Results 1 to 11 of 11
06-15-2007, 11:11 AM #1
I'm turning (trying to at least) a 3" .5" Pitch 1.0" lead (double start) Left hand ACME thread. At least it's a 2G. I'm making a test piece of aluminum before starting on the actual job [img]smile.gif[/img] I'm having trouble measuring the pitch diameter with the 3 wires method. I've got the correct wires .25823" but can't figure out the constant? Any help would be appreciated.
06-15-2007, 11:30 AM #2
I've never heard of that method of checking an ACME thread. Usually folks use the one-wire method.......at least that's the only method I've ever used, and the only method I have any info on.
06-15-2007, 12:16 PM #3
Looking at my _Guide to World Screw Threads_ there's a section on 3-wire gauging of threads, including an ACME section. The row with your wire (best for the pitch) has the entries:
Wb = 0.25822
Wmax = 0.32501
Wmin = 0.24363
WbY = 1.28953
WbZ = 0.77311
pX = 0.96668
I *think* the formula using these is
measure = pitch_dia - pX + WbY
If I were doing this I'd run through the numbers completely, I think the helix angle of the 2 start will really mess this up, particularly with an ACME thread. But this might give you a quick check.
06-15-2007, 12:23 PM #4
Machinery's Handbook, 25th edition, page 1796, "Three Wire Measurement of Acme and Stub Acme Thread Pitch Diameter". I hope that you and your calculator get along well if you are going to use this method. I have done it several times and it heats up your brain cells by the time you get it done. You have to take the helix effect from the two start into account as rke[pler stated.
Glenn @ Metro North.
06-15-2007, 01:53 PM #5
Another point: That's a 1" lead. You'll need to span two of the wires with a little parallel to catch the tangency plane of the two wires with the mike anvil. Make a simple jig from Starrett stock to hold the wire pair at about the correct distance. Check the height so you can include the correct offset for the thickness of the jig.
Work up complete manufacturing data before you start - that includes the class of fit and how it affects the other data. Use the one wire method or a gear tooth vernier to track progress.
How long is that screw? If over a two feet long you're getting into follow rest terrirory.
I suggest cutting it to depth with a narrow tool then side shifting to get pitch diameter.
If your lathe has a 6 pitch lead screw be careful of when you close the half nuts.
06-15-2007, 03:53 PM #6
I found all the stuff in the machinery's handbook and the formula was heating the brain cells, but not enough. I was having a hard time with the formula and remembering which step to do first.
The helix angle is steep. We had rubbing issues on the leading side of the tool. This resulted in the tool slipping and making a weird shaped thread. We fixed that and I tried side shifting but the tool didn't cut it rubbed, then I went over another thou, then it rubbed for a while, then grabbed and the tool slipped again.
The Length of the part is about 20" with 12" of thread.
I'm "trying" to turn this on a TL-1, so no worries about the 6 pitch lead screw. I'm a little worried about the speed. I have no gearbox and I'm feeding straight in .005 per pass. This makes a lot of passes for a double start thread. [img]smile.gif[/img] I'm at 75 rpm now and that works out to 75 ipm. The spindle load is about 60% and this is an aluminum test piece. The max I can run is 150 rpm and 150 ipm (max feedrate of z axis). I'm wondering if I should bump up the rpm to try to get a little more torque from the machine.
Another question. Should I be cutting the thread with a 14 deg infeed angle then straight in for the last few passes, or just feeding straight in?
06-15-2007, 03:55 PM #7
Oh, and what is the one wire method? I've never heard of that before.
06-15-2007, 04:20 PM #8
A variation in 'straight in feed' is what I would recommend if you must do this with only one tool. This would involve programming in single pass moves, not an automatic routine such as might be used for V threads.
You can pick a Z start point of whatever, say .500" in front of the part. Now create a series of start points that stagger ahead and back of this Z.500 start position. Obviously, at the outermost passes, the tool can be staggered the most, and this amount will have to steadily decrease as the depth of cut increases, until theoretically, the stagger amount is zero with the tool at full depth.
So you can take a cut starting right on Z.5, then the next cut ahead of Z.5, the next cut back of Z.5 and all done at the same X value. Then take the 4th pass starting at Z.5 again, but at increased X depth. And so forth. Keep the chip forming on basically one side of the tool at a time. Keep the rpm up to try to get the best smoothness. Using this method should not get you into overload on your spindle.
06-15-2007, 09:20 PM #9
Why do you want to feed straight in???
Set the compound at the correct half angle of the thread which is 14.5 deg. and use the compound to feed in. That way you are only cutting on the leading edge and the tip. I have never had any luck plunge cutting an acme thread. Cutting an acme thread puts a heavy load on the threading tool and if all clearances are not good it will hog in and tear up the work and the tool as you have already found out. Take small cuts and don't get in a hurry.
06-18-2007, 01:00 PM #10
I did get the test piece cut sucessfully! Looks cool in 6061 too. I showed it to the customer and he wouldn't give it back [img]smile.gif[/img]
I ended up having the most trouble with the tool rubbing on the high helix angle. It screwed up the thread the first time around. I couldn't cut it after that without the tool digging in. I ended up using Forrest's advice on the narrow tool. I ground one for a 4 thread per inch acme, and cleaned up the boogered up side with .0005 passes. The other side cleaned up perfectly with .001 passes.
Hu, your method looks like it's a winner for cutting the real pieces. Haas has a G76 Canned cycle with an option for Double edge cutting, which I think is similar to what your talking about. I haven't done much in the way of hand programming threading cycles, but I think it feeds in at the infeed angle specified and alternates which side of the tool it cuts with. I hope so at least, because the last prog I wrote was with G32 and it was a long program.
Thanks for all the help.
06-24-2007, 02:25 PM #11