Odd behavior threading with G32

[simmonds]

I am getting a strange behavior when trying to thread with a G32 cycle on my new Hardinge/Centroid conversion. To illustrate this, I took a single pass with a very light cut using that cycle. Here is the relevant section of code:

N14 T0202
N15 G54
N16 M8
N17 G98
N18 G97 S100 M3
N19 G0 X0.6 Z0.5
N20 G0 Z0.015
N21 G1 X0.494 F5.
N22 G32 Z-0.235 F0.03125
N23 X0.56 F0.03125
N24 G0 X0.6
N25 Z0.0133
N26 G0 X0.6
N27 Z0.5

This is the spiral path the tool tip made on a 0.5" brass rod:

The pitch is correct (0.0312") for about half of the thread length, but the pitch tapers down to nothing by the end of the cut. The total length of the thread is also correct (0.235"). I could not find any discussion of this specific problem on the forum, but from reading about other threading issues, I am anticipating some questions:
1. The spindle encoder (on input #6) is putting out an index pulse (asterisk appears) every full revolution, with 4096 counts between these pulses.
2. According to the Encoder window, the spindle encoder is performing perfectly: no errors.
3. If I run the program a second time or add a second pass, all subsequent cuts line up perfectly.
4. If I change the spindle speed between 100 and 500 rpm, the pattern is exactly the same. Not speed dependent.
5. The depth of the cut has no effect. It does not appear to be caused by loading on the Z axis since cut is only ~ .005" deep.
6. The behavior is not affected by the position of the Feed Override knob, as one would hope for a threading operation.

I suspect there may be an incorrectly set parameter causing this since I have carefully ruled out many other possibilities.

See the attached report file and complete G-code program.

Other than this, the Centroid control appears to work correctly on my lathe. Using a modified FANUC post (I described and uploaded in another thread on this forum) I can run NC files generated by HSMWorks with no problem. It handles both front and rear mounted tools and should also work for files generated by Fusion 360.

[tblough]

Try setting parameter 240 to -1 to disable deceleration on threading cycles.

[simmonds]

Thanks Tom, that was it. Now, after two passes it looks like this:

Not sure why my control had a value of 0.1 loaded instead of the default of 0.

Since I have servo motors and am cutting slowly the -1 value is the right choice. I had scanned through all the parameters looking for likely suspects, but since it was labeled "Ridged Tapping Decel and Stepsize" I missed it.

So many parameters, so little time!