topic Re: 4-axis Eding CNC post processor in HSM Post Processor Forum

4-axis Eding CNC post processor

mauritswoudenberg — Wed, 07 Feb 2024 09:47:45 GMT

Hi all,

I have a 5ft x 10ft CNC router with XYZ linear axes and a tilting spindle rotating along the Y axis, so let's call it B.

The machine is controlled by an Eding CNC760 controller. The standard Eding CNC post processor works fine when it comes to 3 axis machining, but I can't get it to work with the 4th axis. I have the manufacturing extension so I have access to multi-axis toolpath generation.

What I did:

- took a generic 3-axis machine from the library for testing.

- created a 3D parralel toolpath and kept it on 3-axis in the multi-axis tab

- with standard Eding CNC post processor from fusion library selected it worked and generated usable gcode

- then I added a new machine from the fusion library. I used the 'Autodesk generic 4-axis (B Head)' machine. I abandoned this strategy because I couldn't even get it to work on 3 axis.

- instead I added a rotary axis to the generic 3 axis machine. In 3 axis mode the post processor worked and I got usable gcode.

- Now I changed to 5-axis (there is only 3 or 5 axis, even though my machine has 4), made sure the toolpath was correct and only used XYZ and B, but it gives an error when posting: Error: Failed to invoke function 'onOpen'.

Does anyone have an idea what is going wrong here?

See below for the full log.

Information: Configuration: Eding CNC/USBCNC
Information: Vendor: Eding CNC
Information: Posting intermediate data to '/Users/mauritswoudenberg/Desktop/1001.cnc'
Information: Total number of warnings: 1
Error: Failed to post process. See below for details.
...
Start time: Wed Feb 7 09:46:31 2024
Warning:
Post processor engine: 4.6050.0
Configuration path: /Users/mauritswoudenberg/Autodesk/Fusion 360 CAM/Posts/eding 3.cps
Include paths: /Users/mauritswoudenberg/Autodesk/Fusion 360 CAM/Posts
Configuration modification date: Wed Feb 7 09:12:57 2024
Output path: /Users/mauritswoudenberg/Desktop/1001.cnc
Checksum of intermediate NC data: 45ee9065f7da8211c1243c3adee25dec
Checksum of configuration: 7171545363d83b79460033e471cf4b4c
Vendor url: http://www.edingcnc.com
Legal: Copyright (C) 2012-2023 by Autodesk, Inc.
Generated by: Fusion CAM 2.0.18434
...
Error: Failed to invoke function 'onOpen'.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to invoke 'onOpen' in the post configuration.
Error: Failed to execute configuration.
Stop time: Wed Feb 7 09:46:31 2024
Post processing failed.

Re: 4-axis Eding CNC post processor

KrupalVala — Wed, 07 Feb 2024 09:55:44 GMT

Hi @mauritswoudenberg ,

Please ensure that the toolpath orientation (Rotary Direction) is correct. It would be great if you could share the project details along with the post-processor information.

Thanks,

Re: 4-axis Eding CNC post processor

mauritswoudenberg — Wed, 07 Feb 2024 20:11:25 GMT

Hi @KrupalVala ,

Thanks for your reply.

This is how I edited the generic 3 axis machine.

I also attached the post processor I used.

This is a test project I setup: https://a360.co/3SwDQG3

Many thanks!

Re: 4-axis Eding CNC post processor

KrupalVala — Thu, 08 Feb 2024 06:50:46 GMT

Hi @mauritswoudenberg ,

It seems that the issue is related to the lead-in and lead-out in the parallel toolpath, potentially causing errors in generating a pure 4th axis toolpath. Consequently, you're encountering errors in both the post-processor and the toolpath machine simulation. Would you mind trying the Rotary Parallel option with the generic 4th Axis machine simulation? For more controll you can choose between the Spiral, Line, or Circular rotary toolpath style.

Additionally, I would recommend defining the Work Coordinate System (WCS) at the center of the job/component. This will save you time when making selections around or along the rotary axis

Thanks,

Re: 4-axis Eding CNC post processor

mauritswoudenberg — Thu, 08 Feb 2024 15:04:01 GMT

nice! Taking out lead ins and lead outs didn't fix it, but changing the strategy to rotary parallel, with circular style, and then turning of TCP worked. Well at least it exported something that my machine could read. When I run it on my machine (in a safe place far above the table) I notice that the B axis moves as expected, but the X and Z axes don't compensate for the distance between B-tilting point and tooltip. The simulation does do that though.

I feel that I'm almost there. Could you help me out getting it done completely?

Many thanks again!

Re: 4-axis Eding CNC post processor

Charliegeorgelos — Thu, 08 Feb 2024 18:00:05 GMT

I am experiencing these very same issues on my Laguna IQ CNC machine with the 4th axis attachment. I have been all over trying to find a solution, but have only found others facing similar issues. I am hoping this thread can help me finally find that solution I've been looking for!

@KrupalVala

your help is greatly appreciated!

Charlie

Re: 4-axis Eding CNC post processor

KrupalVala — Fri, 09 Feb 2024 05:23:28 GMT

HI @mauritswoudenberg ,

Could you please verify if your machine supports TCP functionality? If not, please uncheck the TCP checkbox. If TCP is supported, please ensure that the calibration parameters, including offsets and distances, are accurately configured to with the B-axis.

Thanks,

Re: 4-axis Eding CNC post processor

mauritswoudenberg — Fri, 09 Feb 2024 13:00:55 GMT

I turned off TCP. With TCP turned on it gives an error.

Shouldn't it also be possible to generate working gcode without TCP if I tell Fusion the distance between tooltip and tilting point? If not that would mean writing some complicated inverse kinematics functions in post processor. Something I'm not too familiar with. Would be a nice challenge, though preferably I fix this in Fusion.

Re: 4-axis Eding CNC post processor

mauritswoudenberg — Fri, 09 Feb 2024 14:38:24 GMT

update:
in the post processor there was a boolean to control TCP. I set it to TRUE and then it did generate gcode. It still doesn't compensate ZX plane for B-asix movement, but I think we're on the right track. It probably still means that I'll have to set up the kinematics and do the programming.

Any help is aprecieated!!

Re: 4-axis Eding CNC post processor

KrupalVala — Mon, 12 Feb 2024 05:04:17 GMT

HI @mauritswoudenberg

You can use a Machine Definition in the CAM system to define the rotary axis kinematics of the machine or it can be hardcoded in the post processor. The hardcoded machine configuration can be found in the defineMachine function.

For a deeper understanding, I recommend referring to the Post Processor Training Guide, specifically Chapter 8.1.3.

Note that you can only EITHER use a machine configuration in Fusion OR define the machine within your postprocessor. When a postprocessor with a hardcoded machine configuration is used together with a machine configuration in Fusion a warning/error will be generated, and the hardcoded configuration will take precedence.

Thanks,