Results 1 to 19 of 19
Thread: Thread milling acme threads
09-16-2009, 02:59 PM #1
Thread milling acme threads
I have looked for Acme thread mills and cannot find one. So I assume this is not normally done. Is there a clearance problem, some other problem or is there just no call for it?
09-16-2009, 04:20 PM #2
I have seen some tools in the kennametal book that are for making groves in the side of a part on a mill. the tool holds 3 or so top notch inserts that you would see in a lathe. im sure others will chime in but i would think that this same tool could hold a top notch acme insert and do the job that your after. it would only do one thread at a time but it could be done. it might just depend on how the inserts hold up on all of the interupted cutting.
09-16-2009, 04:41 PM #3
09-16-2009, 05:26 PM #4
That tool is primarily for lathe work. The back side of the tool would interfere with the cut for thread milling if you chucked up the shank. I suppose you could cut off the end and chuck up what remained, but it would not have very much cutting depth.
09-16-2009, 05:51 PM #5
I'm thinking you can't, for the same reason that you can't threadmill a square thread. No matter what your relief angles are on your tool, you're still swinging a revolved solid(that may or may not make sense). Combine the 29 degree included angle(getting close to square) with the helix/pitch of most Acmes (Steep) and I don't think its going to work.
Add in how tiny the shank would have to be vs. the cutting diameter and the amount of material that needs to be removed, it would be ugly.
Somebody with solidworks could probably draw it up in no time. I'm thinking it may be possible to do an external thread though, maybe.
09-16-2009, 06:21 PM #6
You might have to use a tool that has a thinner profile than the gauge width, and perhaps even modify the angle from 14.5° because the top angled edge of the tool enters the work first, and the bottom edge leaves last.
I'm reminded of the way that an involute gear cutter plows a wider tooth space than itself when it cuts a helical gear tooth. There is even a formula that calculates what number of cutter is to be used for a given tooth number, that takes into account this widening effect.
As for modelling the shape of tapered wheel that would fit in an Acme internal thread, wow, I can't imagine how one would do that with technical perfection. It would be great if somebody could show us the trick
09-16-2009, 06:24 PM #7
09-16-2009, 07:17 PM #8
I was in a gear shop in town a few years ago and saw a lathe lead screw being milled. The screw was 12 ft long and the machine could handle only a 6 ft length. The work had to be reset after the first half was cut. I asked the owner about the change over point and he said the customer would not be able to find the location.
09-17-2009, 03:10 AM #9
09-17-2009, 04:48 AM #10
09-17-2009, 07:38 AM #11
Well now at least I know it is possible. What I am looking for is a single point tool capable of doing inside diameters in the 0.5" - 1.0" range.
09-17-2009, 10:34 AM #12
09-17-2009, 12:20 PM #13
I called Vargus, the tools you see are for the lathe. They don't have anything for thread milling in the range I seek.
09-17-2009, 01:07 PM #14
Bridgeport leadscrews are thread milled. Saw it being done at the factory. Don't know what Hardinge is doing now.
09-18-2009, 12:56 PM #15
I'm sure Bruce is trying to thread mill INTERNAL threads, not a leadscrew. Internal acmes and external acmes are not the same. It's EASY to do external acmes by thread milling or grinding, it's another matter to do the mating nuts.
I have a hard time seeing how a acme thread mill would work other than it has to be narrower than the machined thread. I would think it would wipe out part of the thread as it's revovling. Trying to thread mill in the 1/2 to 1 inch range for very deep, may be interesting. what's wrong with single pointing the thread and then tapping for size.?
09-18-2009, 06:23 PM #16
Brian - your point about threadform is a good one. I assumed that if threadmilling Acme was possible, the mill profile would not reflect the threadform exactly. As cncprogman points out - Vardex does supply insert based thread mills for larger threads. So I now believe that it is possible. I can of course do the threads another way, but I just wanted to find out what was possible. If it can be done for larger internal threads, it can be done for smaller as well (depth might be a problem). My guess is that there is not enough call for small threads to make it worthwhile for a toolmaker. But maybe someone will prove me wrong.
09-18-2009, 10:10 PM #17
Considering hardly anyone uses acme machine threads in production machines, what's the point in a tool and cutter shop making them. Most people would probably cut their acme threads in a lathe rather than try and thread mill them.
You want a possibility to accurately thread mill small acme threads? The trick is to get the cutter angled at the helix angle of the thread, which is different for every diameter of every acme thread. Your NUT would have to rotate and move at the right pitch. Frankly you CAN do this with a VersaMil with a Universal head, mounted on a manual lathe. So there is one example of thread milling small threads. And you could use a thread mill that DOESN'T have to compensate for rubbing on the threads. IT does have to be a relatively small diameter mill though.
I find it interesting that the new CNC cylindrical grinders made by Studer claim to be able to THREAD GRIND. Now they do this unlike thread grinders, that the wheel is angled to match the thread, but by dressing the wheel unequally on both sides to give the right profile. This same theory could certainly be applied to a thread mill. Your question is a pretty interesting one, as I thread grind threads, and threadmill them on a Pratt and Whitney threadmill. I also have a Vetcoa thread milling table that enables me to threadmill even on a manual Jig Bore. So I have lots of options for cutting threads, beside the obvious, single point them in a CNC lathe. The Pratt and Whitney threadmilling machine EASILY can do acme threads even in small sizes, because it's able to rotate the cutting head to the correct helix angle, and revolve the part being milled at the same time as feeding the part into the thread mill at the correct pitch. I have to assume you're trying to accomplish this on a CNC mill, which unfortunately doesn't have the ability to match the helix angle of a thread.
05-09-2012, 08:03 PM #18
Recognizing this is a 3 year old thread ... it happened to be a top google search result for internal milling acme threads. Emphasis on internal.
So I spoke with these folks mentioned above:
Single & Multi Flute Replaceable Insert Thread Mills, Thread Mill Inserts, Solid Carbide Thread Mills: Advent Tool & Manufacturing: Lake Bluff, IL
They have an off-the-shelf product to thread mill internal acme in general so long as the thread major diameter is around twice the diameter of the tool. In other words 3/4" shank tool for 1-1/2" threads.
At extra charge, they can relieve the shank, obviously weaking the tool and reducing the depth of cut per rev, to thread extra deep holes.
At extra charge, they can custom-grind the cutter form so that for small diameter threads, where it's impractical to keep the cutter body dia < 1/2" the thread diameter, custom grind so that the ... cutter is shaped so that its interference on the "exit" leaves the correct thread form. Sounds complicated.
Might use it later, but will stick with boring in the lathe for now.
05-09-2012, 11:15 PM #19
I had the need for a acme thread mill on a job I did last week, specificly 3/8-12. I found one from Scientific Cutting Tools, http://www.sct-usa.com. I special ordered it through MSC and it came a couple days later, I think it was $96. This was a cheaper alternative to a tap at $150. The tap is extremely long and makes the thread in two passes. The material was aluminum and I had 120 holes to thread. Programmed the part in SolidCAM like a regular thread mill with the data that I measured off the actual threadmill. Ran the 1st part and it came out perfect the first time I ran the rest of the parts checking the thread every 10 or so. I was checking the parts with a short piece of acme threaded rod. Parts came out great. Didn't have any data on speeds but I ran the cutter at 8000 rpm and 10"/min to make sure I did not brake the fragile cutter.