postprocessing following 10/1/2020 update

[xbeerd]

just ran into this issue where i exported a gcode file from F360 following todays update and it would not run on my cnc router.  yesterdays file i tried and it still worked.   

opened both files and compared them and there is a long commented out line of text regarding feeds/travel/etc in the new file versus the old.  removed that and my problem was solved. 

blackbox controller, using openbuilds Control Software.  

[seth.madore]

That's interesting. What was the alarm generated? Was it a comment in general that caused your machine to alarm out, or was it the length?

[xbeerd]

thats the thing,  there was no alarm.  i loaded the gcode file into the software and hit "Run" and it just sat there,  didnt start up the spindle or move or anything,  i opened up the file in a text editor, removed the text, saved the file and it ran the file like normal.   

below was the text i removed, maybe its the length of it?  

(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.)

[xbeerd]

oh, i just stumbled onto this bit on a shapeoko wiki site....

GRBL is limited in the number of characters per line it can handle, which causes it to ignore the end portions of too-long lines. If your job is previewing correctly, but not running properly, check to see that line lengths are w/in its limits (50 for older versions, 70 for 0.8c dev or later) as discussed in the forums.

https://wiki.shapeoko.com/index.php/Operation_Troubleshooting#Toolpath_Differs_from_Expected

granted a line thats commented out. i wouldnt expect that to make an error, but maybe?  i'll try it and see. 

[seth.madore]

Well, it's not seeing the ending ")'" so it's hanging up on that. I will open a ticket to investigate: CAM-24898

Seems to me that the comment needs to be truncated or split into several lines that are sub-70 characters long..

[mykldevlin]

Exactly the same symptoms and solution running grbl on an arduino nano using candle as the sender.

The program just stops, waiting for the command to finish.

Naturally enough, does it on each change of operation.
runs after the comment is deleted (but was annoying to find one further down! 😐)

thanks for looking into it.

[jerry.king]

I found the exact same problem.

editing out the line in the gcode file allows the file to run.

[xbeerd]

it does seem to be a character limit issue.   i deleted the comment back to the word 'which' before it finally would run the program. 

[wmbYBW5Q]

This is a big problem.  I am a developer/maintainer for two different components in the DIY CNC ecosystem - CNCjs and Grbl_Esp32.  We are seeing a rash of bug reports aimed at our software that are caused by this too-long line.  In many cases it is not practical to deploy a fix, for two different reasons.  The first reason is that most GRBL controllers run on memory-limited AVR processors, so it is just not feasible to increase buffer sizes.  The second reason is that updating all of the different GCode senders and controllers is just not practically possible.  The number of system setups is practically endless, and the majority of users do not have the skill to perform an update while maintaining the careful machine configuration that is necessary.  The recent change to Fusion 360 licensing has already caused a lot of consternation among Fusion users; this latest item now also has the developer community up in arms.  I suggest that Autodesk should put a very high priority on fixing this and delivering an update, lest it lose a great deal of goodwill.

[seth.madore]

This is also of utmost priority to Autodesk. It was certainly an unintended consequence that this message would cause GRBL controllers to spazz out. We are currently working through this bug and hope to have a hotfix sooner rather than later.

[wmbYBW5Q]

Thanks very much.  I will inform my team and users of the good news.

[seth.madore]

We pushed out an update today that addresses this issue in addition to a couple others that were plaguing the Personal Entitlement community. Terribly sorry for the significant inconvenience that these particular issues caused.

Issues fixed:

1) G1 F0. feedrates on drilling toolpaths.

2) Too long "rapid reduced" comment

3) Correct feedrates not being posted for plasma/laser

[jerry.king]

Thank you! 
Looking forward to trying it out in a couple days.