how to do point to point with edgecam??

[tony_skipper]

Is there a way to do point to point with Edgecam? Do you have post processor examples that permits it?

We need this because our milling machine is enable to interpret circular interpolation command (G2 and G3) in XZ plan (just in XY plan).... So the only remaining solution seems to do point to point in replacement of these circular interpolations...

Any cue on this?

Regards, Tony

[sea-n-see]

** disclaimer ** I'm new to post editing so test and re-test to be sure.
I believe in the Code Wizard under Machine Parameters you can specify "Arc Planes" as XY only. Yours may be set at XY+ZX+ZY by default. Click the Help Button on the Machine Parameters tab and read about Arc Planes.
What control are you outputting for? Most should still be able to do arc moves in the XY plane. Your controller may be looking for specific values for arc moves. One of mine requires the end point and signed I + J from the arc start point while another can use start point, end point + rad.

[timf]

i believe there are a couple ways to get that output for any plane.
what cycles are you having this problem with?
are you doing 3-d? who made your generator?
may try this:
one the first page for profiling the nc output smoothing has a line arc button, make sure that is not on that lets g2 and g3 be output in xz and yz.
or
i'm sure somewhere in the code generator you can restrict this, i have actually went thru the effort of making sure mine will output arcs in all 3 planes to save on program size but my machines dont have a problem with them.
if you wrote your generator try to look at the areas that control the output for arcs.
go into the code constructors/general motion/circular interpolation(both directions) and make sure the I,J,K values are not forced.

run the code trace and see what area the output comes from, that will help you restrict it, be careful you don't restrict all I,J,K output or you wont get it in X,Y and your program size will increase dramatically based on tolerance settings.

always save a back up first.
good luck

[jstikeleather]

Also check your 'Machine Parameters' page, look at the top right area for 'Arc Planes' and what is allowable.

[tony_skipper]

Thanks a lot everyone! The problem is solved by marking "Arc Planes" as XY only.

I really appreciate your help,

tony_skipper