Autodesk Fusion 360 and LinuxCNC

Let me start by saying that I am a novice CNC lather. I have done lots of manual lathe work, and am currently running LinuxCNC on my mill. Until now, I have just been using LinuxCNC to drive a modified Emco Compact 5. I am using Fusion 360 CAM to generate Gcode the same way I have done with my mill. I select the emc.cps file for post configuration. When I try and generate the code, I get an error saying:

Vendor url: www.autodesk.com
Legal: Copyright (C) 2012-2015 by Autodesk, Inc.
Error: Turning toolpath is not supported by the post configuration.
Error: Failed to invoke 'onOpen' in the post configuration.
Error:
Error: Failed to execute configuration.
Stop time: Monday, October 12, 2015 1:53:58 AM
Post processing failed.

If I select "Turning" in the drop down next to the cps selection, no emc cps files appear. What am I doing wrong? Is there another cps file specifically for lathe work?

Can I use another turning cps file that already ships with fusion and trust that that would work? I don't read Gcode, so I don't really know what I'm looking at but don't want to cause a crash.

Any help here would be appreciated.

You are trying to use a milling post processor to produce lathe code, bound not to work.

Ten seconds googling found this
camforum.autodesk.com/index.php?topic=7514.0

The autodesk forum would seem the logical place to start.

I don't read Gcode, so I don't really know what I'm looking at but don't want to cause a crash.

I would suggest that you make the effort, or you will be completely at the mercy of software and stuck in a tortuous CAD, CAM, post cycle to do the simplest of tasks.

Never mind not being able to tell when the code produced is dangerous gibberish.

regards

I have a post that pretty much works for my lathe. I'm not at the shop at the moment, but I'll post it once I get back.

I am using the post off the autodesk forums that is supposed to be beta, however it has quite a few issues.

So far I have found that threading does not work correctly, tool calls are incorrect and lastly you have to have M6 coded to call G43 for all tools. Otherwise you have to manually call your tool offsets after tool changes. I'm sure there are more issues, however this is all I have found after trying to run one program.

Alloy Craft wrote: So far I have found that threading does not work correctly, tool calls are incorrect and lastly you have to have M6 coded to call G43 for all tools.

If the tool-changes are a T-only version then this matches how Tormach has things arranged and it is possible to configure LinuxCNC the same way. For a lathe this is probably more convenient, the only reason to separate tool-select and tool-change (TN then M6) is because mills can pre-fetch tools, whereas lathes typically can't. In this setup G43 is assumed, though you can have separate tool and wear offsets.

Have a look at the lathe-fanucy sim config for an example of how this works. (sim/axis/lathe-fanucy)

From the README

"An example of combining the G43.2 compound offset idea with remapping to create
a toolchange similar to Fanuc.

T1 = select and load tool 1, and apply the base offset for tool 1
T0101 = select and load tool 1 and apply offsets 1 and 10001
T0201 = select and load tool 1 and apply offsets 1 and 10002

This might not exactly match Fanuc, but the behaviour is easy to change
by editing toolchange.ngc"

I have modified the latest Tormach post from their web site to work on my lathe with metric.
Im using a Gangtool setup with the parting tool upside down at the back.
All the front tools at the front are set to turret 1
and the parting tool are on turret 0
using_Gangtooling in the properties window is set to true.

Added an option to use more than 1 springpass when threading
Added an option to use a goto function with the parting tool if TurningPart operation is used.
Changed some variables to forceDecimal:false because it added a decimal to integers without a zero.
Removed the G30 call and added G0 Z instead.
Have only tested the threading, profiling, parting, facing and drilling operations yet so be careful if you get it to work!
Have written down all my changes in the .cps file at the top after Tormachs comments. Just open it in a text editor!