[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.

[sinha_nsit]

...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.

The best way, I believe.
If the profile consists of both convex and concave corners, and tool radius is too large compared to the individual path segments, interference in radius compensation may result. Since you are using a CAM software, offset the profile by a distance equal to the tool radius, and do not use radius compensation at all.

[gotyernumber]

The part is all convex arcs except for the entry and exit moves. I really need the compensation, we have 9 different sizes with variations of approx .0025-.005" between each size. Then we have 17 different "items" so I would prefer to have 17 programs with cutter/comp than 153 programs without c/c and the chance of someone not choosing the correct program...... cuz you KNOW that will happen. I have been looking at the parameters and #5010 (vec neg limit) is set to .0019. This is an Oi control, still researching whether I can just change that one parameter or if there are some sister parameters that need to be looked at also. Thanks everyone for all your input!

[txcncman]

You would still have 17 programs for your different sizes. For each the cutter comp entered into tool data would be zero instead of actual tool diameter. The problem would come when someone puts in wrong tool size or reground tool.

I still suggest your try to get rid of the line segments and output your G-code with arcs if at all possible. Would make for a smoother looking part.

[sinha_nsit]

Increasing the size of the line segments may help. Try this if it gives you acceptable smoothness.

The other way would be to offset the smallest size by tool radius in your CAM software. Now machine with radius compensation specifying the difference in size as tool radius. The might solve the problem because "tool radius" would be pretty small. I am not very sure, but this method should work. Do try and let us know.

[angelw]

gotyernumber,

Plotting both your DXF and NC file resulted in two entirely different shapes, see the attached pictures. The DXF plot is on the left.




Apart from the cutter rad comp issue you're experiencing, with small moves such as those in your NC program, you may have trouble actually obtaining the programmed feed rate due to acceleration/deceleration at the start and end of each block. There simply may not be enough distance for the slides to obtain the programmed velocity before having to decelerate.

You could construct your shapes using circular moves by drawing arcs using the 3 point method, or if that is not accurate enough for the application, the biarc spline method can be used.

Rrgards,

Bill

[gotyernumber]

I won't be able to try anything for a couple days due to production, however i am working on a new program using arcs. I'll let everyone know how it goes.
Yes, the shapes are different, I just grabbed a dxf file that was handy trying to show that it was all convex curves on an OD. The second plot is of the actual part.
I'm fairly new to the programming side of things and when I first started I was getting more c/c alarms using arcs than with lines so I stayed with that and all was good until this part came along. I did try lengthening the lines but still couldn't get around it and the faceting was unacceptable. Thanks everyone!