5 axis drilling

[MetalSlinger5]

seems like no matter what I do in the mastercam toolpath parameters, when I drill multi-axis holes on the Haas UMC machine, after each hole the machines G53 Z0's before every hole (tilt & rotation move), this has to be a post issue, correct?

 

(SPOT HOLES FOR KNKDL1032J KEENSERT)
T14 M06 (1/2 X 90DEG SPOT DRILL, 1.5)
G54 G17
S1528 M03
B90. C-82.957
M10
M12
G254
X-2.4008 Y-.5802
G43 H#3026 Z6.0269
M8
G94
G98 G81 Z4.8034 R5.1268 F12.22
G80
Z6.0269
G255
G53 Z0.
G54
M13
B90. C-82.475
M12
G254
X-2.4227 Y.4113
G43 H#3026 Z6.0262
G98 G81 X-2.4227 Y.4113 Z4.8026 R5.1261 F12.22
G80
Z6.0262
G255
G53 Z0.
G54
M13
B90. C-78.596
M12
G254
X-2.5393 Y5.5522
G43 H#3026 Z6.2507
G98 G81 X-2.5393 Y5.5522 Z5.0272 R5.3506 F12.22
G80
Z6.2507
G255
G53 Z0.
G54
M13
B90. C-69.129
M12
G254
X-2.3771 Y9.6105
G43 H#3026 Z7.5914
G98 G81 X-2.3771 Y9.6105 Z6.3679 R6.6913 F12.22
G80
Z7.5914
G255
G53 Z0.
G54
M13
B90. C69.129
M12
G254

 

so on and so forth??

[Greg Williams]

Yes correct, the G53 Z0 comes from the post. I think that code looks good. The post cannot know your setup or what holes you are drilling next and if there will be interference, so post guys er on the side of caution and add the retract in between the holes. Some posts have a retract switch add into the Misc Reals. maybe your does?

[crazy^millman]

I believe G254 requires a G53Z0 when changing planes. That is the same way CAMPLETE posts code. I have programmer several jobs for UMC-750, UMC-500 and the UMC-1000 and all of them using G254 output G53 Z0 at planes changed when doing 3+2 and no one tired to do what your asking for wanted it. Might need to check with your Local HFO and make sure that is not needed. I cannot be 100% sure since I cannot get in front of a machine and test it.

 

[Miki67]

I got this in my  misc

[crazy^millman]

Then you will nee to manually change the code and test on the machine and see if the machine will allow what your looking for. If the machine required it then you're stuck with what you are getting doing it with canned cycles. Switch to long code and should be able to do what your after with a Wrap Safety Zone. Like I said reach out to your HFO (HAAS FACTORY OUTLET) and talk to an applications person and see what they say about what the machine needs. You can confirm then you need to reach out to your post builder and have them make the changes to reflect what the machine will accept. At that point you assume all liabilities for any crashes or collisions because you requested this change. 

[Leon82]

Camplete has the 3+1 block which you can remove the Z0 (works on fanuc). It only uses it at A-90 only when the c axis changes though.

 

Have you tried making separate ops and then using multiaxis link?

It's a little more programming but if you have a million pieces I guess it's worth it.