Linux CNC Sherline Fusion 360

[dogsbody658X2]

Hello,

I've got Sherline mill and lathe. I use EMC post processor with a mill without any problems. Unfortunately I can't run lathe post processor. It shows multiple errors. I chose Linux CNC turning from Fusion 360 library.

Here's the log for a simple face operation.

Error: Failed to post process. See below for details.

...

Start time: Sun May 1 19:14:46 2022

Post processor engine: 4.5851.0

Configuration path: /Users/..../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps

Include paths: /Users/....../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts

Configuration modification date: Fri Apr 1 00:00:51 2022

Output path: /Users/....../Fusion 360 CAM/nc/1001.ngc

Checksum of intermediate NC data: d2beb883270a10b27d24df4e967ee79f

Checksum of configuration: d6425971936a52dd892edb82fb884d77

Vendor url: http://www.linuxcnc.org

Legal: Copyright (C) 2012-2022 by Autodesk, Inc.

Generated by: Fusion 360 CAM 2.0.12888

...

Warning: Work offset has not been specified. Using G54

###############################################################################

Error: ReferenceError: forceCoolant is not defined

Error at line: 1180

Error in operation: 'A 1 Face1'

Stack dump:

getCoolantCodes@/Users/....../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps:1179

setCoolant@/Users/...../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps:1157

onSection@/Users/....../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps:781

Failed while processing onSection() for record 404.

###############################################################################

Error: Failed to invoke function 'onSection'.

Error: Failed to invoke 'onSection' in the post configuration.

###############################################################################

Error: ReferenceError: forceCoolant is not defined

Error at line: 1180

Stack dump:

getCoolantCodes@/Users/..../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps:1179

setCoolant@/Users/...../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps:1157

onCommand@/Users/...../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps:1310

onClose@/Users/....../Library/Application Support/Autodesk/Autodesk Fusion 360/CAM/cache/posts/linuxcnc turning.cps:1526

Failed while processing onSection() for record 404.

###############################################################################

Error: Failed to invoke function 'onClose'.

Error: Failed to invoke 'onClose' in the post configuration.

Error: Failed to execute configuration.

Stop time: Sun May 1 19:14:46 2022

Post processing failed.

_________________

As I got it I have these errors:

1 Warning: Work offset has not been specified. Using G54 - I didn't set any offset for a mill EMC post processor...

2 Error: ReferenceError: forceCoolant is not defined - I put coolant disabled in a tool library and checked disabled in a operation window

3 Error: Failed to invoke function 'onSection'. 

Error: Failed to invoke 'onSection' in the post configuration.

- what are these?

[dogsbody658X2]

I successfully got a file with a Tormach post processor but it doesn't go with Sherline linux cnc. The simulation in Fusion 360 goes smoothly either.

Here it is

; program: 1001

;

;When using Fusion 360 for Personal Use, the feedrate of

;rapid moves is reduced to match the feedrate of cutting

;moves, which can increase machining time. Unrestricted rapid

;moves are available with a Fusion 360 Subscription.

; CAM: Fusion 360 CAM 2.0.12888

; Document: Chassis 0.3.6 0.52 v1

; Post Processor: Turning post for Tormach 8L with a PathPilot control.

; Post version: 43777

; Post modified: 2022-04-26 12:40:16

; Date: 05012022 12:33:17

;

;== BE SURE TO PROPERLY SET THE G30 HOME POSITION FOR TOOL CHANGES ==

;== MOVE THE Z-AXIS TO A POSITION THAT CLEARS ALL TOOLS AND PRESS THE SET G30 BUTTON ==

;

; -- tool: 1 Quick Change Front Tool Post cycle time: 00:01:11

; op: A 1 Face1

;

; Total cycle time: 00:01:11

;

G7

G18

G21

G54

G40

G90

G30

; ==============================================================

; Tool: 1

; Tooling: Quick Change Front Tool Post

; Op: A 1 Face1

; Time: 00:01:11

; Z: -1.

N10 M0 (CHANGE TO T1 ON FRONT TOOL POST)

T0101

G54

G97 S1078 M3

G95

G90 G0 X18.

Z0.

G96 D3500 S61 M3

G1 Z1.214 F0.0508

X10.828

X8. Z-0.2

X-0.406 F0.0127

X2.422 Z1.214 F0.0508

X18.

Z0.914

X10.828

X8. Z-0.5

X-0.406 F0.0127

X2.422 Z0.914 F0.0508

X18.

Z0.614

X10.828

X8. Z-0.8

X-0.406 F0.0127

X2.422 Z0.614 F0.0508

X18.

Z0.414

X10.828

X8. Z-1.

X-0.406 F0.0127

X2.422 Z0.414 F0.0508

X18.

X10.828

X8. Z-1.

X-0.406 F0.0127

X2.422 Z0.414 F0.0508

X18.

Z0.

G97 S1078 M3

M5

G30

M30

%

[boopathi.sivakumar · Accepted solution]

Hi @dogsbody658X2 

It seems like forcecoolant variable is undefined in the post processor which is causing the issue. I have logged a ticket which will be resolved soon. I'll let you once its done.

meanwhile if you want make changes edit the post and find for this lines

var currentCoolantMode = COOLANT_OFF;
var coolantOff = undefined;

and add var forceCoolant = false; as shown below

var currentCoolantMode = COOLANT_OFF;
var coolantOff = undefined;
var forceCoolant = false;

Save the post and test it.

[dogsbody658X2]

Thank you, that really helped.
In order to run an .ngc file on Linux CNC you need to delete all G95 code otherwise your lathe will stuck at G1 line