CNC thread cutting issue

[rambozhou]

When i cut the ACME thread on CNC Lathe,i face a problem:
the first tooth is a little wider than the others (about 7 teeth totally), as i know that when we use the CNC lathe to cut the thread, there will be a short incorrect threaded length at the beginning and the end,the lengh is depends on machine time constant T,but after i have set the constant to 0.033s, the error still exists,are there any tips for this issue?

Thanks

 

[mrainey]

I'm not sure what the machine time constant refers to. If the part geometry and setup allow, increase the length of air cutting before the threading tool contacts the workpiece. The distance required increases with higher RPM and/or coarser thread pitch. So if all else fails, you might try slowing the RPM.

 

[twinny]

I'm with mrainey on this one it sounds like you have not allowed enough distance before cutting the thread to allow the spindle to syncronise with the cross-slide.
Slow the spindle down if you cannot increase the air cutting.
Most cnc lathes have a constant they are constrained by in thread cutting i.e. the speed at which they 'sinc' on newer lathes it is 6000 i.e. at 2000 revs you can pitch 3mm max and at 4000 revs 1.5mm max pitch.
With acme style long pitches you will come across the problem of correspondingly low spindle speeds and therfore not much torque.
The min distance of air cutting can be as much as 2 x pitch.

 

[rambozhou]

The spec is ACME 1/4-16-2G (Lead=0.0625"=1.5875mm),machine time constant 30ms,i have tried from 4 to 10mm air cutting space,200-800RPM spindle speed,still first tooth is a little wider,totally 7 teeth,i have tried only machine 3 teeth or 4,5 teeth (so i can get more air cutting space),things is same as before.

 

[mrainey]

I'd have to see your workpiece, setup, and tools before I suggested anything else.

 

[EdDanzer]

I think your work piece is deflecting. If the part is 1/4” diameter, the minor diameter should be used to determine the length to diameter ratio. Machinery’s Handbook gives 0.161” as the minimum minor diameter. Acme threading will work best with a 2:1 length to diameter ratio. This means the most unsupported stick out you should have is 0.322”.
You may have to center drill the part and use a live center, or chuck closer to the threading area to reduce part deflection.

 

[airuno]

Try to chamfer the part again after you cut the thread.

 

[rambozhou]

By changing the G command from G92 to G76 and adding a 3 degrees shim under the insert, i have got perfect result.
The thread can be overlayed perfectly with the 50 times template under the optical comparator.

The system we are using is FANUC-0T series
G92 thread cutting cycle means the cutter infeed direction is perpendicular to the spindle axis--the cutter three edges machine the shaft at the same time.

G76 mutiple thread cutting cycle means the cutter infeed along one side of the tooth, then only two edges machine at the same time--maybe the machining force is less than G92.

The spindle speed is 200RPM now.

Thanks for all your help!