Buildbotics Forum

Just getting my machine up and fully running. I made a pretty simple carving sign. When I save all of the toolpaths individually from Aspire v9.514, they all load fine, render fine, and cut fine. But when I save them all into one file, I get errors about arcs are off by 4.xx mm, and the file renders as a squiggly line, and that's it. It doesn't print most of the way through, though. But then throws an error I can't seem to recover from - I had to reboot the controller. I then loaded the individual file where it gave me the error, and it continued on OK and I finished up the last files one-at-a-time.

In the file is the all-toolpaths file, and each individual path. They are saved in this order:
Huskies Outline
Text
Huskies
Inner Circle (it errors when starting this one in the all-toolpaths file)
Outer Profile
Huskies Outline (Clear)
Cutout

I also attached a screenshot showing what the rendering looks like (just a single squiggly line), and the errors it gives.

Thank you, and I hope it's something simple that I'm (not?) doing.

Please post tbe version of software you are running and the gcode programs in question. I will take a look at them to see if I can tell what is going on.

Doug

Thanks for reply. I’m running 0.4.15. All of the G-code is in the MTU.zip file attached above.

Had another issue last night, also. I was running one of the programs and then stopped using the stop button when when my piece moved. At that point, I was unable to jog it because it kept saying a job was already running. Hitting stop didn’t do anything. The list of programs shown on the controller was incorrect and I had to reset the controller. After that, the list of programs returned to the correct list and I was able to jog again.

Attached are pictures of the program list before and after cycling the power. There’s also one where showing that it couldn’t load the selected program from the list.

Thank you.

Hmmm,

This loads and simulates correctly on my controller.

Please go to the 'General' page and click 'Bug Report'. This will create a file that includes the system logs, the controller configuration, and the current program that is loaded. Then, attach the bug report to your posting. When I get it, I'll load your configuration on my controller to see what happens.

Are you able to recreate the problem where you stopped the program but it said it was still running?

I tried to upload the file, but it's too big to attach (~10mb), so I broke it into 2 parts.

I have not played with it any more to see if I can recreate the issue with the it stopping, but saying it's still running. That's a task for this weekend. I will follow up when I have more time to play with it.

Thank you for your assistance!

OK,

I loaded your configuration and then reloaded 'Michigan Tech Round Up (all toolpaths).ngc and now I get the errors with a squiggly line displayed. I'll dig further and let you know what I learn.

The problem is that your tool change procedure on the 'Settings' page changes the units to 'Metric' using a G21 command. Your program runs in 'Imperial' units using the G20 commands but the tool change procedure changes it mid-stream.

Since you want your configuration for tool changes to work with either metric or imperial units, you should push the machine state at the beginning of your tool change procedure and then pop the state at the end of the procedure.

You can do this by inserting n 'M70' at the beginning of the tool change procedure on the 'Settings' page and inserting an 'M72' at the end.

You can see this in my posting on the subject of probing at viewtopic.php?f=6&t=117 .

Thanks AGAIN for the quick reply! I will correct that and keep it mind. I’ll let you know if I can reproduce the other issues (unable to jog after a stop, and program list incorrectly populated with old/deleted programs).

Thank you!