September 8, 2019 at 12:27 pm #112583
Since 2 weeks i’ve got me a working Lowrider and i’m very happy with it. It runs stand alone using Marlin with GCode from an SD card. For Cad/Cam i’ve so far used Fusion 360. However on this project i’m running into issues.
First run Z kept comming down, turned out to be the bit sliding out of the collet, so that was my fault mounting it. However the second try on this project something weird happened when the gcode execution moved from curring an Adaptive 3D profile to a first parallel finishing pass. Instead of starting the wanted vertical arcs it started cutting lateral circles (destroying the workpiece in the process :-p).
also the motion of the machine was not smooth like normal but jerky. I tried to switch it off using the button on the controller, but it did not have any effect. Any clues on where to start digging?
Gcode: see attachment.
So the toolpath itself does not seem to be the problem. I’m trying to mill a bit faster every pass now to search for the limit’s but that does not seem to explain this problem.
Attachments:September 8, 2019 at 1:25 pm #112600
To be complete, i did a fastforward (250% that was fun) to the failure point in a dry run and recorded the behaviour.
You can see it making circular patterns instead of the parallel passes it should make, and clearly you hear the engines missing steps and moving irratically.September 8, 2019 at 5:21 pm #112622
I saw cursed project and I was hoping for Halloween decorations.September 8, 2019 at 5:22 pm #112623
Make sure you are completely in the positive workspace. Negative commands are funky with the current dual firmware.September 9, 2019 at 12:15 am #112656
I’m not at my computer to look at the gcode myself but I do know that marlin supports G2/G3 in the XY plane only, unless you enable extra options in the configuration. In principle these extra options enable switching modes to do arcs in the XZ or YZ planes but I’ve never used it. I suspect these are common in CNC land but rare for Marlin.
If fusion generates an XZ or YZ arc and Marlin can’t handle it, maybe it would create XY arcs instead.
Look in your gcode for arc plane switches G17 G18 or G19. Maybe you just need to enable CNC_WORKSPACE_PLANES.
And its also true that exceeding machine limits is bad.
1 user thanked author for this post.September 9, 2019 at 12:39 am #112658
I think @jamie is right. I checked the GCode at the problem location and it is running arcs in g2 with I and K, as far as i can see K is not supported by Marlin and is supported bij GRBL. No clue why it did not use arcs in the candle holder. ( Milling was done in positive workspace, exept for Z btw which is practically impossible).
So if this is the problem, how can i prevent it from using G0-G2 K arcs (in z plane)?September 9, 2019 at 6:03 am #112703
Wow, learn something new everyday.
The post processor might allow you to turn off arcs.September 9, 2019 at 8:34 am #112741
@Ryan, but how? I’m just using the Fusion360 Post operation and select GRBL as post processor (since Marlin is a fork of GRBL) as far as i know, right?
What option do you guys use in Fusion 360?September 9, 2019 at 9:36 am #112752
No, we are not GRBL, we have a post processor for Marlin. It is linked in the milling basics page at the bottom.
I do not know if it has the option or not, I use Estlcam.September 9, 2019 at 10:59 pm #112923
@Ryan: thanks, changing the post processor to @guffy‘s Marlin implementation lifted the curse :-). All and all it is a miracle that so many other projects came out just fine with the GRBL post.
Also i like the spindle reminder and status updates it gives on the lcd now. Makes the LR with Marlin even more complete!
Thanks all for helping out.
Attachments:September 10, 2019 at 7:43 pm #113215
Cool, glad we figured it out.
You must be logged in to reply to this topic.