I need some help. I have had my machine for about 2+ years.
I have busted some pieces a few times due to my pushing machine too hard.
Any way, this last time, I purchased the new Burly printed parts kit.
After the rebiuld, I have an issue with the cuts seem correct then start cutting too deep.
I tried the same file a few time and each time it happened in a different spot. I also tried a few other files that ran good, and get the same thing, cuts fine then too deep.
I have checked all the wiring. Only the Z seems to be acting up. All wires are in casings, and plugs taped with electrical tape.
I have thought about static, ( it was an issue when I first built it 2+ years ago), So I shut computer down, unplugged power and USB and all wires to Arduino board. Board is the one that came with the kit 2+ years ago.
After putting all plugs back and trying a few more cuts still have same issue, starts cutting to deep.
My machine is leveled to table. X, Y, and Z, move smoothly, when I jog them with the controll panel in Repiter Host. I have moved it all around the whole cutting area, 23"x 23", with no hang ups.
I have enclose some pictures of machine and what it is doing.
Thanks in advance for any help to get me going again. I love making things with my “Minion”, so named for the blue and yellow colors.
Check out my FB page Krieteative Designs, to see some of what I make.
You need a voltmeter, and you can measure from the screw potentiometer on top of the driver to ground. Be careful to not short anything, or you could toast some parts. I find the easiest ground to measure from is the power supply ground.
Does aspire generate gcode with inches per min in the gcode and repetier host do the conversion to mm per min? Marlin doesn’t support inches by default so it might be interpreting in the wrong units.
Ideal would be if Aspire would allow inches for working coordinates and generate gcode with mm per minute that Marlin expects.
I am sorry to be slow with this. Could you send a link or picture of what I need to clip where. My skill level is low with this stuff. I can do simple things like get the machine wired up but am not very knowledgeable beyond that.
This line is funny. I can’t explain why that would affect your Z height, but it is odd:
G0 X106.421 F2000 Y39.611 F2000 Z5.001 F500
I think Marlin would read the x,y,z, but I’m not sure which F it would choose. In this file, I only see that after the Z is already at Z5.001, so I don’t think the Z is moving too fast. The other Z moves show F254, which is 10ipm, or 4mm/s.
Actually, the very beginning has this:
G00 X0.000 Y0.000 Z0.000
G1 Z5.001
That would move the Z up at whatever the last rate was. That would explain it. You should add F600 to the Z lines, like this:
G00 X0.000 Y0.000 Z0.000 F300
G1 Z5.001 F300
I don’t know aspire well enough to change a setting. If there’s an area with some start gcode, you could add G1 F300.
Don’t mess with the multimeter. I am worried you’ll accidentally short something.
OK so Fxxx is the speed at which X, Y and Z move.
Is there any place that tells Z how far up and down to go?
So what is G0, G1 at the begining of the lines?
I really appreciate all your help. I am on winter lay off, I pour concrete and this is the time of year I get to spend the most time using my machine.
I have already missed my time frame for any gifts this year…
I hopefully get this sorted out with your help and make some late gifts…LOL
Sorry you’re missing that time. I bet that’s frustrating. Hopefully, you’re finding other things to do to enjoy your time off.
The Fxxx is speed, in mm/min. It applies to the current line, and it is “sticky”. It applies to moves after the current one too. So:
G1 X10 F600 ; Speed is 600 mm/min, or 10mm/sec
G1 X20 F1200 ; Speed is 1200 mm/min or 20 mm/sec
G1 X0 ; Speed is still 1200 mm/min
G1 Z ; Speed is still 1200 mm/min. Now this command is potentially dangerous, because that's too fast for Z on some machines.
The G0 means the same as G1 on these machines. It’s the type of command, and G0/G1 means “Move in a straight line”. So G0 X10 means, “Move in a straight line to X=10”. G1 X10 Y10 means, “Move in a straight line to X=10 and Y=10”.
These lines mean:
G00 X0.000 Y0.000 Z0.000 ; Move in a straight line to X=0, Y=0, Z=0
G1 Z5.001 ; Move in a straight line to Z=5.001mm
The trouble is, the speed is stuck from whatever command came last. Whatever speed it moved at before, it’s going to try to lift the Z from 0 to 5mm. If that speed was 2000mm/min, then it won’t be able to move that fast, it will skip steps, and even though it thinks it is at 5mm, it will be at 4 or 3. Then when it move back down to 0, it will really be at -2mm.
So I need to max all the Fxxx to a slow speed no more then 600mm/min.
That should cover this issue.
that should be for X and Y too?
And I will switch Aspire and Repiter Host back mm/min in the settings.
