These are 16"x 40" pieces (cut on my full sheet Lowrider). 1hr+ long cuts. I’ve added a fan to my controller case thinking it might be a stepper driver overheating. Still having the issue.
It cuts absolutely perfectly until sometime near the end of the cut and then just goes a bit haywire. It’s definitely not in the gcode.
Any thoughts gang?
Have you attempted the same cuts twice and had them go off in the same way or differently?
Looks like a neat project. Would you mind pasting the gcode anyway? Maybe we’ll see something.
It looks like it is mostly shallow cuts for a while, and at the end, it cuts out the middle pieces?
Overheating drivers usually just stop for a few minutes. So I don’t think it is overheating. Skipping steps is more likely. What controller and drives do you have?
Another possibility is loose pulleys, or on a LR, it could be shifting on the Y.
Once it starts getting away from it’s normal path, and it is very deep, it will be biting a lot with the whole bit. After that, all bets are off.
I’ve actually tried it 3 times with three different failures. What you’re seeing in the image is two of the same cut (different orientation) and two different failures.
Thanks Jeff. I’m just grasping at straws at this point. I’m running the Rambo 1.4. Considering moving to an MKS so that I can swap our drivers (and add a touch screen for easier control).
Skipping steps sounds right, but it’s weird that it’s always happening at the tail of the piece. Feels like it’s probably a controller issue to me as well. This is my first CNC, but I’ve spent a lot of time upgrading/troubleshooting/rebuilding the 3D printers that In have. Very familiar with marlin (although I haven’t touched the firmware on this build yet).
Gcode to follow.
The rambo is (IMO) the best board for the job. I wouldn’t want to replace it with something else. The fact that the drivers are integrated is a big advantage.
I said I thought it was skipping steps, but I don’t agree it is something wrong with the board. I just wanted to make sure the current setting was appropriate for the motors. If it’s a rambo from Ryan, it is set correctly, and it shouldn’t skip steps (unless something else is wrong).
If you are very familiar with Marlin, you could check the current setting on the board, to make sure it is the same as Ryan sets it. https://github.com/Allted/Marlin/blob/V1CNC_Rambo_Dual/Marlin/Configuration_adv.h#L909
Looking at the gcode (this is from kiri:moto?), I see some huge feedrates on moves like this: G0 Z15.0 F6000. That is asking for a 100mm/s move in the Z. That is asking for trouble. It doesn’t look like the big circle has a cutout, so I could see that kind of move causing problems.
I just tried kiri:moto a few days ago, and I found the Z travel speed to be something I’d like to fix. But in the meantime, make sure your Marlin Z feedrate is set low. Something like 8mm/s in a standard configuration. Lower if you have a 1 start leadscrew. I would be worried even about a 100mm/s travel move in XY on my machine.
Interesting. What do you have your feedrate set at? And does the slicer you’re using have a “rapid Feedrate” as well?
Those numbers came from your file. The estlcam basics doc shows the standard settings. It has separate rapid speeds for Z (F480) and XY (F2100).
F2100? Yeesh, I’m a chicken. I run my XY rapids at F900. Do most of you guys run at F2100 for XY rapids?
Z rapids at F500, plunge at F300 for me.
2100 is 30mm/s. It should only be used when your bit is in the clear (you aren’t milling). That should be fine in XY for pretty much every V1 machine. But if you have any trouble, slower is fine too. IIRC, the new firmware is limited to 30mm/s XY and 10mm/s Z. I suspect many expert users will want to push it faster.
Well yes, if only possible.
I’m still trying, My settings are F(xy) 2000mm and F(z) 600mm.
Did some good smaller pieces with Z+3mm in 20mm plywood today,
planning on reducing Z+ to 2,2mm for some larger pieces, as I’m not too
confident that I might loosing steps.
I did run 6,50mm Z+ by accident at those speeds but the bit and piece did survive,
forgot to activate trochoidal milling in Estlcam.
I was running speeds far over 20000mm/min with 20 teeth pulleys, in idle, just a pen,
without loosing any steps (8000mm/min Estlcam and 300% in Repetier host)
Although not able to cut 2,5mm @ 1200mm through plywood, hence I went back to 16 teeth pulleys.
I’m thinking to go up with the voltage to 19V from an old Laptop PS, must just do an additional wiring for the cooling fans to 12V.
With F900, my bit is just close to go up in smoke.
A lot depends on the milling bits too, well it’s a (steep) learning curve, but a lot of fun too.
