using the Myford Vertical Slide [myfordlathes] Posted by: "Stephen Voller" stephen_vollerx~xxhotmail.com Date: Thu Apr 9, 2015 8:21 am ((PDT)) Hi all, Apologies if I've already asked this in the distant past. I have an ML7, a suitable headstock nose mounted collet holder and the Myford vertical slide with two pivots - one in the vertical and one in the horizontal axis. If you disregard the issue of removing the tool post and topslide each time and then converting back after you've done your milling, how good is using this attachment to do any milling? I am a member of a couple of 16mm scale garden railway groups and have received negative comments ref using the lathe for milling. I do appreciate there is probably no substitute for a dedicated mill but was hoping to use what I've got, so what do other Myford owners think? Regards, Steve V [and in a later message] Sorry folks I just found older messages ref milling in the Myford; am only just getting around to actually doing it! It would seem the answer is to give it ago and take it steady. I would still like to here how others have got on doing it though. Regards Steve V ------- Re: milling using the Myford Vertical Slide Posted by: "David Everett" dernhx~xxyahoo.co.uk deverett2003 Date: Thu Apr 9, 2015 8:43 am ((PDT)) Hi Steve. For what you are contemplating, it will be perfectly adequate to use the vertical slide for milling. Remember, before the days when most model engineers had a milling machine, many fine models were been built using just the setup that you are asking about. It is inconvenient for sure and the vertical slide is nowhere near as rigid as a milling machine, but with light cuts you should be fine with the work anticipated. Dave The Emerald Isle ------- Re: milling using the Myford Vertical Slide Posted by: "Nigel Heasman" nigelx~xxnigelheasman.com Date: Thu Apr 9, 2015 8:51 am ((PDT)) Hi Steve, I have the same set up as you and have done many successful milling jobs with it, but I've also had a few problems! The secret, as you say, is to take it really steady (small cuts) and ensure that your work piece is really well held in the vertical slide (vice or otherwise). Also, always mill "against" the cutter -- don't be tempted to take a cut "with" the cutter -- things will jump about and cause you distress/loss of a carefully prepared work piece or worse! Guess how I know! I would love to have a dedicated mill but they do cost a few ££££'s Good luck Nigel ------- Re: milling using the Myford Vertical Slide Posted by: "Grant Jones Professional Engineer" grantwjonesx~xxshaw.ca Date: Thu Apr 9, 2015 8:54 am ((PDT)) Steve, I am relatively new to model building but not to lathe work. I have milling attachments for my lathes but became very frustrated, as you are so limited as to the setups you can do. You can spend hours trying to create setups, which probably some guys do. The issue that you will keep coming up to is you are too limited to the available height between your lathe centre and the milling table on your lathe. Some guys I note have built an accessory to raise the driving height of their centre to accommodate the work height. To me a lathe and a mill are like and hand and glove, they are a pair. My advice for what it's worth is to put the money that you would spend in milling attachments towards a milling machine and you will be a lot better off. There are a lot of milling machine types out there, and again some guys use some of these very successfully. The knee-type, although more expensive is what I feel gives you the best result. Grant ------- Re: milling using the Myford Vertical Slide Posted by: "Alan Moore" a.j.moorex~xxbtinternet.com Date: Thu Apr 9, 2015 9:24 am ((PDT)) Steve, It is possible to mill using the vertical slide, just as it is possible to cut your lawn with a pair of scissors, but it is all just so much better and easier with a milling machine. Quite apart from the limited size of workpiece you can handle, the biggest problem is the lack of rigidity. In this respect the swivelling vertical slide is worse than the fixed version. It is almost impossible to tighten things up so tight that it cannot move if the tool digs in (I speak from bitter experience here). If it does move it is likely to make the dig in that much worse. Since you can only take very light cuts you are going to wear your milling cutters away faster than if you could take proper cuts. And you are almost inevitably going to get vibration and poor surface finish. Yes, it is possible to mill in the lathe, but in a very limited way. I agree with