How to Convert SVG files to DXF to machine your logo

One of our sponsors gives us laser-cutting service, so we’re cutting our team’s logo into some of the parts.

Our art students use GIMP (which supports a slew of image formats including SVG, but not DXF). Our mechanical students use SolidWorks, which can import image files, but not SVG.

We can save the images as PNG or JPG, import them into SolidWorks as images, and manually trace them, but this is lossy, very tedious and never as good as the original.

To export your GIMP art cleanly into SolidWorks:

  1. It works best if your SVG is 2-color, not grayscale.
  2. Save it as SVG (scalable vector graphics) - a file format that scales nicely and doesn’t blur like PNG or JPG.
  3. Post your SVG file on Google Drive or Dropbox.
  4. Create (and activate) an account at CloudConvert.
  5. Use CloudConvert to turn the SVG into a DXF (design exchange format - a 2D CAD format that will work with a variety of CAD programs including SolidWorks, Creo, and Inventor)
  6. Open the DXF in SolidWorks (or Creo, inventor, etc). In the import dialog, choose “Import to a new part as a 2D sketch”.
  7. The sketch should have all the lines from the SVG, but might need cleanup (make sure you don’t have a mix of open and closed surfaces, for instance) if the original SVG was too complicated. The “trim entities” (especially the ‘power trim’) tool is useful for this.
  8. Extrude a Boss from the the sketch.
  9. Insert->Features->Scale to scale the logo to the right size for your part. Scale about “Origin” works better than about “Centroid”.
  10. Go to the part where you want to make the logo cut.
  11. Insert->Part, inserting the logo part. The import dialog in SolidWorks is pretty annoying, so don’t stress out about getting it oriented and positioned here. It should import as an additional solid body(ies).
  12. Insert->Features->Move/Copy to rotate or translate the logo to where you want it. You can do this in several steps (which I recommend: try getting the orientation 1st then translating 2nd).
  13. Make sure the logo sticks through your sheet on both sides. Make the logo part thicker if necessary.
  14. To turn the logo into a cut in the main part, Insert->Features->Combine. Select the plate as your Main Body, then select all of the logo bodies (1+) as your Bodies to Combine. Select Subtract if it’s not already. You can preview.
  15. You’re done! Be careful of stress concentrations due to sharp corners. Also be mindful of the minimum cut size of your manufacturing process (i.e. laser cut or plasma cut diameter).

Would of been nice to know before manually measuring arcs and circles on a picture and then imputing into inventor. Most likely will do this to get a more accurate version.

Inkscape is useful in this process too. If it doesn’t directly export to DXF, I know there’s a plugin for Inkscape that will allow it to.