Post problem

[Mgrenier]

Hello everyone,

I am trying to modify my post for a Fanuc controller. I am using the "post processor user guide - september 1997" book. In the parameter Gcode tables, for pocketing, I can identify these:

Gcode 10008 for cutter compensation in computer

Gcode 10007 for cutter compensation in control

But I can not find the Gcode parameter for wear cutter compensation. One more litle thing, when I check the value of these values in my post, How are they going to come out for left, right or no compensation. Any help would be greatly appreciated.

[Mgrenier]

Sorry for the omission, We are using Mill level 3 and the post is a Mpmaster derivative.

Sorry once again

[Guest CNC Apps Guy 1]

You will not find "Wear" compensation anywhere in Mastercam except in V9. Ooops I don't think I was supposed to say that. Anyway, "Wear" Compensation is accomplished by turning Compensation ON in the Computer AND ON in the Control.

Hope that helps.

[Simtech]

Martin,

Salut, comment ça va!

Well, James is on the mark here. Wear cutter comp is a new feature for V9. Variables should be available like others with the post.

My suggestion for you is the new MP Post Processor Guide, version 2001 in CD format written in PDF permitting searches and fast lookup's.

I'm going to e-mail you an example of this.

Luc Simoneau

[Mgrenier]

Thanks James and Luc,

I just want to know one thing: If Mastercam does not handle wear compensation how come the system gives you the choice of activating the wear compensation in the pocket mode? That is why I am asking the question mentioned above.

Thanks,

[Simtech]

Martin,

The wear option in Pocket will affect the cutter compensation variable, being the same as a control compensation with the difference that the coordinate's outputted will be offset but not center line.

Hope this helps!

Luc

[Allan Brown]

So for 'Wear' comp in pocket, perhaps both the parameters for computer and control would be set to 1?

[Mgrenier]

Hello again,

Thanks for the replies, after reading these, I was wondering if there was something that I could use in my post to determine which of one of the compensations is used : control, computer or wear. Off course, I am still talking about a pocketting operation.

[Simtech]

Martin,

NCI variable 10350 is used to determine the type of cutter compensation used in a pocket finish toolpath.

In computer: 0

In control: 1

Wear: 2

Dave, can you answer on how to get this info into the post?

Luc

[bryan.davis]

Actually the ommision of wear compensation in MasterCAM 8 isnt quite correct, you can simulate wear compensation by setting both cutter compensation options to yes.

I can make comments on MCAM 9 because what I say is based on what Ive seen in demos, rather than me being part of the beta program.

MCAM 9 has changed the way it presents the offset options, they have replaced the two settings with two opions each (giving a possible 4 permutations) with a single setting with 4 options which gives you the same 4 permutations as version 8, but this time they are named and a little easier to understand

[Allan Brown]

Covering parmeter tables would be fairly involved.

Perhaps check out the stock left parameter example in Mpmaster.

Search for the following:

pparameter - calls up to the parameter tables based on opcode

fprmtbl - tables to assign variable names to parameter codes

pstock - postblock to output stock variable

1501. Insert parameter information in the ascii NCI? n

1502. Write operation information to binary file (.ops)? y

[Mgrenier]

Thanks a lot you guys tried everything you said and I am finally able to output the tool radius compensation value directly into the NC program without any intervention from my part. Once again, a big thanks to everyone.