Brand new to these things and really like the product, so I figured i’d try it out in the local makerspace. I am trying to mill down a piece of cylindrical stock to final dimensions, but for some reason fusion 360 (what i am using) errors out when exporting the g code. Right now I am working on a test piece to get familiar with the machine, but I have a project i’d like to do this on. The error file is as follows:
Information: Configuration: Pocket NC
Information: Vendor: Pocket NC
Information: Posting intermediate data to ‘C:\Users\Benni\OneDrive\Documents\Fusion 360\G Code\test.ngc’
Error: Failed to post process. See below for details.
…
Code page changed to ‘1252 (ANSI - Latin I)’
Start time: Thursday, November 3, 2022 1:16:33 AM
Code page changed to ‘20127 (US-ASCII)’
Post processor engine: 4.5911.0
Configuration path: C:/Users/Benni/AppData/Roaming/Autodesk/Fusion 360 CAM/Posts/pocket nc.cps
Security level: 1000
Include paths: C:/Users/Benni/AppData/Roaming/Autodesk/Fusion 360 CAM/Posts
Configuration modification date: Thursday, November 3, 2022 12:39:49 AM
Output path: C:\Users\Benni\OneDrive\Documents\Fusion 360\G Code\test.ngc
Checksum of intermediate NC data: 0bbcdf86bdea86655e13824a35222dc5
Checksum of configuration: 2b46106147a8c7c74dad71e4bf66c394
Vendor url: http://www.pocketnc.com/
Legal: Copyright (C) 2012-2022 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.14569
…
###############################################################################
Error: Error: Tool orientation is not supported for available machine axes.
Machine angles not supported: A-153 B9.63e+03
Error in operation: ‘Rotary2’
Error at line: 1
Stack dump:
(“Tool orientation is not supported for available machine axes.\nMachine angles not supported: A-153 B9.63e+03\nError in operation: ‘Rotary2’”)@:0
activateMachine()@C:/Users/Benni/AppData/Roaming/Autodesk/Fusion 360 CAM/Posts/pocket nc.cps:483
onOpen()@C:/Users/Benni/AppData/Roaming/Autodesk/Fusion 360 CAM/Posts/pocket nc.cps:573
Failed while processing onOpen().
###############################################################################
Error: Failed to invoke function ‘onOpen’.
Error: Failed to invoke ‘onOpen’ in the post configuration.
Error: Failed to execute configuration.
Stop time: Thursday, November 3, 2022 1:16:33 AM
Post processing failed.
No idea why it’s messing with the A axis, I just need it to act like a rotary table. Any help with the issue would be fantastic. Thanks!
Based on that error message, it appears your program is trying to rotate the A axis farther negative than the machine is able to accomplish. This is usually due to WCS orientation or tool orientation not being set correctly.
If you are confident in those orientation settings then it is possible that the operation is simply not possible within the machine’s movement constraints. So make sure what your operation is doing is actually possible by visualizing how the machine would have to move to accomplish the operation.
If you haven’t already, it may be helpful to work through our First Part Tutorial. It walks you through all the fundamental steps of programming for the machine as well as machine set up and other important basics.
Honestly I have no idea why the WCS are being so troublesome. I tried to attach my .f3d file but it looks like new users cannot upload files (which is fair, although annoying). I have resorted to scalloping N-S-E-W sides of the cylinder, and facing the top down to proper length. Originally I had a rotary operation, but it didn’t work for the same reasons. I am unfortunately running out of time, so I think I am going to run the machine as a manual mill and see how much I can get done. Attached is a screenshot of all my toolpaths, cause apparently I can do that haha.
You should have an email from me in your inbox. Feel free to send over your Fusion file there, I should be able to look at it early next week (have to leave the office for the rest of the afternoon and tomorrow).
Hi, I will join because of similar issue I have - it may be related, looks like the post processing failed in my case and I got this error on the machine during operation:
Worth to mention during this program it did unwind from almost negative limit to almost positive limit once successfully.
(sorry if hijacking and please move it as new thread)
regards,
Piotr
odd, it does look similar though. For me it just never compiled, if it had moved the A axis while cutting was going on the part would have been scrap either way so I guess I am glad for that. Hopefully both issues can be solved
@piotr I am not sure there is enough information in the bit of code you posted to determine what exactly is causing your issue. However, typically, that error message is accurate and the solution is to reduce the number rotations the B axis has to make to achieve the desired geometry. When using the Rotary toolpath in Fusion you can either increase the step over of each pass or break the single operation into several operations.
@piotr, if you’re willing to share your G code publicly, you can attach the whole program to a post on this forum, which allows anyone to quickly and easily view it in the simulator. This makes it a lot easier for us and others to help diagnose issues like this.
I have to make lots of round parts, and this was my first attempt to use rotary toolpath on whole part - testing surface finishes with different approaches - when generated .ngc file I got warnings that there will be 3 retractions to rewind - which I will create new topic to ask how to do it properly.
Issue here is that retraction and rewinding B axis failed with error - meaning postprocessor had attempted to make it as you can see in gcode and it failed with the second rewind operation. -I am trying to pretend to understand what failed it could be gcode interpreter that failed.
@john sorry I just realised I posted totally random code(!) so the N75075 repeats few times in the file (wow!). So error is about file line 75075:
let me interpret the code:
line 75071 - B table is at -9999 (so at the limit)
line 75075 - because of calibration or whatever machine has to do this line -it is attempting to go more negative for B axis.
line 75077 - B table is winding back to positive limit to prepare for next rotary toolpath.
@qrothing after the above analysis: for me in this case the postprocessor should start rewinding 360degrees before the limit to avoid this kind issue.
Let me know your thoughts.
Regards,
Piotr
@piotr When Kinetic Control reports an error, it’s reporting the actual line number of the program, not the line with the matching N number. I encourage people to turn those N numbers off, as they are completely meaningless and make it harder to detect changes to a program using standard text comparison tools.
My guess here is that there is a floating point round off error triggering the error. It’s reporting the error on line 75075, which is the first move after disabling TCPC. During the calculation resulting from disabling TCPC, the B value is likely just slight less than -9999 (so slight that it’s much smaller than any real world value the machine is capable of moving to). I checked the default INI configuration and while we specify the [JOINT_4]MIN_LIMIT as -10000 to avoid this rounding issue, we are still specifying -9999 as the [AXIS_B]MIN_LIMIT (there are subtle differences between what these values represent, but they really should match in this case).
So, a work around for now would be to edit your INI Overlay in Config tab > Server tab > Machine Config pane > INI Overlay tab. Add a section AXIS_B and add MIN_LIMIT with a value of -10000 (you can also add a MAX_LIMIT of 10000 to avoid this issue when reaching the max limit). This should make it so the machine will allow you to move to B-10000, but the post still treats the max as -9999, so you shouldn’t have an issue when it commands the machine right up to the max. Alternatively, you could edit the G code wherever it commands B-9999 and change it to something like B-9998.99999.
In the next Kinetic Control release, I’ll change the defaults to appropriate values to avoid this rounding issue.
