5 axis curve A axis rotation problem

[dforsythe]

Kind of weird, but any idea what might cause the tool path to want to rotate to this number after the cut is complete. All other tools ran fine. Its cutting the profile of a part.

 

 

code:

---

 X-6.3953 Y-4.6858 Z-.5167 A389.046 F239.89

X-6.2954 Y-4.6875 Z-.5117 A389.039 F239.92

X-6.1955 Y-4.6892 Z-.5067 A389.032 F239.93

X-6.0956 Y-4.691 Z-.5017 A389.026 F240.04

X-5.9957 Y-4.6927 Z-.4967 A389.019 F240.04

X-5.8958 Y-4.6945 Z-.4916 A389.012 F239.86

X-5.7959 Y-4.6962 Z-.4866 A389.005 F239.97

X-5.696 Y-4.698 Z-.4815 A388.998 F239.92

X-5.5961 Y-4.6997 Z-.4764 A388.992 F239.94

X-5.4962 Y-4.7014 Z-.4714 A388.985 F240.05

X-5.3964 Y-4.7032 Z-.4663 A388.978 F240.06

X-5.2965 Y-4.7049 Z-.4612 A388.971 F239.97

X-5.2457 Y-4.7058 Z-.4586 A388.968 F472.28

G00 Z-.2086 A28.968 ****crash*****

Z6.5414

M84

M05

G91 G28 Z0.

G91 G28 Y0.

G90 G54 X-53.1

G28 Y0. A0.

G90

M30

---

[Verndog]

There is a problem with wind up in your post. The A move you are rapiding to is the exact same position the machine is already at only 360 degs. away from it. I'd really need to see the post to find the problem.

 

As a work around you can select force tool change on this operation and the post should reset the initial move back to A28.xxx before making this cut. It will throw a Txx M6 in but machine will do nothing if left besides rapid up turn off coolant and spindle then go back and start cutting again. Re posting will be safe this way also.

[dforsythe]

That makes sense. The post is just a mpmaster. Any suggestions on where to find the wind up information inside the post?

 

Thanks for the help

[Verndog]

Look for a section like this.

 

pcoutrev #Rotary axis revolution calculation (Modify for wind-up)

cdelta = csav - prv_csav

while abs(cdelta) > ctol, #If motion exceeds ctol, add wind-up

 

xx

[dforsythe]

Easy enough to find, not sure what to change.

[Verndog]

Is this a rotary/tilt 5 axis with 360 on A and over 90 degs. on C?

 

If so, and you look at your toolpath there is no need to make this cut in 5 axis curve. Also...if true, that cut is nothing more then a fancy coded 3ax profile done in 5ax curve (unless there are C moves not posted somewhere in path)

[dforsythe]

The set up is on a 4th axis. The part is a dished rectangle shape. The tool path cuts a 5.0 deg angle around the part on a vacuum fixture. The end mill is moving in x,y,z and the A is rotating around to match the angled edges on the front and back. I probably didn’t explain it very well. Im sure a picture is worth 1000 words.

We do several versions of this part and have never had an issue like this before.

 

Anyway, thanks again for trying to help.

[Verndog]

Ahhh...that makes sence now. Your running 5ax curve posting in 4ax mode with vertical 4 axis machine.

 

Try this. Its winding up the rotary axis prob. because of previous cuts and where it left off. Make a toolplane that is identical to the one your in (Likely Top) and save it. Then pick that toolplane before making this toolpath. That may trick Mastercam into unwinding and starting from A0 to begin this cut. Editing the post takes time and experiance...and often 1 change leads to several sections of post mods.

 

Also...option C...above the part, you can create a 5axis curve toolpath that forces (rolls) the rotary axis (at high feedrate) back toward A0 then the next toolpath (the one you posted) will roll back to A28xxx to begin. This can be done with 1 curve and 2 lines.