Cutter Compensation for Rough / Final Cuts

I am profiling some 12 mm steel plate, side frames for a 5" gauge locomotive.
The profile includes deep wide slots for the bearing blocks, and subtle curves.

The desire is to get acquainted with G41/G42, and G41.1/G42.1.

I am getting "Tool radius not less than arc radius with comp" when I load the file with G42, and a small diameter tool.
After investigating I can see the problem, the error message is correct.

I used CAM to generate the path with a specified cutter diameter, then edited the file to add G42 and tool change aiming to get a roughing pass first.

My question is:
What is the best general approach to achieve roughing cuts, then final cuts?

Keep well,
John (in Sydney Lockdown).

 

You might be doing radius compensation both in the CAM and in the controller. (ie. twice). If you needed to tell the CAM the tool diamtere then it will already have offset the paths.

One option might be to tell the CAM to use G41, and then you can edit the numbers.

Which CAM?

Thanks for the comments Andy.

I use CamBam and entered the diameter of the desired tool.
The code produced uses some small radius arcs for the tool paths at internal corners.
Eg: for a fillet of R6, a Dia10 tool moves in and arc of R1.

So, if I attempt a G42 with a tool Dia3 (to get a roughing pass), LC quite rightly complains.
I can sort this out, but it appears I am approaching this the wrong way.

What I did was use a slot drill to mark out the desired profile, then a combination of various tools to manually machine up close to the marked edge.
Hence the need for a systematic roughing pass, then a final to size.

One aspect of the descriptions for G42 is that of gouging.
How many steps does LC calculate in advance for G42 ?
Is it just the current step, or does it allow for the subsequent step to avoid a gouge ?

Keep well,
John.

What is your input shape? The profile must be a shape that the selected cutter can touch all of for G42 to work.
If the shape is suitable, but then CamBam creates an offset profile with sharp corners because it is adding an offset to the G-code then the resulting path will not be compatible with G42.

So, I think that you probably have to turn off cutter comp in the CAM. Though it is possible to use both, for example using 6mm cutter in the CAM and a 1mm dia then 0mm dia in the G42 for an actual 6mm tool.

I didn't put cutter comp into the CAM, I hand-edited the file to add G42 and the change in tool (diameter).

I generated separate files for 16, 14, 13, 12, 11 and 10 mm cutters without G42..
All passes used a (12) 10 mm tool, side cut at full depth, and completed this job.
The minimum design fillet radius was 6 mm.

Your suggestion will be taken on board and trialled on the second plate.
That is essentially what I was trying to do.

Another investigation is whether CamBam can be instructed to code with a selected minimum tool path radius.

John.

You mentioned that you told CamBam what the tool diameter was.
If it isn't doing cutter-comp in the CAM then it doesn't need to know.