a axis subprogram transform

[rchoward]

i am using ver8.1.1

 

thank u for your help the past now i have a problem i cannot beat any suggestions would be great

 

i love mcam but it is a code hog i use subprograms, join entites, and i am still getting dicked here

 

my control (okuma u10m) only has 126k of program space and i need to fit a big roll die program in.

 

this is a y axis substitution type part

 

the part is a pocket the same 10across rotated at three intervals 120 deg around the part can i pick a chain and tanform it across and around the part (ican in the control using a modein mode out command) but can i do it inside mcam all on the same work offset?

 

bascially i want to put a subprogram on a grid perhaps incrementally

 

ican post on ftp if my description is poor

 

thanx

[gstephens]

It sounds like what you really need is v9 where you can transform a transform (rectangular then rotate) In v8 I think your only options are chain ALL 10 pockets in 1 toolpath then rotate it around 3 times, or build each of the three rotations for 1 pocket, toolpath them, then transform rect. it 10 times. The latter will most likely have less code, but your part will be spinning around a lot.

[Part Factory]

I'm not a MasterCam user. You could be trying to hard getting CAM to do a simple thing.

 

A solution that I use is to create a subprogram or a subroutine:

[*]1 Post the output for one pocket.

[*]2 Replace the M30 with a M99.

[*]3 Create a small program that prepares the tool and executes a coordinate system rotation G code (my Haas uses G68 R-angle)

[*]4 Call the subprogram.

[*]5 Reapeat for the remaining angles.

Tip:

This is a brief explanation of the process. If you have not done this before then walk before you run. I always test a concept with a prototype program (a long rectangle move). Watch, learn, and improve. When the comfort level is right go for more. Over the years I have built a collection of pulletproof G-code templates that assemble exactly what your doing in a couple minutes.

[Jim Evans from CNC Software]

rchoward,

 

The problem with transforming a transform in V9 is that subprograms are NOT supportted via the post in both transform operations. The MP executables will disable the subprograms in the sceond transform and the posts are not setup to handle them.

 

If you are going to use Axis Substitution toolpaths in transform, DO NOT use ROTATE. You must use Transform Translate of the flat toolpaths. Axis Substitution toolpaths are required, by the post, to be done in the flat (not rolled). Then you can perform a linear translation on it using transform to get what you are looking for.

 

Do a search of the forum as I believe this topic was presented not too long ago.

 

I hope this helps!