I have finally gotten my mill working but have run into an unusual error. the time to carve in Estlcam says ~2.5 hours. When I load it in Repetier it says ~57 hours. I did a test run on a different project and it indeed took 22 hours when the time was significantly lower in Estlcam.
I find it hard to believe that carving a 6 letter name, 3mm deep, should take ~57 hours. does anyone know why the times would be different and how I can fix this?
BW Steelers logo2.gcode (423.9 KB)
gooley halftone.gcode (2.7 MB)
Attaching more information could be helpful in tracking down the issue here. You could attach one or more of:
- The EstlCAM file
- G-code file
- Short video of the cut
- Screenshot of the project in EstlCAM
I’m not an EstlCAM user, but knowing things like type of toolpath, feed and speeds, rapid speeds/limits, size of the letters, etc., are likely important to understanding the root of the issue. Note that the EstlCAM file will need to be put in a ZIP file in order to be uploaded to this forum.
Thanks, Edited to include files used. gooley halftone is the file that registers ~57 hours. I carved the BW Steelers logo file in about 22 hours using a 1/8 endmill.
Thanks for the help. These are some of my first cuts with the machine. In fact the Steelers file was my first cut after testing with the crown.
A quick look at your g-code file, and I see your feedrate is absurdly low. It is set at 6mm per min. I suspect some sort of unit problem where EstlCAM is putting out the feedrate in mm per second. Marlin expects mm per min, so I should be seeing a feedrate of 360 instead of 6. See the ‘F’ parameter in this line:
G01 X12.3985 Y149.2593 F6
As I mention, I’m not an EstlCAM user, but I suspect the issue is in Setup/Basic Settings in these two settings:
Edit: I took a second look at the g-code file before closing it, and found something strange. The rapid (G0) feedrate appears to be in mm per min.
G00 X12.5838 Y151.0823 F2100
I also did not see any “compensation” for the need for the Z axis to be moved slower than the X and Y for rapid movements. Make sure you’ve setup EstlCAM as specified here.
The good news is that when you get this sorted out, your cut times should be around what EstlCAM estimates.
Looks like this was a NOOB error. Thank You so much!