Is it possible to only home Z after a program? Meaning stay in place after the program has been run and get the bit out of the way?
I’ve yet to crash the machine during a program, it’s after the programs are finished and the machine rapids home (straight diagonal angle) that I’ve crashed a dust boot into a clamp. I’d like to avoid this and jog the machine with the joystick after it’s over.
Apologies if this has been covered before.
Thanks in advance!
_Mike
That’s entirely a feature of your CAM. Fusion 360, for example, annoyingly insists on moving the router to home (or a coordinate you define) after milling. Carbide Create (if I remember well) does not.
You could edit the g-code and remove the G0 command to return home.
If your CAM doesn’t allow you to stop that, then increasing your safe Z height will keep you from crashing into your clamps.
Thank you! I will look into Fusion 360 to address this. I hope there is something that I can do to the post-processor so I don’t have to remember every time.
_Mike
Thank you! I was thinking the same thing and will likely make a different dust boot that travels with the router. If I do this and what you are saying I shouldn’t have an issue. The suck-it system is what is crashing since it is stationary. It makes sense for some operations but not others.
Thanks again for the reply!
_Mike
Quick update.
I was able to achieve what I was trying to do with a quick manual delete of a line g code.
Here is what the last bit of code for each program looks like for me:
N620 G1 X29.648
N625 G3 X30.283 Y57.785 I0 J0.635
N630 G1 Y58.42
N635 G19 G3 Y59.055 Z-18.415 J0 K0.635
N640 G0 Z15.24
N645 G17
N650 G53 G0 Z0
N655 G53 G0 X0 Y0
N660 M30
%
I delete the line with “G53 G0 X0 Y0” and modify the last line to read “M2” so it looks like this:
N620 G1 X29.648
N625 G3 X30.283 Y57.785 I0 J0.635
N630 G1 Y58.42
N635 G19 G3 Y59.055 Z-18.415 J0 K0.635
N640 G0 Z15.24
N645 G17
N650 G53 G0 Z0
N660 M2
%
Now when the program ends the Z raises up to home and it stays in place regarding to X and Y so the Suckit doesn’t crash into clamps.
I plan on looking into how to update the post so I don’t have to do these manually, although it isn’t much trouble. I found this video, it seems attainable.
Thank you for your help on this! This is a great forum.
_Mike
If you are using Fusion 360 all you have to do is select clearance height from the safe retracts menu. After job the machine will retract to Z clearance height and then stop. You can move with the joy pad after. Simple 
@alldaysammyj I am using Fusion 360. Thank you this is so much easier! I’ll give it a try this evening.
BTW - Do you have a Fusion fix for posting M2 rather than M30 at the end of the program? M30 sends the spindle to the start of the program. For me anyways. No worries if not.
Thanks again,
_Mike
Captain PostProcessor (aka @blaghislain ) maybe able to help.
Unfortunately I haven’t posted M2 vs M30. Check in the settings menu on the 1F controller. You might be able to enter it in there.
Wow! Excellent tip, thanks. I wish I had seen this earlier.
It’s probably easy to fix but I dont Understand the issue having m30 instead of m2. Can you explain so I can better resolve your issue and test.
@blaghislain the issue I was having with M30 was it was sending the program back to start and running it again. M2 ends the program where it sits and it much preferred for my current workflow. I’m not sure if this is an issue for anyone else.
Thank you for looking into this.
_Mike
@MustCreateThings Just created a new dev_1 branch to the github repository. Give it a try and let me know if it’s ok to release.
see README
see CHANGELOG
download link
New properties are disable by default. You will have to enable them manually by editing your NC Program.
@blaghislain Wow thank you! Unfortunately the download link isn’t working for me. I’ll search the page for a latest build in the meantime.
_Mike
@blaghislain I found the branch you referenced.
Is the M6/M0 box meant to pause the program between each process? I can see this as a great feature for proofing a program. If I want to group processes in a single post (all using the same tool) I’m assuming I would not check this box so it will run through all of them without me having to be standing at the machine.
Thanks again. I’ll report back.
_Mike
fix the bad link.
The M6/M0 feature came from @Aiph5u suggestion here. This permit to probe for each tool change. User that dont need the pause can use the native ‘Output M06’ property.
@blaghislain Thank you again for reving the post processor.
The M2 function is working well and perfect for what I was looking for. The M6/M0 check box is always triggering the pause feature regardless if it is checked or not. Not an issue for me just yet but I would prefer to not have to be at the machine when I link multiple tool paths with the same tool, which I do 80% of the time.
Again thanks,
_Mike
Thanks for getting back this fast. I must appologize for the M6/M0 to be always trigger. I found a copy paste typo. This is now fix.
@blaghislain 've downloaded the new post (same location) and will give it a try this afternoon/evening. Thank you for making the update so quick! You rock!
