Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

mrichards
Posts: 34
Joined: Thu Feb 28, 2019 12:05 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 3)

Post by mrichards »

swissi wrote: Thu Apr 04, 2019 3:30 pm Check for conflicting Tool Numbers (same Number but different Tools): Logic has been added that checks for conflicting Tool Information e.g. using the same Tool Number but with different geometry.
In F360, I have some mill-drills https://www.lakeshorecarbide.com/altinc ... mills.aspx set up as three different tools with the same tool number:
-As a twist drill for drilling ops
-As a endmill for side milling ops
-As a chamfer mill for chamfering ops

As far as I know, this is the only way to handle this type of combo tool in F360 as the different tool types have different settings available that are required for the different ops, particularly milling vs. chamfering. I think the drill definition is probably not required as I think you could probably drill with a endmill.

Anyway, I get an error during the post about the differing geometry for the same tool number. My current workaround is to use a different tool number for the different ops and edit the .nc file after posting to set all the ops to the same tool number. To complicate this is the fact that the post creates unnecessary tool changes as it thinks the tool numbers are different. For now I'm editing out the M6 tool change.

Related; For "dummy" tool numbers above, it would be nice to use a tool number out of the Centroid range (>200), like perhaps adding 1000 to the dummy tool numbers. This would make them easy to spot/search for in the .nc file. This is currently not possible as the 200 max tool number is hard coded in the post. Would it be difficult to have the >200 tool number check selectable as optional?

Any Ideas?
------------
Mark
mrichards
Posts: 34
Joined: Thu Feb 28, 2019 12:05 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 3)

Post by mrichards »

Coolant:
The post creates the following code:

Code: Select all

(Drill2)
(begin job)
N110 T148 M6
N115 S4500 M3
N120 G54
N125 M7
N135 G0 X0. Y-0.651
N140 G43 Z0.6 H148
N150 Z0.2
N155 G98 G73 X0. Y-0.651 Z-0.4 R0.2 Q0.126 F18.
.....
The coolant command (M7) is created before the rapid, causing the machine to spray coolant all the way from the tool change position back to the work. Is it possible to alter this so the coolant starts after the rapid? Possibly before or after the z move to clearance height?

In an enclosed machine, this would not be a issue, but on an open machine (Bridgeport) it makes a mess.

I often edit Intercon created files to move the M7 command on jobs that are going to be run multiple times.

Thanks.
------------
Mark
Muzzer
Posts: 446
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 38D269594F9C-0110180512
Location: UK
Contact:

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 3)

Post by Muzzer »

Presumably you'd need to edit the post processor to change the order. Can you handle Javascript?
mrichards
Posts: 34
Joined: Thu Feb 28, 2019 12:05 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 3)

Post by mrichards »

Muzzer wrote: Wed Dec 30, 2020 4:34 pm Presumably you'd need to edit the post processor to change the order. Can you handle Javascript?
Barely, but I'll give it a shot!
------------
Mark
swissi
Posts: 433
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 3)

Post by swissi »

I created a new Beta version that has the following changes based on the comments above:
  • 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 of the coolant command (M7/M8) has been moved and will now be inserted after the Z axis has dropped.
If you would like to test the new features, download the beta version below. I tested the M7/M8 change with a couple of parts but haven't done extensive testing yet if it works in all situations. Post here if you find something that doesn't work as expected.


Remove the .txt extension at the end of the file:
****File removed. New Beta version below******


-swissi
Last edited by swissi on Mon Jan 18, 2021 5:49 pm, edited 2 times in total.
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
swissi
Posts: 433
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 3)

Post by swissi »

I had to modify the position at which the M7/M8 command is being inserted and made a few other fixes and enhancements.

Here's a new Beta version that has the following changes compared to the official Version 4:
  • 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 of the coolant command (M7/M8) has been optimized and is now placed after the point when the Z axis has dropped to 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
  • From other posts I have seen that users ran into issues with Fusion 360 posts because they were using Program Numbers that are reserved for CNC12 (9100 - 9999). This beta version will now create a post error with a log message that these program numbers can't be used
If you would like to test the new features, download the beta version below. If you are going to download and test this new version, please provide positive and negative feedback here.

Remove the .txt extension at the end of the file:
***File removed. New Beta3 below***


-swissi
Last edited by swissi on Fri Jan 22, 2021 2:56 pm, edited 1 time in total.
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
swissi
Posts: 433
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 3)

Post by swissi »

I have made one more change in this new Version 5-Beta3 Post Processor.
  • In addition to the changes listed above, I have moved the M9 Coolant Off command also to the point when the Z-Axis has retracted to the clearance height rather than keeping the coolant on until the Z-Axis has retracted all the way up to the Tool Change position.
Here's the download link for the new v5-Beta3. Please provide feedback here in this thread.

Remove the .txt extension at the end of the file:
***File removed. Version 5 is now officially released. Check first post for download link***


-swissi
Last edited by swissi on Tue Jan 26, 2021 12:41 pm, edited 1 time in total.
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Muzzer
Posts: 446
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 38D269594F9C-0110180512
Location: UK
Contact:

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)

Post by Muzzer »

A bit more digging and experimentation and I've found that using the swissi v005 post outputs a curious "E10" line at line 14. When I post with v003, that line contains G54. That seems a fairly significant difference. No idea what an E10 would mean on a good day!
Ahah.JPG
Using the V003 code, my job air seems to air cut correctly. I may even cut some metal with it later...

### refer to the "907 error" post for background viewtopic.php?f=60&t=5289 ###
cbb1962
Posts: 345
Joined: Wed Jan 03, 2018 10:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 38D2695C8301-0122180576
Location: NW Arkansas

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)

Post by cbb1962 »

This is not what I am seeing. In Fusion when I have a setup's Work Offset = 1, I get a G54 every time. When I change the Work Offset = 10, THEN I get an E10. What is your Work Offset? V3 had a problem setting everything to G54 even when I wasn't supposed to. viewtopic.php?p=43875#p43875
Clint in NW Arkansas

The more I learn, the more I realize I don't know...
swissi
Posts: 433
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 4)

Post by swissi »

Muzzer wrote: Sat Jan 23, 2021 2:50 pm No idea what an E10 would mean on a good day!
The Pro versions of CNC12 support 6 different WCS numbers named WCS#1=G54 to #WCS#6=G59. They can also be addressed as E1 to E6 but G54 to G59 is more common.

The Digitizing and Ultimate versions of CNC12 support 18 different WCS# from E1 to E18.

As Clint mentioned, you most likely have WCS#10 selected in your operation in Fusion 360. Please report back if this is not the case.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Post Reply