the previous correspondent -- save up your money towards a proper milling machine, one with dovetail slides, not the inferior mill/drill with a circular column. Look for a good secondhand machine in lathes.co.uk or ebay -- they do come up now and then. Look for one from a model engineer, a school or a college -- it won't have had the heavy use that a machine from a factory will have had. Regards, Alan ------- Re: milling using the Myford Vertical Slide Posted by: red-rosex~xxgreenview.fslife.co.uk jackofalltrades.masterofnone Date: Thu Apr 9, 2015 1:00 pm ((PDT)) Hi Steve, I will repeat what I put on Steam Model Loco. Fly cutting is better than trying to use an end or slot mill. Please don't think people were all being negative about milling in the lathe -- they were pointing to the pitfalls so making sure that your set up was accurate. I also have a two-axis vertical slide. I have tried milling in the lathe and the trick is to go slowly! Keep the speed down as a dig-in can push the slide round if it is not securely clamped in the vertical axis. I used a 1/2" slot mill and probably went too fast and got a horrible dig-in that broke a tooth on the mill. A flycutter will sweep more gently. I set the vertical slide against a chuck face (with the jaws out) to get it square to the spindle but have seen recommendations since to place a piece of paper between the mating surfaces to increase friction which will make clamping more secure. Be sure to lock all slides that you are not using to get maximum rigidity, and practice first. Flycutters are easy to make -- you just need a blob on a stick that is concentric, and a hole for a piece of HSS ground like a right hand knife tool with a round face to give a good finish. OK, that is a bit simplified but you can find proper descriptions anywhere. I will take one for you to see if you are going to Peterborough on Saturday. Andy ------- Re: milling using the Myford Vertical Slide Posted by: stephen_vollerx~xxhotmail.com stephen_volleruk Date: Thu Apr 9, 2015 1:17 pm ((PDT)) Thanks to all who replied and especially to Andy for your patience -- sadly I won't be able to meet you as am unable to get to Peterborough. I will certainly give it a go to see what can be achieved but do appreciate that a dedicated mill is the way to go -- better start saving I think. :O) PS - Andy - thanks for taking the trouble in describing the setup. I will give the fly cutter a go -- if I don't try I'll never know Steve V ------- Re: milling using the Myford Vertical Slide Posted by: "Kevin" tadpolex~xxbtinternet.com klokenz Date: Thu Apr 9, 2015 1:21 pm ((PDT)) I'd say just get yourself a few brand new milling cutters and have at it! Just take it easy and you'll be delighted with what you can do, big smirky grin time! Once model engineers in home workshops did all their milling in the lathe. Number 5 in the Workshop Practice series of books is "Milling Operations in the Lathe", by "Tubal Cain", highly recommended. Kevin, England ------- My new lead screw has arrived. [atlas_craftsman] Posted by: abigalesdadx~xxcomcast.net abigalesdad Date: Fri Apr 17, 2015 9:06 pm ((PDT)) My 5' piece of precision acme lead screw from Roton has arrived. It came in a spiffy spiral cardboard tube sealed with wooden plugs. Cost including shipping was about $80. I plan to machine it into a replacement for the badly worn screw on my Craftsman 12" and do the work on my Wards Logan 200 and my Sharp SM mill. The lathe work will be straightforward, but machining that nearly full- length slot will be a little tricky. The effective bed length on the mill is only about 20" so my plan is to fasten two co-planar parallels to the table and, using two 5C collet blocks to hold the screw against the parallels and centered under the end mill, machine the slot in segments. Once I get the end mill on center and cut the first segment, I can loosen and reposition one collet block, and then loosen and reposition the other one. With the collet block repositioned, I can fasten each block to the table up against the parallels and machine another segment of the slot. This technique will keep the slot precisely on top of the screw and the screw represented to the end mill in a manner that will keep the centerline of the slot directly above the axial centerline of the screw. I'll reposition and cut until I complete the entire slot. It's making sense in my head. We will see how it works out in reality. I'll keep you posted. I attached several photos. One shows the cardboard tube and the other shows the new screw beside a heavily