Hey all,
I recently completed my build of the MPCNC, I have been doing some test cuts to makes sure everything is working as it should. I was able to cut out simple text, but moving to a more complex design I ran into an issue. Randomly, the tool head will plunge very deep into the material I am cutting forcing me to immediately stop the job. I am using estlcam as my CAD software and repetier host as my controller. Any help would be greatly appreciated.
Is it plunging or just not moving up as far as it should?
We have recently found the software issue. Year and a half later…Turns out estlcam and Marlin firmware do not communicate very well. Estlcam uses the standard G0 gcode to do rapid moves and relies on the firmware to control that speed. Marlin does not use G0 in that way and relies on the gcode to set all speeds. So what happens is estlcam tells the machine to move the z axis way too fast (usually in the up/retract command), marlin should only move at max speeds that I have set. It does not always obey this speed limit. Marlin will either ignore it if it happens to much or try to move the stepper and it can not physically move that fast so it skips the steps.
We have revamped the fusion 360 post processor, and things seem to be working flawlessly now. I’m sorry for the software switch. It is a bit more involved but there are many more resources out there to learn it. We have just ironed out all the bugs so over the next week or so I hope to revamp all the tutorials to include the Fusion 360 workflow. The upside is there is much more control, and it is more free than estlcam.
Just to add to that. Estlcam does work and has worked very well for me the whole time but I cut slow and my rapid moves were never set very high. Most of the issues show when you try to push things too fast.
So if you have a project you are trying to get done and don’t have time to learn fusion right now, just set the “f” command to repeat on every line and use a slow speed in the box like 510mm/m (8.5mm/s) this is just under the firmware max for the z axis. You can go higher but this should give perfect results temporarily with the down side of very slow movements between cuts.
Thanks for the quick reply! I will add a little more detail I should have added in the beginning. The tool end either plunges too far in while beginning a new cut or after retracting from a cut, starts preforming the next cut above the material. It always comes out of a cut fine and never drags the tools head on the material. I don’t have a specific project I am working on at the moment so a switch to Fusion 360 is defiantly an option.
Just a quick question why not use estlcam as controller? I have been using it for some time time now I have had it randomly cut deep, but for me at least it was because my wires were not shielded and it would loose or change home on z axes. I had the router power cable running right next to the stepper wire. once i got shielded wire and ran the power cable the other way i have not had the problem since. text on etslcam is lacking and it is not wysiwyg. great program but text is very broken.
I’m having the same issue with text. I’m going to try routing my Dewalt power cable the other direction and see how it goes. I think I was having the same problem with text with the pen mount but I assumed it was ink saturated paper.
What did you use for shielding on your Z axis?
I had that issue at first and it was the Z axis binding causing skipped steps. After I greased the Z screw it stopped.
I oiled my Z axis when I put the machine together. It moves up and down very well. I haven’t heard the motor grind or miss steps on the Z axis. I haven’t tried running with the Dewalt power cable running the other way yet.
https://www.v1engineering.com/software-updates/
Have you updated your Estlcam or your fusion post processor?
I thought mine was moving good too and did not hear anything that sounded like it sticking but it worked after I put a bunch of grease on the screw.
Part of my problem is my threaded rod has stripped out my pineapple coupler. My tool would lower to the work piece but wouldn’t come all the way back up. This was causing my Z axis to change. I don’t know when it started or if I was having the same problem with the pen.
I’m fixing this now and will update after I’ve made some cuts.
Shapes are coming out well with everything the same depth. I’ll try letters generated by estlcam next.
Sorry to resurrect a 4 year old post. But I’m having this issue today in 2020. I am using the latest version of Estlcam 11.224h. My machine was working flawless for weeks until now, and nothing has changed as far as I’m aware except the Estlcam version.
To troubleshoot, I took the t-screw completely out and greased it and I still randomly get this plunging problem.
Do I need to upgrade my firmware? I still have the original Marlin firmware from back in 2016. Maybe it’s a power issue with missing steps?
Settings below:
Not sure where to start to be honest.
Is the Z travel speed set, and do the G0 Z commands have a speed set on them?
I have the Z travel set in the tool settings in Estlcam.
And it looks like the gcode has a G0 Z command has a feed rate on it at the beginning.
;Project Colts-blackcut
;Created by Estlcam version 11 build 11.224
;Machining time about 00:10:22 hours
G90
M03 S24000
G00 X0.0000 Y0.0000 Z0.0000 F2100
G00 Z5.0000 F480
Each time this has happened it has occurred at either the beginning or end of the print. But it also happens randomly. Sometimes the cut will come out perfect. Other times it will drill deep into the workpiece into the spoil board and break the bit or cause a fire hazard.
That first move is F2100, or 35mm/s. If that has a Z move involved, that is too fast. F480 is 8mm/s, which is usually fine, unless you’ve got extra resistance in Z.
Do you have any F2100 moves at the end of the gcode?
Yes, there is a drill move at the end of the GCODE: G00 X90.0000 Y0.0000 Z5.0000 F2100. Any idea why Estlcam wouldn’t inherit my tool settings for the Z-move when generating this GCODE?
Colts1mm-blackcut.gcode (10.4 KB)
It looks like that speed is for Z positive and is inheriting that number for the rapid feed settings in ESTLCAM. So it’s going 35mm/s upwards, but more slowly (F480) when it goes down. 
Weird. Is it hard coded in the start/end gcode?
