EstlCAM is for generating GCode.
This software seems to do everything I want. It also seems to be translated into every language I’ve ever heard of, if not you can add translations in the software. The installer is in German I think but the options are easy to understand. Please buy a copy if you find this works for you.
Step one – Install Estlcam¶
Install Estlcam. Using the default options in the installer, add Icon to start menu and desktop. The first window that pops up I set the language, change the display units, and set it to show the feed rate in mm/s on the tool popups.
After you click okay close Estlcam and restart it to update the settings.
Step 2 – Setup¶
After restarting Estlcam, open the setup tab, these are the settings from the first window plus a few extra.
Changing the clearance plane to something a little smaller really speeds up a job since the z axis is the slowest. This is how far above the material it should travel to before it moves. You should change the milling direction depending on what kind of material you are cutting, more on this in another post. Setting the z-axis origin to the top of the material makes it easy to set the home position, along with that is program start – at origin. Choosing to end the program “above origin” is safe, “above last position” is the fastest.
The creator of Estlcam recently updated his software for us! In the CNC Program Generation tab, choose Marlin (if you are using my firmware). Important – Set feed unit to mm/min- (this is what the marlin firmware needs). Change the file extension “gcode” so all the programs recognize it.
Next up is the travel feed rates. 2100/60=35mm/s, 480=8mm/s (keep the Z low)
I delete all the default tools and use this as a conservative test speed setting for an ⅛″ flat endmill in wood. Do not exceed 8mm/s in the z plunge field unless you know what you are doing and know what firmware limits you have.
You are ready to generate some GCode.
Step 3 – 2D gcode, Good for pen plotting or 2D milling (cutting things out)¶
Grid Size. DXF files are crazy sizes sometimes so to make sure your DXF is the right size change the grid. Found in View>Grid I set mine to 10mm or 25.4mm=1in.
For this 2D or 2.5D work .DXF files are used. You can use any vector program to make them, illustrator, SolidWorks, etc. Get some files from here, (Need a new source, sorry).
Open DXF. File>Open – If your DXF is completely the wrong size try again with different initial units.
This is what the crown looks like imported in inches as the initial units. This is whatever units you save your DXF as.
Step 4 – Scale / Re-Zero¶
The crown imported at about 55mm wide I want about 150mm wide.
Select>Resize>Drawing Layers, then click on the DXF to select it. I scaled the crown 250x to get it to 150mm (5 ¾″). Zoom out to see your DXF.
Zero>Create arbitrary point, then select outside of the DXF paths. This is how to set your origin (or Home). The little blue plus symbol is what your machine sees as 0,0 (x=0, y=0, generally the lower left corner of your work). When you start your program the machine will work to the right and above where you start it from (represented by the blue plus). Some people like to work from the center for round or oval objects.
Step 5 – Select the tool paths¶
To use the pen you want to drawn on the line so use engrave (tool centered on line), if you were cutting a part you can choose part (tool edge on the outside of line), or cutout (tool edge in inside of line). Click Engrave then just click on each line segment.
Step 6 – Save¶
Export. File>Save CNC Program. Give it a name. You will get a depth popup, for the pen I use 1mm or less, anything else set it to the thickness of your material plus a bit to cut all the way through. You can then preview the path.
Step 7 – Control Software¶
Open repetier-host. load the .gcode (or .nc , .ngc) file you just saved. If you have the bed size adjusted you can get a sense of scale. If you can’t see the lines check the box Print Preview>Show Travel moves.
View it from the edge and you can see, that the path is below your z-home, and the movements are above z-home.
Don’t pay any attention as to where it is shown on the bed. It will start where ever your head currently is.
Start. Put the tip of the pen (or tool) a hair above where you want it to start and hit run. It should pick up, move, drop down and go. If it goes down first and doesn’t pick up between moves your z axis is backwards. Flip the plug.
Test Crown 12mm/s– If you are having problems try this one (If you are having download issues -Right click- Save as.).
This all it takes to plot with a pen or do basic 2D (2.5D) milling, some of the most common things this type of mill is used for. Make sure to adjust your tool and its settings depending on the material in use. Always do a test cut!