WCS

[cnc@gci]

Is there a way to change my part origins after all my tool paths are created. I have a HMC with parts on a fixture, I had just one offset for the whole fixture, but I think I need a differant offset for each part.

[Dan@home]

If you set all your origns to be (associated) to one (point), you have to have all your toolpath parameters set to Inc. Otherwise the toolpaths will move with the moving of the point. If you have them all set to Inc. the toolpaths will stay on the part but only the orign will change.

[cnc@gci]

I have 4 parts on the fixture and I want each one to have to have its own offset. but I already toolpathed the parts with just one offset on the fixture, can I change that with out retoolpathing the parts..

[Dan@home]

Create a new view with a new orign, then go into your planes button located in the toolpath parameters, select the two little arrows on the bottom left to expand the Toolpath Coordinate System window to show three windows change the last two, (Tool Plane) and the (Construction Plane) to the new view you created. Don't change the Working Coordinance System window. You will have to do this to all ops that you want to change the orign of.

[Dave Ball]

yes maybe, no maybe. It depends on how you chained your operations when programming them. If you chained multipule parts for each operation, then no, however if you chained each part seperatly then yes it is possible to set up seperate work offset without rechaining all of the geometry.

[Steve Arteman]

Not sure if this has what you are looking for but its free anyway, take a look.

http://www.cad2cam.net/zany.html

yes you can change the offsets in each toolpath as shef said they need to be seperate ops. for eack offset

steve arteman

www.cad2cam.net

[cnc@gci]

Everytime I change the toolplane and then try to change the construction plane the working coordinates changes to. How do I get it to not do that?

[Dave Ball]

uncheck these two boxes in system configuration. "Update Cplane and Tplane when changing Gview" and "Reset C-plane to Top in Iso Gview"

[cnc@gci]

Thanks guys that thats a big help, but when I post it says 0-work offset number used in more than one view. And I only get one offset number in my program, what am I doing wrong.

[cnc@gci]

I think I got it figured out, thanks guys you,ve been a huge help.

[Dave Ball]

click on the parameters of an operation to get this...

 

 

in the lower right corner click on the Planes button to get this...

 

 

in the lower left corner enter a work ofst number 1 thru 6. 1=G54 2=G55 3=G56 etc.

 

make sure the center Tool Plane area has the name of the desired Tool Plane listed at the top, if not, click the small button to the left of the arrow button, in the tool plane area to get this...

 

 

and then select the desired Tool Plane. Green check your way back out of all windows and repost.

[cnc@gci]

Sheffercnc You're awesome man.

[Na Dtuath]

I allways get that "0-work offset number used in more than one view" warning when I post out more than one work shift offset...I just ignore it.