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

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

cbb1962
Posts: 349
Joined: Wed Jan 03, 2018 10:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D2695C8301-0122180576
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: NW Arkansas

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by cbb1962 »

Swissi,

G54-G59 plus extended WCS supported in the Fusion PP?

In Fusion, I am using Work Offsets=2/#4/+2 For anything above G59 I get E7 and E8.

Thanks,
Clint in NW Arkansas

The more I learn, the more I realize I don't know...
cbb1962
Posts: 349
Joined: Wed Jan 03, 2018 10:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D2695C8301-0122180576
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: NW Arkansas

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by cbb1962 »

I just did some more reading and E7 and E8 are the correct designations, I assumed they were an error code.
Clint in NW Arkansas

The more I learn, the more I realize I don't know...
swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by swissi »

cbb1962 wrote: Mon Dec 30, 2019 4:01 pm I just did some more reading and E7 and E8 are the correct designations, I assumed they were an error code.
Clint,
glad to see this got resolved.
Clarin wrote: Wed Oct 16, 2019 4:50 pm Hello,
Would it be possible to add cutting (Laser, Plasma, Jet) it would be greatly appreciated.
Thanks
Clarin,
I apologize for not answering your question back from October. I did not see your post until now.

My post processor is for milling only and I have no plans at this point to support other machine types. My next version of the post processor will have support for the CNC12 Smoothing Profiles and most likely some improvements for the rotary axis.

Stay tuned.

-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
cbb1962
Posts: 349
Joined: Wed Jan 03, 2018 10:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D2695C8301-0122180576
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: NW Arkansas

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by cbb1962 »

swissi wrote: Mon Dec 30, 2019 5:05 pm My next version of the post processor will have support for the CNC12 Smoothing Profiles and most likely some improvements for the rotary axis.
Can you elaborate on the support for smoothing profiles?
Clint in NW Arkansas

The more I learn, the more I realize I don't know...
swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by swissi »

Clint,

CNC12 supports G-code Smoothing called AD2. AD2 is an algorithm that pre-processes G code and smooths out the geometry before handing off the moves to the Acorn.The details about AD2 can be found in the Centroid Acorn CNC12 G-code Smoothing (AD2) User's Manual

The new added Smoothing Fusion360 Post Processor Property will allow you to select/change the Smoothing Profile directly in Fusion360 depending on the job you are working on:

Fusion360 Smoothing Property
Fusion360 Smoothing Property
Capture11.JPG (34.93 KiB) Viewed 5037 times

The default value (-1) will not change any smoothing configuration and will just use the current CNC12 settings. Selecting 0 will turn off all smoothing and any number between 1 - 99 will activate the corresponding Smoothing Profile configured in CNC12.

-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
cbb1962
Posts: 349
Joined: Wed Jan 03, 2018 10:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D2695C8301-0122180576
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: NW Arkansas

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by cbb1962 »

Swissi,

A quote from Post Processors, a guide to Centroid CNC12 G&M codes
There are two features that can be helpful on ATC machines, even though neither is required:

A user-selectable M code (usually M17) can be inserted at the end of the last cut before a tool change, after the tool is clear of the stock but before a G28 or M25 move to Z home. If the control is so configured, this M code will turn off the spindle and coolant and begin the spindle orientation process. That saves time in the tool change because the orient can take place while the head moves up to the ATC level.
On machines with a random-access tool changer (generally ones with a double-ended transfer arm) an M107 code with the next (upcoming) T number can be inserted immediately after the completion of each tool change. That will allow the ATC carousel to pre-stage the next tool while the current tool is cutting.
CNC Services Northwest Home

Copyright © 2016 Marc Leonard
Last updated 16-Nov-2016 MBL
Would you consider adding the option to add M17 and M107 as described above to your Fusion PP?
Clint in NW Arkansas

The more I learn, the more I realize I don't know...
swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by swissi »

cbb1962,

not 100% sure I understand all this correctly and how your M17 command file looks like but from what I read in Marc's comments, there should be a M17 before the G28 and a M107 right after the M6.

I added this to the attached Fusion360 post processor Beta version. Check it out and let me know if it does what you need.

Both M17 and M107 are now property settings that are disabled by default so you need to enable them before you run the post process. Also the M107 depends on the property "Preload Tool". The property Preload Tool also needs to be enabled too, otherwise the M107 command will not be added. The next tool needed in the job file will be right before the M107 command.

Let me know how this works and if anything needs to be changed.

And as always: Use at your own risk. No warranties given :o

-swissi


Remove the extension .txt from this file:
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
slodat
Posts: 793
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by slodat »

swissi - trying to sort out how to use your post processor on my new mill conversion. How/where do I drop the file(s)? Which files in the GitHub page do I download? I know this is a novice question, but I'm not seeing it anywhere.
slodat
Posts: 793
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by slodat »

Got your post processor working with Fusion. Issue I'm having is it's not putting an M5 at the end of any program to stop the spindle. It's doing the M9 to turn off the coolant. Looking through the post, not sure why it's not stopping the spindle. It's not stopping the spindle prior to the M6 either.

sample output:

