Page 10 of 16
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Sun Jan 24, 2021 12:14 pm
by Muzzer
I was posting the exact same setup with 003 (=G54), then reposting it with 005 (=E10). I did this many times and found the behaviour was very repeatable. Bear in mind I'm using the 4th axis here. I will experiment further when I have time but on the upside, I managed to make the part using the file created by 003. I'll let you know what I find.
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Sun Jan 24, 2021 12:21 pm
by tblough
What WCS do you have set in Fusion? If you have WCS 10 selected then V3 will incorrectly post that as G54, while V5 is correctly posting it as E10.
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Sun Jan 24, 2021 2:42 pm
by Muzzer
As far as I was aware, this was G54 but it's possible I'm mistaken. I have the digitising version, so it would happily support E10 by the sounds of it.
I have to admit, I didn't create the CAD and CAM for this (that was David Loomes) but looking into the various setups, I can't see the WCS being changed. Sounds like the most obvious explanation, though. Having said that, the version with the E10 line would have crashed the tool into the work, judging by how it behaved when doing an air cut, so it would raise more questions than answers for me!
The Fusion f3z file is here, if somebody could have a look and see any better than me:
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Sun Jan 24, 2021 3:21 pm
by swissi
Muzzer wrote: ↑Sun Jan 24, 2021 2:42 pm
As far as I was aware, this was G54 but it's possible I'm mistaken. I have the digitising version, so it would happily support E10 by the sounds of it.
I have to admit, I didn't create the CAD and CAM for this (that was David Loomes) but looking into the various setups, I can't see the WCS being changed. Sounds like the most obvious explanation, though. Having said that, the version with the E10 line would have crashed the tool into the work, judging by how it behaved when doing an air cut, so it would raise more questions than answers for me!
The Fusion f3z file is here, if somebody could have a look and see any better than me:
David Loomis dodecahedron v13.f3z.txt
Just right click Setup1 and go into Edit mode and you'll see that WCS# is set to 10:
- setup.png (8.87 KiB) Viewed 4157 times
-swissi
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Mon Jan 25, 2021 1:31 pm
by cbb1962
I opened the file and it has WCS = 10, Change it to WCS = 1 and it will output G54
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Mon Jan 25, 2021 2:18 pm
by swissi
It looks like this was not a bug in version 3 of my post processor after all.
I'm 100% certain I checked different WCS#'s when I added Probing to version 3 and I would have noticed if it didn't set the WCS# correctly.
I just tested the old version 3 with the latest update of Fusion 360 and it does set the WCS# correctly again so it looks like it was a bug in the last version of Fusion 360 that's been fixed with the latest version of Fusion 360 (2.0.9642).
If nobody reports any issues with version 5 Beta 3, I'll make it the official version.
-swissi
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Mon Jan 25, 2021 2:57 pm
by Muzzer
David Loomes got back to me after I enquired about work offsets in the file he said:
"If you right click on your cam setup, select 'edit' and go to the post-processor tab, you'll see the output wcs is set to 10.
That's because I keep wcs 10 for all 4th axis stuff. y and z axes are aligned with the rotary axis, so all I have to change is x. Just one less thing to have to worry about when setting up!"
So when I set my WCS origin, I would have needed to be in E10 whereas I was almost certainly in G54 / E1. That was waiting to catch me out - lucky I was doing a paranoid air cut!
Many thanks for looking into this - I thought I'd been through the WCS but it was hiding in plain sight. Hope I didn't waste too much of your time on it.
The post seems to be fine from what I can see!
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)
Posted: Mon Jan 25, 2021 5:09 pm
by cbb1962
Muzzer wrote: ↑Mon Jan 25, 2021 2:57 pm
Hope I didn't waste too much of your time on it.
Not at all, once I wrapped my head around what all could be done with multiple WCS systems I found all kinds of uses. Generally, I use G54 for the top of my spoilboard and G55 for the top of the part, unless I can have a production run like the one below then I take WCS to the extreme.
These boards were machined using 2 g-code files, one for the face and one for the back, each program utilized 8 different WCS's! Fusion 360 made it easy to do.
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)
Posted: Tue Jan 26, 2021 12:39 pm
by swissi
A new version of the Post Processor has been posted in the
first post of this thread.
***Change Log v5
- The check for redundant Tool # (same Tool# with different tool geometry) is now a Post Processor Property that can be turned on and off. The default setting is to check for redundant Tool#
- The maximum number of tools can now be adjusted in the Post Processor Properties. The default is set to 200 tools matching the CNC12 tool library
- The activation/deactivation of the coolant command (M7/M8 and M9) has been optimized and is now placed at the point when the Z axis is at the clearance height
- When using the Post Processor Property “Check/Update CNC12 Tool Library” it was possible that a message was displayed that the tool diameter in the Fusion 360 tool library is different from the CNC12 tool library but they were displayed exactly the same on the screen. This issue was caused by CNC12 internal rounding errors. The new diameter comparison method is now using a comparison tolerance factor that solved this issue
- Program Numbers that are reserved for CNC12 (9100 - 9999) are creating issues when being used in the Post Processor. This Post Processor will now create a post error with a log message that these program numbers can’t be used
Please post here if you find any issues.
-swissi
Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)
Posted: Fri Jan 29, 2021 4:21 pm
by nicolasjolliet
Fabulus, Thanks Swissi, I'll check it out.
Would it be difficult to port some of these features (like using letters instead of program numbers) to the default centroid turn post processor in the fusion's library? I'm scared of trying to program a new post myself.