[Captdave]

I was having trouble parting off some parts the other day that were .393” dia with a .075” chamfer. The problem was that the parting tool was cutting the part off before it had a chance to add the chamfer. After looking thru the parameter manual and the TPC data section of the programming manual for grooving process, the only possible parameters that I could find that may control the amount of over shoot was “Groove start clearance (diametral value) in X-axis” U8. Noted the original setting of .2”, and did some test cuts which worked fine and settled on a value of .05”.

My question is this: Is this the correct parameter to use in this case and what is the typical amount (value) that should be used to allow for proper clearance?

Also, when a value is changed on the TPC date page, does that change just the associated value for that program or does it effect any program the same as changing the U8 value in the normal parameter section?

T32-B QT-8 Mazatrol program.

[extanker59]

I've checked before. The TPC changes effect only that tool in that program. I've meant to change all the calls for that tool in a program, forgot, and rubbed a boring bar.
BTW, have you noticed that the TPC changes in turning a relief ($1 in Bar Out, K33-K34) have no effect? I have to change the parameters in the parameter page to change the motion. Am I way off base?

[Captdave]

I found that too. Try $4 K35 K36, not sure what the difference is but it worked for me. Remember to set the minor ID in the common process to just under the bore size to keep the boring bar from going to X0 during rapid movement at retract.

[extanker59]

Got it. Thanks. I'll try the $4

[Mikiemo]

I don't remember the exact parameter from t32, and matrix is completely different, but I think the parameter has a description of x-axis groove clearence (diameter). I would typically set this to .005 so in a type #4 cutoff cycle the tool tip will only clear the bottom of the chamfer diameter by .005Ø.

Mikiemo