Hi again! I got my machine up and running and I am thoroughly impressed with how it turned out so far, it’s doing great. I just want to get a few things figured out before I get on here again to show pictures and stuff.
The biggest issue I am having right now is with the jobs I export from Fusion 360. After running the print in Repetier, if the first cut is not located near the origin, the Z axis will plunge down about a millimeter into the stock and trek over to the lead in point where then it will lift up and plunge again starting the actual cut.
I don’t know what causes this, it doesn’t show up in the gcode or on the visualization of the tool path in Repetier. It’s suppose to be doing a rapid travel move over to the starting point where the lead in should be. I set the origin in the lower left corner and set the height by putting the tip of the bit to the top of the stock.
I’m using V10 of the post processor for Fusion. The board is from the shop with the firmware already flashed onto it, I haven’t touched it at all.
I’ve already done some pen tests using Illustrator and a script that turns the vector paths into gcode, and there was no issues with that at all, the pen paths were always on point. So I feel like this is a Fusion issue.
Again according to Fusion’s CAM, it should be lifting the z axis by 10mm and moving from the origin to the first cut path.
Any ideas what’s causing this? If needed, I can support any specifics or pictures. Thanks!
To give you an idea, here’s a picture of what it did my last cut. I’m cutting this logo out of plywood and as you can see it makes a diagonal line about a millimeter in depth into to wood and then starts cutting near the center of the logo. That bigger outline around it is where it did it even worse. At first I was trying to do a larger scale cut, but it went down deep in depth from the origin, went upwards, then took a right until it reached the lead in point.
previously set to 0,0,0
G1 Z18 F300 ----this moves up by 18mm Are you positive you set 10mm?
G1 X508.576 Y307.817 F2500
G1 Z5 F300
G1 Z-2.365 F180
G1 Y307.813 Z-2.436
There is nothing in this code to make it do that diagonal cut, unless it did not move up the initial 18mm.
When you start this gcode, you start at the origin and at the surface, what are its next few moves?
I just tested it again and figured I’d try to see if any of the starting gcode lines are getting mistranslated.
I found the issue is the M117 command, which is supposed to be an LCD message. I dont have an LCD on my board, so after deleting that line, it did what it’s supposed to, lifting up all the way to the clearance and moving over to the lead in point.
M117 could be sending a “Get Zero Position” command, I’m not sure if that has anything to do with it.
Is there a way I can stop the post processor from making these messages? I didn’t really plan on using an LCD any time soon.
Are you selecting the correct stock origin point in Fusion? Its almost like it sees the bed as Z0 and “raises” 18mm before it travels (which if it is 3/4" stock) would make a 1.05mm deep cut. 3/4"=19.05mm I would think the G92 would take care of that and everything would be high in the air if the stock origin were wrong, but maybe its a double negative kind of thing?
I had some weird stuff happen with the V10 post-processor on travel moves. It did not seem to go to the full clearance height before moving and struck a hold down screw as it crossed.
I had been using MPCNC_Mill_Laser.cps but marlin had a weird reaction to a G3 move that cut a chunk of my work out of one corner with the arc. I think somebody made some improvements to MPCNC_Mill_Laser.cps, but heck if I can find that post right now.
Ignore my previous post. You are actually using the MPNC_Mill_Laser.cps post-processor, not the MPCNC_Fusion360_V10_SDcard.cps.
To get rid of the M117 commands, just comment them out on lines 83 and 157 in the cps file. I would use something like Notepad++ and not just notepad or word to keep the formatting.
Comment them out by adding // in front of those lines.
Ok awesome, I just did that and tested out a new version of the gcode, so now there is no M400 or M117 commands and everything looks like it’s going to run smoothly now.
My guess is something with those commands is getting mixed up when it starts the first travel move, because when it would make that diagonal cut it would move extremely slow, like way under the feedrate speed.
Thanks for all your help though! I’m glad it was an easy fix in the script and not something in firmware. Hopefully this helps anyone else with a similar issue with the MPCNC Fusion 360 combo.
I am having the exact same problem, the M117 line is causing the issue (although I do have an LCD).
Was wandering if there is a way to prevent Fusion from generating the M117 line in the first place?
