Need Help!- cutter compensation

[gotyernumber]

We have 2 mills with fanuc controls, one horizontal, one vertical. I have a program that runs fine on one machine but I can't make one pass on the other without getting a "PS0041- interference in G41/G42" alarm. This is on an all OD cut (it is almost circular)! I have never had cutcomp alarms on an OD milling move like this before, this is just a different size than many other parts we make and they run fine on both machines. So I'm thinking the issue is some setting on the control?? At first I thought it was an issue with the model (and it still could be) then I tried it on the other machine and it ran fine. The entrance and exit moves are arcs and are double the tool diameter. I have tried point to point and arcs with no success. Any ideas?? I have attached a sample but this is my first post here so it is a coin toss on whether it makes the trip. Thanks!

[txcncman]

You DXF file came through ok. I would, in this case, rather see the code, especially the 3-4 lines just preceding and 3-4 lines following the error.

[gotyernumber]

It alarmed out @ X-3.2177 Y-2.054. I put the entire pass in the attachment. Thanks!

[MIYANO vs FANUC]

#41 = interferrence in CRC.

overcutting will occur in cutter comp C.

Two or more blocks are consecutively specified in which functions such as an auxillary function and dwell functions are preformed without movement in the cutter comp. Whatever that means...

[txcncman]

Looking at it now. Normally this occurs on radius moves. I can see from your code you are cutting arcs with line segments. There is no "X-3.2177 Y-2.054" line in your code. Was this the machine position where it stopped? I really need to know what line of code it stopped on, not the machine position.

[gotyernumber]

OOPS! It should read X-3.2477 Y-2.054. and yes that is the machine position, I will try to get get the line it stopped on when they are between parts, maybe 45 min. before I can do that. Thanks!

[txcncman]

I have identified two Y moves that potentially were causing your problems and commented them out of your G-code with parentheses. I suggest you run this G-code in your machine with the tool length offset set to run above your part and see if the problem was corrected.

[gotyernumber]

Thanks, I will try that !

[gotyernumber]

OK, it ran past your edit, and stopped at Y1.9758, I blocked that and it ran past that...

[txcncman]

Well, I hope you see what is happening here. With cutter comp on, the CNC thinks it can't get from one point to the next and maintain the line. Since the way you programmed this output small line segments of only a few thousandths step at a time, it might be possible to eliminate a few and still make a good part. I would suggest for future programs you either use arcs or increase the size of your line segments.

Another way to work around this problem is to offset your tool path the radius of the cutter and put 0.000 in for the radius offset of the tool.

[gotyernumber]

Thanks txcncman, we used to program using "0" in the tool radius offset but these new machines have laser measuring capability for length and diameter. Everyone started using them which led us to where we are today. This is the first part that has really given us fits so I'm thinking we will have to go back to that. However I also got a cut/comp alarm using arcs, can't remember if it was the same alarm, just know it was a no go. Thanks for your help and I'm still wondering why it ran on one fanuc and not the other, that is why I thought there might be a parameter/setting that might fix things. Thanks again!

[txcncman]

On all Fanucs I have worked with, there is a parameter setting that controls how much error is allowed on either arcs, cutter comp moves, or both. You will have to check the book to find out which. Normally I would think this would be set to 0.0001.