here is the g code for the one part of the file. the whole file is 7 parts, one for each bit.
Script Letters 20V 12_18_19.gcode (474.2 KB)
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.
The XY speeds are ok. And It looks like the Z moves were already ok. The one that I saw that was dangerous was just that first one.
1 Like
make sure the x-y gantry isn’t too tight and causing the z axis to bind.
whole machine moves nice and cleanly. I use the jog buttons on repeiter host and it moves all around the table and up and down.
Hello Jeff,
I went back into Aspire and Reptier host and set them both to mm/min.
Then I went back and updated the file and resaved it.
Then when I loaded the G code into RH I scrolled through the code in the editor.
I you look at the picture above, Line 1088 and 1089, repeat themselves about 15+ times so far and I am only slightly into the code.
If I try and delete the lines it leaves an empty line. Will that affect the code or do I need the lines in there?
As you can see in lines 1090 and 1091 the F speeds go back to being correct.
It is like this all through the code, like I said I have seen it 15+ times and I am barely into the code.
I don’t think that’s the problem. Those are goofy (because they define F more than once), but I can’t see how that would affect your Z. The next Z move defines a F254, which is fine.
ok I am running a test cut of the resaved file in a piece of foam board now.
I will like you know how it goes
thank you for all the help
it still looks like it is too deep.
I lowered it it only .045" deep, that should be about 3/64" deep.
still looks like about an 1/8".
But it is all uniform in depth …so far
It cut the whole file complete with out any issues.
Thank you.
I have one last question.
I am using a 1/8" 20 degree V bit, cutting the script letters.
What should the depth be, I am still loosing the inside of the "e, o, a, d, b, p, R, B, etc.
Could you post a Pic of the cut, to show us what you mean by losing the inside of the letters?
Something is goofy with that dialect of g-code. There is a Marlin postprocessor for Aspire. Are you using that?
Here are some pics. even one of my micrometer.
I started with the depth setting of .075, thought that would be nice.
lowered it to .045 and still to deep.
the pics are at .045" deep.
I think so. Have been using it for a while.
says;
marlin (mm) (*.gcode)
If you do that type of cut with a V Bit it will vary the depth for you and keep real sharp corners.
But the whole cut, ( all the words are too deep), as in the pictures all the inside of the letters are missing.
Two solutions/issues. Firmware or CAM.
Test the machine when you say move up 30mm does it move exactly 30mm? If so you have bad CAM or CAM Post Processor. If you are still using Aspire all sorts of people are having issues with the ebay version and my PP, I suggest estlcam.