Help please with Mastercam V9

[emimec.19@btint]

I have mastercam V9, and am not the programmer in the shop, so please bear with me. My pal, who uses mastercam, tells me that having drawn out a part, and then run the NC file and sent it to our Bridgeport interact with a Heidenhain TNC 151 controller, there is a small problem. It appears that he is unable to adjust the tool compensation on the controller direct? I think what he is saying is this: if programmed manually at the TNC 151, he can adjust the tool diameter to allow for tiny compensation in tool cuts, basically he can "Lie" to the controller about the tool diameter. But when a programme is done via a drawn out part in Mastercam, and sent to the TNC151, he cant make this change. Is this making sense? Any ideas please on how to "lie" to the controller.
Bob.
London UK

[Superman]

I'm not sure on Heidenhain, we have Millplus,

What values are you puttinig into the rad. comp ?
If you are using R=0.0 in the machine, then your mate is either using "wear" or "computer"
If you are using R=(1/2 tool diameter) in the machine, then he's using "control"

Tool compensation can only be done on paths using "control", "wear" or "reverse wear"

"wear" says it all, it allows for small +-adjustments, regrinds, etc. not large over-compensations, like a 1" tool path over-comped for a 2" cutter.
Sometimes, the machine's parameters cause tangency errors on a compensating toolpath.

"control" on the other hand allows for this situation, the actual toolpath is the comp to profile, as long as the lead in and out accommodate the tool and there is no internal arcs smaller than the tool radius, then all should be OK

The only danger is the these methods cannot be mixed on the same tool( the control may allow R1=0 and R2=tool rad )( ie T1R1L1 is a different tool to T1R2L1) but like I said not sure on Heidenhain

[emimec.19@btint]

Hi, and thanks.
I think my pal is using "computer". I do recall him playing with the options, but on the computer screen, nothing was seen to visibly change. I dont know if it would have if he had sent the file to the TNC.

Regards
Bob

[Superman]

Sorry, the only one I left out was "computer"

"computer" is what it means, Mastercam controls the toolpath, you tell Mcam the tool diameter and the toolpath is only for that tool diameter. There will not be any G40/G41/G42 output with those paths for the operators to adjust the t/path on the machine. You could add the codes manually.

The "computer" toolpath is the "wear" path, but with cutter compensation option taken away from the operator.

and the other " reverse wear", I don't use. I think it outputs G42 instead of G41, from memory