Eagle has the ability to load images into library components and directly onto boards using the import_bmp.ulp user language program. import_bmp.ulp imports an image as a series of thin horizontal pieces; this works well on the silkscreen layer, but will generate errors on the copper layer as the pieces are most likely thinner than the minimum trace width your DRC is configured to check for. I have been searching for an easy way to import relatively complex logos and graphics and have them load onto the copper layer effectively without hundreds of errors. Loading the logos into the restrict layer seems to work well.
For this example, I will import the logo from the University of Alaska Fairbanks into my Eagle libraries. The logo without text was taken from the UAF branding site’s alternative options. Gimp was used to resize the source image to 3000×1500 and threshold it to be black and white. I have had more luck using a large input image and a small conversion factor than the other way around. MSPaint was used to resave the bitmap as a monochrome bitmap. The image was imported three times; one to layer 1 (Top) and layer 21 (tPlace) by selecting the black sections, and another to layer 41 (tRestrict) by selecting the white sections. The target size was .5″ tall. The pixel/mil conversion factor should be 500 mil/3000 pixel or .1667.
It is clear this isn’t a perfect approach, as it requires two steps to add the logo. Adding the restrict object from the library and the copper pour is more complicated than simply adding the copper object. If the logo has too much detail, the width of the pour needs to be small enough that it generates a DRC error as well. I’m not sure what the results of having these two approaches manufactured would look like; while Eagle generates a large number of DRC errors, the I suspect the gerber files would be very similar and I’m not sure if board houses have a preference on etching one over the other.
Here is a quick shot of the board with a zero-width copper pour using Mayhew Labs’ 3D Gerber Viewer to see the resulting gerber files. The layer 1 logo and restricted-copper approach logo appear indistinguishable in this viewer.
Here are the board and gerber files used above: eagle_logos.zip