Subprograms A-axis

[wfcPain]

Is there a way to use subprogram for a-axis incremental moves of 7.2 deg.?

 

I've always hand type it. ex. M98 P1300 L50.

[Allan Brown]

If would need to be a custom, application-specific post, like Mpsubrep with angular reps.

 

Mastercam doesn't really support sub repeats, with inc values, like Z for a depth cut.

 

You can take one op, and do a Tranform, Rotate op with subprogram output. Your output will be abs angles with a sub call after each

 

G0G90A0

M98P1100

G0G90A7.2

M98P1100

G0G90A14.4

M98P1100

 

etc.

[wfcPain]

Thanks, dave that's exactly what i was looking for.

My output for the first 5 rotations is fine, but then it starts putting a p # on the rest.Example line 104,118, p1 thru p44.

Also it goes to g28 z0 everytime.any ideas?

 

N94 (ENGRAVE MARK)

N96 X0. Y0. Z2.

N98 M98 P12016

N100 M05

N102 G91 G28 Z0. M09

N104 G00 G90 G54.1 P1 X0. Y0. A-43.2 S3000 M03

N106 G43 H1 Z2. M08

N108 (ENGRAVE MARK)

N110 X0. Y0. Z2.

N112 M98 P12016

N114 M05

N116 G91 G28 Z0. M09

N118 G00 G90 G54.1 P2 X0. Y0. A-50.4 S3000 M03

N120 G43 H1 Z2. M08

[code]

[Allan Brown]

Try to not allow the Work Offset numbering to increment. Keep it at 0 for G54.

 

If you post has a Misc Value to 'lock onto first WCS' then use that.

 

Basically you are getting G54 through G59 then G54.1 P1 and up as the Work Offset value is automatically incremented by Mastercam.

 

The retract is something in the post to do a full retract when the toolplane changes.

 

Mpmaster has a switch

ret_on_indx : 1

 

Machine home retract on rotary index moves, (0 = no, 1 = yes)

 

If using Mpmaster, you'd set that to 0.

[PeterM]

You can also do this to supress new workshift creation. In tranforms first page on the lower right there are selections under work offset numbering, one of the selections is assign new, check that, also check match existing offsets. This combo works for me. Peter

[wfcPain]

SUCCESS!!

Thanks dave and peter!

I seen assign new,but i thought, i don't want a "new" work offset. I want the same offset,g54.A bit confusing, but i see now.

code:

---

N10 G00 G90 G54 X0. Y0. A0. S1069 M03

N12 G43 H1 Z.1 M08

N14 M98 P12016

N16 G90 X0.

N18 M98 P12016

N20 A-7.2

N22 G90 X0.

N24 M98 P12016

N26 A-14.4

N28 G90 X0.

N30 M98 P12016

N32 A-21.6

---