worn section of the old screw. Dave ------- Re: My new lead screw has arrived. [2 Attachments] Posted by: wa5cabx~xxcs.com wa5cab Date: Fri Apr 17, 2015 9:48 pm ((PDT)) Dave, I would suggest that you broach a keyway into one of the two collets. Do the mill work before the lathe work as that gives you around 3" at the tail stock end that doesn't need to be slotted that you can hold onto for the first slotting pass. Plus I would imagine that the screw that you received is longer than the lead screw needs to be, which gives you some more to hang onto, and the keyway does not need to run all the way to the headstock end. Make the first cutting pass without a key in the collet (there being in any case no keyway in the screw for it). After the first pass, release both collets, slide the screw a little way, and insert the key. Obviously, the orientation of the keyway in the collet is critical and must align with the cutter. I would also suggest that a horizontal mill will do a much better looking job than a vertical mill. And position a roller stand at each end of the table to support the weight of the part of the screw hanging off of the table. Else the weight of the end of the screw hanging well off the end of the table will arch the screw up a few thou in the middle Robert Downs - Houston wa5cab dot com (Web Store) MVPA 9480 ------- [SherlineCNC] miniature end mills (I mean really miniature) and engraving head Posted by: gp_illustratorx~xxyahoo.com gp_illustrator Date: Wed Dec 30, 2015 11:08 am ((PST)) Anyone have any luck cutting Al 6061 with small endmills? I've been able to get decent cuts with a .2mm ball endmill with a .6mm flute length using both the stock pulley and the 10K pulley, but I need to cut deeper than that. So when trying a .2mm flat with a (IIRC) 4mm length, nothing but snapping using the 10K. No matter how much I slowed it down. I was using a DOC of .25mm and a feed rate of anywhere from .3 IPM down to .07 IPM, but I'm thinking my mistake is my DOC. So, is the DOC the problem or should I move up to buying the high speed engraving spindle? WD40 was used BTW in all attempts. As always, thanks in advance. G. ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Jeffrey Birt" birt_jx~xxsoigeneris.com jeff.birt Date: Wed Dec 30, 2015 11:40 am ((PST)) You are not going to be able to cut at 1.x times the bit diameter with such a small bit. Your DOC cut needs to be about ¼ of the bit diameter, then do multiple passes until your desired cut depth is achieved. Jeff Birt Soigeneris.com ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Tom Wade" tomx~xxwade.name arcmaster3 Date: Wed Dec 30, 2015 11:58 am ((PST)) Not tried them on my Sherline, but on my Bridgeport, doing heavy similar cutting in Al bar stock (don't know the alloy) I use 60 degree conical V-bits from 2 L inc, at http://www.2linc.com/ I run these at about 6 ipm on the Bridgeport, and have broken one so far. But that was a full rapid travel into the back of the vise. Another advantage is that you can cut with these in either direction of rotation. They don't care. I'm taking fairly deep cuts, perhaps 1/16 at a time. They are available with a variety of end diameters. These are also really easy to sharpen. Here's a complete video. It's way too long, so just jump through it. https://www.youtube.com/watch?v=L6QGcJht9_I Tom Wade Hope, Indiana ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Gabe Pena" gp_illustratorx~xxyahoo.com gp_illustrator Date: Wed Dec 30, 2015 1:31 pm ((PST)) Thanks Tom, I'll check out the video. G. ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Stan Stocker" skstockerx~xxcomcast.net stanstocker Date: Wed Dec 30, 2015 12:28 pm ((PST)) Greetings, Do your math for chip load. People run small bits far too slowly quite often. If you aren't cutting chips, you're rubbing, and that kills bits in a hurry. Chips also carry heat away from the cutting surface. If you make dust, the cutter overheats. With that small a bit I'd still chase half a thou to a full thou chip thickness. Just for shiggles, try around 5 IPM and inspect your chips to see how well things are going, adjust from there. Chip evacuation is critical with small bits, if the chips are getting recut you're going to get poor results. Good luck, Stan ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Gabe Pena" gp_illustratorx~xxyahoo.com gp_illustrator Date: Wed Dec 30, 2015 1:29 pm ((PST)) So, are you saying slow as in rpm or movement (ipm)? G. ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Stan Stocker" skstockerx~xxcomcast.net stanstocker Date: Wed Dec 30, 2015 2:05 pm ((PST)) Either way. What matters most is the thickness of the chip. Push too hard and you get snapped bits or poor cutting due to cutter deflection. Run too slow and you get recutting of chips, insufficient chip thickness, and overheated and dulled cutting edges. If you're running 10000 rpm with a 2 flute cutter, you're taking 20,000 cuts per minute. If each cut is one thou thick, you're removing 20 inches of chip thickness per minute. It's a swag sort of a ballpark way to estimate stuff, but that says 20 IPM if your cutter can handle it. With a small cutter and good chip evacuation you can probably drop to 10 IPM, and take half a thou chips. If you want to go slower, drop the rpm too. The goal is to cut chips and get the chips with their heat away from the cutter. Once your chip thickness is dialed in, then the DOC comes to the party to remove as much as possible within allowable cutter deflection or machine capabilities. With a small cutter, the cutter rigidity is usually the limiting factor, with a big end mill the machine may not be able to push the cutter beyond some DOC even if the cutter is not deflecting. Many cutter manufacturers have cutting speed calculators online, such as the one Lake Shore Carbide has. They only have their cutters in the tool tables of course, but odds are you can find something really close to what you are running. Take care, Stan ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Gabe Pena" gp_illustratorx~xxyahoo.com gp_illustrator Date: Wed Dec 30, 2015 2:23 pm ((PST)) Thanks Stan. This all makes sense. BUT (and I'm way way waaaaay a novice here, so excuse my questions or assumptions if they seem stupid) when I tried cutting at .3 IPM x~xx 10K the .2mm end mill snapped about 4-5 seconds into the cut after bowing/flexing, so although you're advise seems logical, my experience led me to figure I was going too fast. Again, I'm thinking it was the DOC that was my major problem. As soon as I get a chance after the holidays, I'm going to try your advice, but in the meantime, I am learning quite a bit just reading the thought process, so any more thoughts on this are greatly appreciated. G. ------- Re: miniature end mills (I mean really miniature) and engraving head Posted by: "Graham Hollis" ghollisx~xx517704.com gahollis Date: Thu Dec 31, 2015 1:24 am ((PST)) Gabe, the length the tool protrudes from the holder makes a huge difference with small cutters. It's also very important to have almost no run out on the spindle for this size cutter as this will overload one tooth vs the other. A high precision collet or a custom holder bored in place would be best. The tram of the mill, how perpendicular the head is to table, needs to be perfectly dialed in or else the tool is leaning over. The stickout or unsupported length of the cutter should be a small as possible, 10mm or less, 5mm would be better. This is not only to minimize deflection but also to reduce the effects of any 'out of tram' condition. On a max 10K spindle, a feed of .59 in/min will give a cut per tooth of 0.00003in which is correct for 6061 with a carbide cutter of 0.2mm and a flute length of 4mm. I'm guessing the shank is 1mm above the flutes. The depth of cut should be no more than 0.2mm per pass which should keep the tool deflection within limits given the run out and stickout are not an issue but I would start with less 0.1 or even 0.05 (1/4 dia) and work up to that depth. Graham www.d2nc.com ------- Holding straight shank end mills in collets [atlas_craftsman] Posted by: "Bill Williams" BWMSBLDR1x~xxGmail.com bwmsbldr Date: Sun Jan 24, 2016 10:18 am ((PST)) I have had the experience (on rare occasion) of a mill shank drifting out of a collet and ruining work. To help avoid that I have colored the mill shank up to the collet with a marker. Any movement results in a bright line where the shank is exposed serving as a warning. Bill in Boulder ------- Re: Holding straight shank end mills in collets Posted by: "ogberi" ogberix~xxgmail.com ogberi768 Date: Mon Jan 25, 2016 6:34 pm ((PST)) Same thing I do. Get everything set up, then spin up the mill and use a Sharpie to black the endmill/collet face where they meet. If you do it good, you can spot any deviation pretty quick. ------- ------------------------------------------------------------------ This is just one of some 80 files about machining and metalworking and useful workshop subjects that can be read at: http://www.janellestudio.com/metal/index.html ------------------------------------------------------------------