Today running a long rotary job I was about at +500r or 180,000 degrees. Then I went to the next op and it want a90. Needless to say it unwound to 90 the hard way. Where is the setting to not unwind but only move less than 360degres to get to the required location. It took awhile but I let it rip since I didn’t want to reset. Btw CAM was from fusion 360 if that matters.
Thanks
Tim
Yes, you can do this.
In the rotary settings menu there’s a “unwind rotary” option you can check off. This unwinds the rotary to under 360, so:
180300 would get “unwound” to 300 without moving the rotary.
If you have that option checked every time there’s a spindle start command the rotary unwind command is issued.
So if your second op had a spindle start command (M3) it would have been uwound.
If for some reason there was no M3 command you would have to split the G code up and run two files.
You can also issue a
M151/A
in the g-code to perform the equivalent unwind. You should be able to do this as manual g-code in Fusion between operations.
This command is embedded in our M3 (spindle start) command if you enable it from our wizard.
I put it in the M3 so if you have a CAM tool that doesn’t have the option to output that code (or you don’t wan to alter the post) you can just tick that box in the wizard.
Thank you both, so between operations that don’t have a any M3 change, but just a different place on the fixture will require me to either manually throw in an M3 or the M151/A, wonder if there is anywhere in the postprocessor for fusion I can throw this in automatically so I don’t have to edit the file every time. I haven’t looked at the post processor, but I am sure I can find somewhere to insert it, and expose it as a checkbox, ie unwind after each op? If anyone has suggestions where to start looking I’ll start seeing if I can modify the post processor.
Fusion posts are not easy to edit.
You can insert manual G code operations in Fusion though:
I haven’t really used this too much. You might be able to use “pass through” to type in G code:
Can you post your fusion file, or a screenshot of how your tool paths are setup? I’m curious how you have an operation that winds up so far, and then goes on to something else aren’t just two toolpaths without an M3 in between?
Here’s an example where this occurs: a rotary pocket pass followed by a parallel pass using the same tool and same spindle speed (with the guts of all the moves truncated):
(ROTARY TEST 2)
(MACHINE)
( VENDOR AVID EX ROTARY)
( MODEL CHETEX)
(T21 D=0.25 CR=0.125 - BALL END MILL)
G90 G94 G40 G49 G17
G20
G53 G0 Z0.
(ROTARY POCKET1)
T21 M6
S18000 M3
G17 G90 G94
G0 A0.
G0 X0.075 Y1.0196
G43 Z1.3963 H21
G0 A0.
Z1.3607
G1 Z0.9963 F125.
Y0. Z0.9607
G93 A-178.824 F40.023
A-357.692 F40.0129
A-360. F3101.3873
G94 X0.0736 Y-0.0064 F120.
X0.0696 Y-0.0103 Z0.9608
X0.0634 Y-0.0119 Z0.9609
X0.0554 Y-0.0117
X0.0454 Y-0.0095
X0.0354 Y-0.0073 Z0.961
X0.0239 Y-0.0037
X0.0125 Y0.
X0.001 Y0.0037
X-0.0105 Y0.0073
X-0.0205 Y0.0095 Z0.9609
X-0.0305 Y0.0117
X-0.0385 Y0.0119
X-0.0447 Y0.0103 Z0.9608
X-0.0486 Y0.0064 Z0.9607
X-0.05 Y0.
...
G93 A-139498.286 F58.3726
A-139676.667 F58.3415
A-139680. F3122.0968
G0 Z1.0607
Z1.4607
G94
G53 G0 Z0.
(ROTARY PARALLEL1)
G0 A0.
G49
G0 X0. Y0.051
G43 Z1.4598 H21
G0 A0.
Y0.0255 Z0.73
G1 Y0.0247 Z0.7085 F125.
Z0.65
Y0.024 Z0.6439
Y0.0217 Z0.6381
Y0.0181 Z0.633
Y0.0133 Z0.629
Y0.0077 Z0.6263
Y0.0016 Z0.6251
Y0. Z0.625
G93 A-178.928 F46.1104
Z0.6249 A-357.904 F46.1005
X-0.0002 Z0.625 A-360.696 F2932.0436
...
Y-0.0119 Z0.6281
Y-0.0169 Z0.6318
Y-0.0209 Z0.6367
Y-0.0235 Z0.6423
Y-0.0247 Z0.6484
Z0.65
G0 Z0.7085
Y-0.051 Z1.4598
M5
G53 G0 Z0.
G53 G0 X0. Y0.
M30
Note: despite the name change these are unmodified from avid machine configuration and post processor:
( VENDOR AVID EX ROTARY)
( MODEL CHETEX)
I would try my suggestion of manual G code entry and see how that works.
Another trick you might be able to try: set the RPM differently for each toolpath. That might force the post to output another M3 command. (M3 commands have the rotary unwind if you have that checked from the wizard)
You could set it to something like 18100 to force a change from 18k