Turning Post for LinuxCNC?

[russtuff]

With the new update to CAM for turning in Fusion 360 I assume there are more posts on the way. I use LinuxCNC for a Grizzly G0602 I converted to CNC myself. I've been trying to use the Generic Fanuc post but so far haven't gotten any good code to try. Any idea if/when a LinuxCNC post will be released?

Thanks.

[Anonymous]

The "I" value that I'm getting in the G76 is too large, and the simulation is showing passes at the proper depth.  The CAD/CAM is showing the thread peak at 5.884, which is where the profile finishing pass leaves off, but the code I'm getting has a thread peak of 6.816 so I'm cutting mostly air with the threading tool. 

%
(1012)
(M6X1TEST)
G7
G18
G90
G21

(FACE1)
T2 M6 G43
G54
G96 D2000 S150 M3
G95
G90 G0 X16.7 Z5.
G0 Z-0.5
G1 X12.7 F0.18
X-0.8
X2.028 Z0.914 F1.
G0 X16.7
Z5.

(PROFILE1)
G96 D2000 S150 M3
G95
G0 X16.7 Z5.
Z1.49
X10.7
G1 Z-0.51 F0.18
Z-8.4
X12.68
X15.508 Z-6.986 F1.
G0 Z1.49
X8.7
G1 Z-0.51 F0.18
Z-8.4
X10.7
X13.528 Z-6.986 F1.
G0 Z1.49
X6.7
G1 Z-0.51 F0.18
Z-8.4
X8.7
X11.528 Z-6.986 F1.
G0 Z1.49
X5.247
G1 X4.7 F1.
Z-0.51 F0.18
Z-0.799
X5.933 Z-1.416
G3 X6.284 Z-1.84 I-0.424 K-0.424
G1 Z-5.96
G3 X6.102 Z-6.278 I-0.6
G1 X4.867 Z-7.265
G2 X5.154 Z-7.301 I0.166 K0.364
G3 X6.284 Z-7.9 I-0.035 K-0.599
G1 Z-8.4
X6.7
X9.528 Z-6.986 F1.
G0 Z2.197
X3.535
G1 Z0.197 F0.18
G2 X4.121 Z-0.51 I1.
G1 X5.7 Z-1.299
X8.528 Z0.115 F1.
G0 Z2.468
X1.801
G1 Z0.468 F0.18
G2 X3.374 Z-0.509 I1.
G3 X3.77 Z-0.617 I-0.085 K-0.391 F0.08
G1 X5.65 Z-1.557
G3 X5.884 Z-1.84 I-0.283 K-0.283
G1 Z-5.96
G3 X5.762 Z-6.172 I-0.4
G1 X4.332 Z-7.316
G2 X5.13 Z-7.501 I0.434 K0.415
G3 X5.884 Z-7.9 I-0.023 K-0.399
G1 Z-8.4
X8.712 Z-6.986 F1.
X9.52
G0 X16.7
Z5.

(THREAD1)
T4 M6 G43
G54
G97 S500 M3
G95
G0 X12.7 Z5.
G0 Z8.902
G76 P1 Z-6.56 I-6.816 J0.173 K0.866 R1.3 Q30 H1
G0 X12.7 Z5.

M5
M30
%

[Anonymous]

I guess I wasn't understanding that I value.  I thought it was a diameter value.  It looks like that G76 code is correct.  It must be an issue with how linuxcnc expects the tool X touchoff.

[vilts]

Nice that you got the G30 sorted. I've been busy with other projects, so haven't had yet time to get back to this.

The I value in G76 is a bit weird one indeed. Took me a while to understand it.

I is a thead peak offset from the drive line. But as the drive line can be whereever you say it is, I value changes accordingly.

Actual code to calculate the I value looks like this:

  var peakOffset = (getParameter("operation:outerClearance_value") * 2) - ((x * 2)+ (threadDepth * 2));
  peakOffset = (getParameter("operation:turningMode") === "outer") ? -peakOffset : peakOffset;

 

So it's taking the "outerClearance" and calculating from that.

I'm soon going to do 2 or 3 start internal threads, then I'll see if the code works for that case as well. At least 2-start external threads were ok.

[Anonymous]

My post is failing.  "Unsupported drilling orientation."  I tried the tormach post and it worked.

Information: Configuration: LinuxCNC lathe postprocessor
Information: Vendor: Viljo Marrandi
Information: Posting intermediate data to 'D:\1016.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: Sunday, April 16, 2017 5:10:59 PM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 41304
Configuration path: C:\Users\Robert\AppData\Local\Autodesk\webdeploy\production\110e62f27b395d1e77f65827ad98f9392983e959\Applications\CAM360\Data\Posts\linuxcnc_lathe.cps
Include paths: C:\Users\Robert\AppData\Local\Autodesk\webdeploy\production\110e62f27b395d1e77f65827ad98f9392983e959\Applications\CAM360\Data\Posts
Configuration modification date: Monday, March 27, 2017 11:05:46 PM
Output path: D:\1016.ngc
Checksum of intermediate NC data: 8e87a802c9759cf1b7213b5d4e5bd814
Checksum of configuration: 02c394c499d502b6d5ce9c9c3d46c663
Vendor url: http://www.autodesk.com
Legal: Copyright (C) 2012-2017 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.2938
...
Warning: Work offset has not been specified. Using G54 as WCS.
Error: Unsupported drilling orientation.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to execute configuration.
Stop time: Sunday, April 16, 2017 5:10:59 PM
Post processing failed.

[Laurens-3DTechDraw]

@Anonymous what are you trying to do?

[Anonymous]

I didn't use my lathe for a few months, and now for some reason I'm getting an M4 where I should have an M3 and it doesn't put in the D4000 into the G96 Line. I had to re-download the post, but I don't know what else could have changed.  When I drill I get an M3, but all the other turning tools I get M4.  I haven't changed those tools in the library at all, and the simulation shows everything in the proper orientation.