[Crashmaster]

Hi guys,

I have what I am hoping is a very simple problem with using multiple work offsets (g54-g58) in MC. I currently generate a tool path and then have to copy that tool path 4 times and individually change the offset #(0,1,2,3) in the WCS tab for each tool path. There has got to be an easier, less time consuming way to achieve this.

-CM

Oh- I am currently using MC X4

[Superman]

Yep,
Try the Transform,
You should end up with 1 operation and 3 repeats at the same place,
modifying the 1st operation carries automatically over to the other 3 paths

[Crashmaster]

Thanks for the reply. I tried using transform. Maybe I don't understand the concept behind this. If I leave the type on translate the work offset numbering options are grayed out. I'm assuming I want to use translate and not rotate or mirror. I've tried to find info on this on the MC help menu but can't.. Any suggestions?

[Superman]

-Select the operations you want transformed
-Select the Type of transform (trans, rotate, mirror)(Tplane origin ON for offset # output)
-Method ( toolplane=offset numbers come into play, Co-ord=adds a distance to the NC output values)
-group NCI ( machining sequence if 2 or more ops or tools )(order=finish 1 part in op order before moving to the next, type=fininh each op across all parts before moving to the next op )
Copy source ops =ON
Disable=depends where your source ops are placed
Work offset - assign new start=1, Inc=1 ( your start # may be 54 )

[Crashmaster]

Thanks superman, I think I got it now. much appreciated!

[Superman]

By the way, there is another method instead of transforming

simple to implement for single view parts
is copy to the WCS 3 times and change the work offset number for each

pros
-you can see and plan exactly the sequences you want
-view this method as the step before understanding transform

cons
-lots and lots of ops
-greater chance of errors ( modify a path but not all paths or the wrong one )

[Crashmaster]

Thanks for the info. I can't believe this wasn't discussed in the in program help guide or the manual. I must have missed it!