3+1 Machining Using LinuxCNC

[Anonymous]

I'm using Fusion360 with my LinuxCNC controlled milling machine and recently have installed a 4th axis for it.  I know Fusion360 does not support continuous 4th axis at this point.  I am unable to get it to generate any code for indexing using the EMC or LinuxCNC post processor.  I understand how to use Tool Orientation for getting the 4th Axis ("a" axis in this case) however when I post to LinuxCNC PP (EMC) it gives me the Tool Orientation not Supported Error.  Do I need to change a setting in Fusion360 for it to know to post 3+1 to "a" axis?  Is this something that is not supported at all with Fusion360 and LinuxCNC?

Thank you!

Dale

See full error message below:

Information: Configuration: Generic LinuxCNC (EMC2)
Information: Vendor: LinuxCNC.org
Information: Posting intermediate data to 'C:\Users\TJ\AppData\Local\Fusion 360 CAM\nc\4th Axis\1001.ngc'
Information: Total number of warnings: 1
Error: Failed to post process. See below for details.
...
Code page changed to '1252  (ANSI - Latin I)'
Start time: Monday, February 8, 2016 7:10:08 AM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 40504
Configuration path: C:\Users\T J\AppData\Local\Autodesk\webdeploy\production\66ed5e8cf991ec00ace7e4d2638113959b38c0dd\Applications\CAM360\Data\Posts\linuxcnc.cps
Include paths: C:\Users\TJ\AppData\Local\Autodesk\webdeploy\production\66ed5e8cf991ec00ace7e4d2638113959b38c0dd\Applications\CAM360\Data\Posts
Configuration modification date: Thursday, January 21, 2016 11:15:25 PM
Output path: C:\User\TJ\AppData\Local\Fusion 360 CAM\nc\4th Axis\1001.ngc
Checksum of intermediate NC data: d82376548774dc946598ae5a3ab83e57
Checksum of configuration: 5d363ef0107384e55700f05d103b7096
Vendor url: http://www.linuxcnc.org
Legal: Copyright (C) 2012-2015 by Autodesk, Inc.
Post processor signature could not be verified (error 0xfffffffc).
Generated by: Fusion 360 CAM 2.0.1909
...
Warning: Work offset has not been specified. Using G54 as WCS.
Error: Tool orientation is not supported.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to invoke function 'onSection'.
Error: Failed to invoke 'onSection' in the post configuration.
Error: Failed to execute configuration.
Stop time: Monday, February 8, 2016 7:10:08 AM
Post processing failed.

[stopaginn]

I'm having a similar problem. Post process fails "!Error: Failed to post data. See log for details." file (don't know where that is). You mention the configuration file modification, but I haven't a clue where to find that file. I'm milling on a Sherline (LinuxCNC) and currently have the "a" axis on the right. I have setup my stock for mill turning, changing the Z in each setup stock. At first I wanted to just manually rotate the part and repeat the cuts. However, I am cutting from box stock (4 sides) a three sided part (120º rotate each time). This became a problem with the corner of the stock being thicker from the 120º turn. If I do standard mill stock cut it posts. The minute I change the tool orientation it errors (above). So I switched to mill turning, all setups fail.

Thanks, Jim

[daniel_lyall]

@stopaginn can you post the file you are trying to use, you have to have the trident in the correct orientation, and settings in the post processor.

If you look here it's all explained  

http://forums.autodesk.com/t5/hsm-post-processor-forum/how-to-set-up-a-4-5-axis-machine-configuratio...

[stopaginn]

Thank you for the link! I'm still lost, where is the configuration file that you edit? Path on Mac OS X that is. Or, is it the post process file? If so, my file goes to about 10 lines and fails. I've tried to open it in another editor than Brackets, it's the same thing.

Thanks, Jim

[daniel_lyall]

I use windows.

It's the post that you edit you bring the post processor dialog up and make sure the post you are useing is up then click on open config that brings you the post to be edited.

1 is where the file is 

2 is the post you are going to use

3 is what you click to edit the post

[stopaginn]

That explains it. There is no access to the config file from the F360 gui in OS X that I can find (see screenshot). maybe I could search for it? Do you know the extension of the config file? Do you no the location of the log file its referencing in the error is, or maybe its extension?

So sorry on this, its killing me not being able to get past this error.

[daniel_lyall]

http://forums.autodesk.com/t5/computer-aided-machining-cam/i-have-lost-all-post-prossesors/td-p/5991...

http://forums.autodesk.com/t5/computer-aided-machining-cam/how-do-you-edit-post-processor-configurat...

These 2 posts should help, doing a search in support and learning useing Apple post as the search term there are a lot of posts with the answers. I don't use apple and never will unless I am given one

[stopaginn]

Daniel, Thanks a bunch for your time, you've been really helpful!! 

[ryan.olliges]

I've edited my post processor for linuxcnc to use the b-axis

I've gotten the machine to turn properly using wrap toolpath pocket functions, but when I go to bore with a circular pattern I'm getting issues. The first bore aligned with the origin works great, but when it goes to cut the second bore in the pattern (36 deg rotation) the b-axis rotates to the correct orientation, but the x-axis also moves to the location as if it were trying to accomplish the same thing the rotation is doing. I've included some of the g code. Where might I have gone wrong editing my post processor?

