Fanuc Radius Compensation

[Moray]

From what you've just posted, it sounds like you're combining both...

What Tom maybe wasn't quite clear enough about, is with option 1, the g-code produced should essentially trace the corresponding line on your drawing. It is then up to the machine (aka g-code interpreter) to offset the spindle from that line depending on the tool diameter set in the machine.

With option 2, the g-code produced already allows for the tool diameter, so the produced g-code path is already offset by half the tool diameter set in the CAM tool table, and the machine simply follows that line with no compensation.


Generally option 2 is the easiest, however it does mean if you have to change tool/allow for tool wear, you need to adjust the tool diameter in CAM, and re-generate the g-code, rather than simply changing the tool diameter in the machine.

[TomKerekes]

hi a_j_p,

I was planning (at least in my head it seemed the easiest) to have the CAM software setup with the theoretical/nominal tool diameter and specify the end result. The Tool Table would contain the actual tool diameter and the GCode interpreter would offset itself half the distance of the diameter in the tool table to yield that end result.

If I understand what you have written correctly, I believe this would be your option #1.

Is that not what I am doing?

I'm not sure I fully understand what you said, but no, the path in the GCode created by your CAM in both GCodes you posted is not what the end result should be. Instead it is a compensated tool center path.

Having both the CAM and the Interpreter both offset 1/2 the Tool Diameter doesn't make sense.

Note to see what the GCode Paths are you can enter 0 as the Tool Diameter and simulate the run and look at the GCode Viewer plot. You can also enter a few mm diameter either + or - and see how the paths offset.

Generally option 2 is the easiest, however it does mean if you have to change tool/allow for tool wear, you need to adjust the tool diameter in CAM, and re-generate the g-code, rather than simply changing the tool diameter in the machine.

Actually I don't think this is true. If the tool wears you should be able to enter a small negative Tool Diameter of the amount of the tool wear and run the Job without a need to re-generate the GCode.

I'm thinking your CAM program is set up as for Option #2. Because it is already offsetting 12.7mm and your actual tool is 12.72mm then if you enter a tool Diameter as +0.02 you should get the correct result.

HTH

[Moray]

Generally option 2 is the easiest, however it does mean if you have to change tool/allow for tool wear, you need to adjust the tool diameter in CAM, and re-generate the g-code, rather than simply changing the tool diameter in the machine.

Actually I don't think this is true. If the tool wears you should be able to enter a small negative Tool Diameter of the amount of the tool wear and run the Job without a need to re-generate the GCode.

In theory you could, however it would involve activating tool compensation and manually editing the g-code (unless you happen to program the original code with G41/42 and with a zero tool diameter).
It's one of these things that there are several ways to achieve the same end result, and I wouldn't say any one is better. You just have to understand the method you use, and any potential traps that could cause you problems.

The big trap with option 2, is making sure you've got the right tool numbers/diameters loaded in your CAM tool table, as you have the machine. Otherwise you end up doing stupid things like parts a mm or two the wrong size.

[a_j_p]

Hi again,

Took a minute for me to find time to sort through all of this but finally had the chance to do so. Tom was correct, my cam software does compensate the tool centerline and not the end result - entering a tool diameter value of 0.02mm in the tool table does correctly compensate for a 12.7mm tool that actually measures 12.72mm. Everything seems to be working great.

Thanks for the help!
-ANDREW