Maslow Home Maslow Community Garden Newsletter

Inkscape + Esltcam Basic Workflow: JPG -> gcode

Inkscape is free software. Estlcam is available for a one-time $60 fee, but has a demo period to try it out, which is what was used for this guide. Carbide create is very similar. The goal is to show how to convert a graphic into a cutout with the Maslow Logo:


Using Inkscape version 0.92

  1. open inkscape and verify document is displayed and measured in mm

  2. paste in the maslow image

  3. trace the image
    ** select the image
    ** from the Path menu, select Trace Bitmap
    ** press the update button after making changes to see a preview before executing the trace

    (sharp color borders can make tracing easy using the color multiple scan) If it looks bad, try another option.
    ** press OK to execute the trace, then close the window with the X

  4. the trace was successful if you have two color versions of your image. But the vector trace will be on top of the bitmap image. You may want to select and move the vector just to ensure there are two. Select the new trace. We will change it to no color and outline.

    ** Select Fill and Stroke the right dock
    ** Select the Fill tab and X none (graphic should disappear)
    ** Select Stroke Paint and select the shade next to the fill
    ** Select Stroke Style and enter 3.175 in the line width (for a 1/8" bit)
    It should now look like this:

  5. Ungroup the image and remove all but the M Logo
    ** using ungroup and break apart, remove all but the M logo

  6. resize to 300 mm (~12")
    ** select the m
    ** lock the aspect ratio by clicking the lock between the W and H numbers in the menu:

    ** Change the width or the height to 300 (mm)

    ** verify the stroke size is as desired because scaling the image may change the line weight.

  7. save as svg (File ->save)


Before opening a drawing, set up a tool or ensure there is one that can be used:
click on the tool table for an entry for a new tool. A new line will appear with the name “new tool” and then by clicking on the wrench on the left of the tool line it can be edited.

This is where feeds and speeds are critical. set your flute count, your tool diameter 6.35 mm for 1/4" or 3.175 for 1/8". Set your depth per pass at a value you prefer. If you are cutting at full speed, go no more than 50% of your bit, but if you cut slower or in soft material, you can go higher. Feed rate is up to 1000 on the M2, 700 by default in the mega firmware, but if using webcontrol, it defaults to 800. Plunge is 90 degrees and can be maximum unless your work material has an issue with chipping and needs the plunge to go slower. The rest of the settings can be left alone unless you are pocketing, drilling, which may need adjustment (more info here), or finishing with a different bit. Enter the relevant details for the tool you are using and click OK.

With setup complete, proceed with the gcode generation:

  1. open svg file and select the correct unit (should be mm if that is what was used in inkscape) and click OK

  2. Next we need to select the drawing and pick inside, outside or on the line cut.
    ** If you just want on the line and the shape is a closed shape, select PART then click on the shape

    Enter details, such as the cut depth and cut order
    ** If you want the line cut on either side of the line, use the ENGRAVING option for this then select left for the inside and right for the outside. If in doubt, you can select it and then click on it and press delete to remove it.

  3. Add tabs by selecting the shape, selecting holding tab and clicking on the drawing where the tabs are desired. Spaces in the colored outline will be visible


  • if you want to control the order things are cut, like the insides of closed shapes first or one section cuts before another, use the “machining order” field to assign numbers and it will cut in that order.
  • I use a 1/8" bit, so for tabs, I use a 3 mm height and a 5 mm tab length
  • For surface engraving of only parts of cutouts for detail, use the toolpath depth of 3 mm and then set the outline complete cutout as the thickness of the work piece plus 2 mm.
  • place tabs where the oscillating too blade can easily cut them… makes getting cut piece easier to get out
  • For word cutouts, cut insides on the line and outlines outside the lines.
  1. Save Gcode file with the menu items: File -> Save CNC Program

  2. run the simulaiton and use >> to speed up movement.

cut: upload .nc file to webcontrol or makerverse and cut it out. The origin is the + on the drawing, so position maslow home or work position where the + should be.

Tip: A better surface finish without as much fuzz or soft material chipping can be realized by cutting the first layer shallow and then the remaining layers deeper to save time.


Great tutorial! You can get the estlcam software at cost $40 on our website.


Awesome, job, documenting this. Is there any reason you are using an older version (.92) of Inkscape?

Inkscape released version 1.0 to much fan fair earlier this year. I went through your tutorial using version 1.01 and only difference I noticed is the trace tool interface has been overhauled and looks a little different, but produced the same output.

Great catch. Thanks for reading. Inkscape version 0.92 is on my machine because it will generate gcode directly with the gcodetools extension and Inkscape 1.0 doesn’t work as well with gcodetools. Feel free to drop in a couple screenshots of the new trace tool in the first entry and mention the newer version. It should be editable by anyone since it is a wiki post.

1 Like

Gcodetools hasn’t been supported for years, and nobody was interested in updating it for 1.0. perhaps you could volunteer?

I could volunteer, but I lack the bandwidth and after you mentioned how easy carbide create was, I tried it and I’m about ready to move on from gcodetools.


Thank you @Orob ! This was a great read - I can´t wait to try it!

1 Like