Problems with full circle on Mazak M32

[rsbeadle]

Since updating my posts to V9 My Mazak won't cut a full circle contour, period. I tried to change all the new settings to every possible combination and can't get it to work. I can't get it to helix in a small pocket either. The tool makes an arc til it gets to the point where it should make another full circle and then plunges in a series of small Z moves that would be the position at the end of the full arc as it circles down the helix. Example is using a 1/2" mill in a .875 circle pocket making .1 depth cuts, cutting 1" deep (counterbore for bolthole). If I break the arc the contour will work, but not the helix. I can turn off the "output arc moves" option but I double the code output size. Thanks for any help.

[d0gFartz]

See if in your post the do_full_arcs is turned on,sounds like that might be the problem,its new for v9 posts

[perfecseal mankato]

this has been a problem since version 7

the tool path will only helix 1 time around

then plunge the rest.don't know if this will ever be fixed. I have a couple of projects sent in to q.c. the best way around this is circmill or ramp contour.You could try to helix in the other direction, sometimes this will help.

[Roger Martin from CNC Software]

For information on the post update process to v9, please go ->>

Start, Programs, Mastercam abd select "Post Processors - What's new in v9"

Whend the PDF opens, select the link -> "Post changes for FULL ARCS and HELIX ARCS capability in v9"

This will jump you to -> "Using do_full_arc and helix_arc functionality"

 

Updating a mill post from v8 to v9 using the update utility would not have changed the ability of the PST to cut "full circles".

 

The new variables it adds to a mill post that are related to ARCs & HELIXs are -> do_full_arc & helix_arc

 

With "do_full_arc : 0" in the PST, the post will act exactly like v8 when doing ARC motion.

(In v8 you would NEVER get an ARC move that did 360eg. of sweep in a single NC block)

With the setting above, v9 will act the same. A 360deg (full circle) in the toolpath will be broken into two 180deg motion blocks.

 

To get HELIX motion to work in the post as it would in v8, make sure that "helix_arc : 2" is set in the PST.

If you are not getting X,Y AND Z motion on the same circular block, the PST needs to be altered.

Exactly what needs to be added/altered is dependant on your specific PST.

It is a simple edit that you can try to do (make a BACKUP of your PST first!) or your Dealer can do this for you.

[rsbeadle]

Thanks guys. I think my main problem is getting the HELIX to work properly. I can set do_full_arc: 0 and break_arc: 1 or 2 and the actual CONTOUR arc is broken so that the machine reads two half circles or four quarter circles, but the HELIX still plunges. Code looks like this for .1" Deep smal circle helix:

 

bla bla bla

G0 X0. Y0. Z.2 START POINT

G1 Z.05 CLEARANCE HEIGHT

G3 X?? Y?? Z-.02 I?? J?? START HELIX

G1 Z-.04 PLUNGES

Z-.06 PLUNGES

Z-.08 PLUNGES

Z-.10 PLUNGES

G3 X? Y? Z? I? J? CUTS CONTOUR

X? Y? I? J? BREAK ARCS SET TO 2

G0 Z.2

 

I'm sure the code isn't accurate but I hope you get the idea. I monkeyed with the post a little with no success.

 

Thanks for the help.

[Thad]

Thanks for the excellent reply Roger! You just saved my butt. Not too many resellers open at 6 AM on Monday morning.

 

Thad