Code: Select all

%
O01005
N10 #301 = "Post Processor Benchmark - Milling_MM"   ; Fusion 360 Design File Name
N15 #302 = "1005"    ; Program Name
(T1  D=1.9685 ZMIN=-0.0394 - face mill)
(T2  D=0.315 ZMIN=-0.4331 - flat end mill)
N20 #351 = "T1  D=1.9685 ZMIN=-0.0394 - face mill"
N25 #352 = "T2  D=0.315 ZMIN=-0.4331 - flat end mill"
N30 #353 = ""
N35 #354 = ""
N40 #355 = ""
N45 #356 = ""
N50 #357 = ""
N55 #358 = ""
N60 #359 = ""
N65 #360 = ""
N70 G90 G94 G17
N75 G20
(2D-Face)
N80 #304 = "Setup for Metric tools"   ; Setup Name/Description
N85 #306 = "2D-Face"   ; Tool Path Name/Description
N90 #300 = "T1  D=1.9685 CR=0. - ZMIN=-0.0394 - face mill"
N95 #308 = "face mill"   ; Tool Type
N100 #309 = "millimeters"   ; Tool Units
N105 #310 = "1.968503937007874"   ; Tool Diameter
N110 #311 = "3"   ; Tool Number of Flutes
N115 #312 = "flood"   ; Tool Coolant
N120 #315 = "5000"   ; Spindle Speed
N125 #316 = "CW"   ; Spindle Direction
N130 #319 = "39.37007874015748"   ; Feed Rate
N135 #320 = "0.00262"   ; Feed per Tooth
N140 #321 = "19.68503937007874"   ; Ramp Feed Rate
N145 #322 = "19.68503937007874"   ; Plunge Feed Rate
N150 #323 = "0.00394"   ; Feed per Revolution
N155 #324 = "Stock Coord = Dir+(X1.9685 Y0.9843 Z0.) Dir-(X-1.9685 Y-0.9843 Z-2.0079)"   ; Origin Position
N160 #325 = "0.5905511811023622"   ; Z Clearance Height
N165 #326 = "G54"   ; Current WCS
N170 G28 G91 Z0.
N175 G90
N180 T1 M6
N185 T2
N190 S5000 M3
N195 G4 P5.
N200 G54
N205 M8
N215 G0 X3.1496 Y-0.9596
N220 G43 Z0.5906 H1
N225 Z0.1969
N230 G1 Z-0.0394 F39.37
N235 X-3.1496
N240 G2 Y0.0374 I0. J0.4985
N245 G1 X3.1496
N250 G0 Z0.5906
(2D-Contour)
N260 #306 = "2D-Contour"   ; Tool Path Name/Description
N265 #300 = "T2  D=0.315 CR=0. - ZMIN=-0.4331 - flat end mill"
N270 #308 = "flat end mill"   ; Tool Type
N275 #309 = "millimeters"   ; Tool Units
N280 #310 = "0.31496062992125984"   ; Tool Diameter
N285 #311 = "3"   ; Tool Number of Flutes
N290 #312 = "flood"   ; Tool Coolant
N295 #315 = "5000"   ; Spindle Speed
N300 #316 = "CW"   ; Spindle Direction
N305 #319 = "39.37009842519685"   ; Feed Rate
N310 #320 = "0.00262"   ; Feed per Tooth
N315 #321 = "31.496043307086616"   ; Ramp Feed Rate
N320 #322 = "19.68503937007874"   ; Plunge Feed Rate
N325 #323 = "0.00394"   ; Feed per Revolution
N330 #324 = "Stock Coord = Dir+(X1.9685 Y0.9843 Z0.) Dir-(X-1.9685 Y-0.9843 Z-2.0079)"   ; Origin Position
N335 #325 = "0.5905511811023622"   ; Z Clearance Height
N340 #326 = "G54"   ; Current WCS
N345 G28 G91 Z0.
N350 G90
N355 M9
N360 M1
N365 T2 M6
N370 T1
N375 S5000 M3
N380 G4 P5.
N385 G54
N390 M8
N400 G0 X-0.3829 Y1.185
N405 G43 Z0.5906 H2
N410 Z0.1969
N415 G1 Z0.0394 F19.685
N420 Z-0.4331
N425 Y1.1811 F39.37
N430 G3 X-0.2254 Y1.0236 I0.1575 J0.
N435 G1 X1.5354
N440 G2 X2.0079 Y0.5512 I0. J-0.4724
N445 G1 Y-0.8661
N450 G2 X1.8504 Y-1.0236 I-0.1575 J0.
N455 G1 X-1.6535
N460 G2 X-2.0079 Y-0.6693 I0. J0.3543
N465 G1 Y0.8661
N470 G2 X-1.8504 Y1.0236 I0.1575 J0.
N475 G1 X-0.2254
N480 G3 X-0.0679 Y1.1811 I0. J0.1575
N485 G1 Y1.185
N490 G0 Z0.5906
N500 M9
N505 G28 G91 Z0.
N510 G28 X0. Y0.
N515 M30
(Resetting all used CNC12 User-String-Variables)
N520 #300 = ""
N525 #301 = ""
N530 #302 = ""
N535 #303 = ""
N540 #304 = ""
N545 #305 = ""
N550 #306 = ""
N555 #307 = ""
N560 #308 = ""
N565 #309 = ""
N570 #310 = ""
N575 #311 = ""
N580 #312 = ""
N585 #313 = ""
N590 #314 = ""
N595 #315 = ""
N600 #316 = ""
N605 #317 = ""
N610 #318 = ""
N615 #319 = ""
N620 #320 = ""
N625 #321 = ""
N630 #322 = ""
N635 #323 = ""
N640 #324 = ""
N645 #325 = ""
N650 #326 = ""
%
slodat
Posts: 793
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by slodat »

Think I figured out how to make it work, but I'm not sure if there's not other implications.. Looks like the onImpliedCommand(COMMAND_STOP_SPINDLE) ; should actually be onCommand(COMMAND_STOP_SPINDLE);

It's now puking out the M5 command. This is in the stock Centroid post, too. Hmm.. Interested in what you all may think. I'm thinking if it works, I move on.
Post Reply