Trying to cut green foam from lowes, and I keep melting it. I am pretty sure I need to cut faster. (using a 2 flute bit from the router section at Lowes - not ideal, but still.)
I am having a hard time getting the machine to move above 30mm/s from a g-code file. Running at 40 or 100 produces what appears to be the same speed, in a very jerky motion. Here’s a video - you can’t as easily see how jerky it is, but you can definitely hear it chug-chug-chugging. That’s about as fast as I can get it to move, whether the F(xy) is set to 40mm/s or 100mm/s in Estlecam.
Reading through the forums, people have reported cutting foam much faster.
I know I’m blowing the forums up - but definitely learning a lot and making progress! Can someone help me get up to a better foam cutting speed?
Interesting. I don’t know exactly what the problem is, but I have a few guesses :).
Have you changed the max feedrates or accelerations in Marlin? Just looking and the max in the firmware is set to 120mm/s (really? That’s fast). And the accel is set to 400mm/s/s in xy. So it should be able to get up to 40mm/s in about 0.1s.
What shape are you trying to cut in that video? Is it just a straight line? The Marlin planner will be reading a few lines of gcode and looking ahead so it doesn’t overshoot. If there are a lot of little gcode commands (because it’s very detailed, or made of curves without arc commands) then Marlin will have just a few mms of distance in the buffer. When that happens, it will be careful not to go too fast so it can definitely stop before it reaches the end. I may not be explaining this the best way, but if it’s looking at the next 5 commands, and it has no idea what happens on the 6th, it needs to avoid going 40mm/s, because the 6th command could be to turn around. So it needs to be prepared to stop by the end of the 5th command. The remedy is to use arc commands, increase the acceleration in the firmware.
I should also mention that at those speeds, with 12V power supply, I think the torque available will be less than the maximum. So if you’re going that fast and try to decelerate quickly, even without any load from the bit, you are more likely to skip steps. It doesn’t sound like it’s skipping steps, but maybe? If this is the problem, then you need to reduce the acceleration, or get a 24V power supply (if your controller can handle it).
If you’re ok with 30mm/s and you just want to stop the burning. Can you turn down the speed of the router? What about going deeper per pass? Is the bit you have a straight cutting bit or a spiral cutting bit?
I think junction deviation was set a little too low and I had Arc resolution a little too fine. Pretty sure it was flooding the buffer with really tiny segments. A while back I swear we figured this out but I didn’t change the firmware now I can’t find the post. So I have new firmware running on the 3D printers and will try it on the CNC’s tonight I hope (If I can find code or make some that trips it up)??
“If you’re ok with 30mm/s and you just want to stop the burning. Can you turn down the speed of the router? What about going deeper per pass? Is the bit you have a straight cutting bit or a spiral cutting bit?”
I can try some straight bits and see what I get, and have ordered some single flutes. I’m running the 611 as slow as it will go. I did not think to try cutting deeper - it’s just foam, but I assumed that a deeper cut would get hotter and had been trending the other way in my thinking.
I am cutting letters for signage out of styrofoam, so the particular video I posted was from cutting an O. I am not familiar with turning arcs on and off; is that somewhere in Estlecam?