Thanks,

(BOREROTATETEST)
(T1 D=0.125 CR=0. - FLAT END MILL)
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z0.
(BORE3)
N25 M9
N30 T1 M6
N35 S27000 M3
N40 G54
N45 B0.
N50 G0 G43 X-0.0043 Y3.45 Z7.6 H1
N55 G0 Z7.0175
N60 G1 Z6.95 F32.4
N65 G18 G3 X-0.0167 Z6.9375 I-0.0125 K0.
N70 G1 X-0.023
N75 G17 G3 X-0.0355 Y3.4375 I0. J-0.0125
N80 X0.0355 Z6.9178 I0.0355 J0.
N85 X-0.0355 Z6.8981 I-0.0355 J0.
N90 X0.0355 Z6.8784 I0.0355 J0.
N95 X0.028 Y3.4593 Z6.8743 I-0.0355 J0.
N100 X-0.028 Y3.4157 I-0.028 J-0.0218
N105 X0.028 Y3.4593 I0.028 J0.0218
N110 X0.0105 Y3.4615 I-0.0099 J-0.0077
N115 G1 X0.0055 Y3.4577
N120 X0.0033 Y3.4559 Z6.8746
N125 X0.0013 Y3.4543 Z6.8755
N130 X-0.0006 Y3.4529 Z6.877
N135 X-0.0022 Y3.4516 Z6.879
N140 X-0.0033 Y3.4507 Z6.8814
N145 X-0.0041 Y3.4502 Z6.884
N150 X-0.0043 Y3.45 Z6.8868
N155 G0 Z7.2
N160 Y2.075
N165 Z7.0175
N170 G1 Z6.95 F32.4
N175 G18 G3 X-0.0167 Z6.9375 I-0.0125 K0.
N180 G1 X-0.023
N185 G17 G3 X-0.0355 Y2.0625 I0. J-0.0125
N190 X0.0355 Z6.9178 I0.0355 J0.
N195 X-0.0355 Z6.8981 I-0.0355 J0.
N200 X0.0355 Z6.8784 I0.0355 J0.
N205 X0.028 Y2.0843 Z6.8743 I-0.0355 J0.
N210 X-0.028 Y2.0407 I-0.028 J-0.0218
N215 X0.028 Y2.0843 I0.028 J0.0218
N220 X0.0105 Y2.0865 I-0.0099 J-0.0077
N225 G1 X0.0055 Y2.0827
N230 X0.0033 Y2.0809 Z6.8746
N235 X0.0013 Y2.0793 Z6.8755
N240 X-0.0006 Y2.0779 Z6.877
N245 X-0.0022 Y2.0766 Z6.879
N250 X-0.0033 Y2.0757 Z6.8814
N255 X-0.0041 Y2.0752 Z6.884
N260 X-0.0043 Y2.075 Z6.8868
N265 G0 Z7.6
N270 G53 Z0.
(BORE3)
N275 B36.
N280 G0 G43 X-4.4706 Y3.45 Z6.146 H1
N285 G0 X-4.1282 Z5.6748
N290 G1 X-4.0885 Z5.6202 F32.4
N295 G18 G3 X-4.0913 Z5.6027 I-0.0101 K-0.0073
N300 G1 X-4.0964 Z5.599
N305 X-4.0986 Y3.4497 Z5.5974
N310 X-4.1008 Y3.4488 Z5.5958
N315 X-4.1027 Y3.4473 Z5.5945
N320 X-4.1043 Y3.4453 Z5.5933

[daniel_lyall]

It would be easier to post a file what has this problem and the post possessor, the problem you are seeing could be a lot of things.

[ryan.olliges]

Thanks, I've attached the file and the processor that I'm using. 

[daniel_lyall]

Is this happening on the machine 

@GeorgeRoberts @jeff.pek  Can one of you guys Please have a look at this the X axis looks to be taking a short cut, with the attached Linux post and the default one, useing the mach3 post it is fine.

From the Linux post.

From the Mach3 post.

[GeorgeRoberts]

Thanks for tagging me @daniel_lyall. I've just taken a look at the post and can see there are a few issues:

• The rotary axis is set to the head of the machine... I assume this is a rotary table? If so, the axis specification should look like this:

    var bAxis = createAxis({coordinate:1, table:true, axis:[0, 1, 0], range:[-360, 360], preference:1});

• You have TCP enabled in getWorkPlaneMachineABC, that should be false:

    var tcp = false;
    if (tcp) {
      setRotation(W); // TCP mode
    } else {
      var O = machineConfiguration.getOrientation(abc);
      var R = machineConfiguration.getRemainingOrientation(abc, W);
      setRotation(R);
    }

  I tested the post and the output looks correct after these changes:

Hope this helps!

[ryan.olliges]

Thanks for looking into this @GeorgeRoberts. The TCP function did the trick. Now to run the machine.