work coordinates output in rotated toolpath

[Tom]

 

Anyone in here can show me how to turn off

and on the work coordinates ( G55,G56...) outputting in the nc file of the rotated toolpaths. For instance, I rotated a simple

toolpath around to mill a hex on rotary axis.

Each time the toolpath rotated, it output

G55,G56,G57..Unnecessarily

I wonder if there is an option to turn it on and off or I'll have to configure my post?

I'm TOM. A new user of Mastercam. The Version

I'm using is V8.1.

your help would be greatly appreciated )

------------------

TL

[gregm]

What post are you currently using?

I live for that type of output, but I

would think the stock MPFan wouldn't act

that way.

I could be wrong....

 

GM

[Guest CNC Apps Guy 1]

You may want to try changing the following setting in your post.

force_wcs : no

------------------

James Meyette

[Elad]

Changing force_wcs to "no" doesn't solve the problem.

You can try to set "work offset" (in the t/c plane) to 0 in all the operations.

I tried it,and when posting,i got the message : "work offset number used in more then 1 view", but the gcode looks good, and it use G54 at all the operations.

I didn't try this on the machine,but i think it can work fine.

let me know if it works for you

 

[Allan Brown]

Setting the Work Offset to -1 leaves the WCS mode in 'automatic' - allowing Mastercam to set up a new WCS value for each toolplane. When setting the origin at the centre of your rotary 4th axis, this is not necessary. You can either set all of the Work Offset values to 0 to for a G54, or you can download Mpmaster from the Posts area of this site and use the Misc Values setting "Lock on First WCS [0=No,1=Yes]". Setting this value to 1 will lock on the first WCS value to override this problem.

[Elad]

I tried to set the work offsets to 0, but in few operations the work offset was grey,and i couldn't change it!

anyone knows why?

Thanks,

[This message has been edited by elad (edited 05-07-2001).]

[gstephens]

Never mind

[This message has been edited by gstephens (edited 05-07-2001).]

[Tom]

Hey! ya da man!

your solution works perfectly for me

I got a warning same as yours "work offset numbers used in more than 1 view" but that is normal. The output looks better

thanks a bunch, Elad, Dave and

many thanks to those who responded the question

------------------

TL

[Tom]

Elad, about the problem you mentioned earlier

let' try this see if it works for you,

in operation manager select renumber work offsets then set:

starting work offset number: 0

work offset number increment: 0

check the " use matching..." window

and the "overwrite work offset.."window

have fun!

[Elad]

I tried it already,it doesn't work!

I renumbered the work offset but nothing happends!