(With Illustrator and Eagle)

  1. Draw the outline of the panel around your main PCB. Set the coordinates origin to the bottom left corner of the panel outline.
  2. Set units to mm.
  3. Use the Export / Partlist function to get a text file with the XY coordinates of all parts. You can use grep to remove the lines with R/C components or IC and only get the jacks/LEDs/pots :)
  4. Create a new blank board and draw the outline. Set the coordinates origin to the bottom left corner. In all the next steps, don't bother putting things exactly at the right position - put things at approximative locations, and then edit the object properties to fix the coordinates with the exact ones you have in your text file (Note: one of Mutable Instruments' secret weapons, along with autobom.py is a python script that converts such text files to DXF ASCII for panel CAD).
  5. For the mounting holes coordinates, refer to this. You can use the via tool, this will expose a bit of copper (or gold) around the hole.
  6. For the pots, jacks, LEDs, buttons use the hole tool. The "Drill" property sets the diameter (6.5mm for jacks, 7.5mm for pots, 3.1mm for LEDs...)
  7. For artwork, you have 3 colors in your palette: PCB soldermask color (green, black) is the background color, silkscreen color (white) is what you draw on the tPlace layer, but you can also expose traces (silver for HASL finish, gold for ENIG finish). To draw something in golden/silver, draw it on the Top layer (red color), duplicate it, and set it to the tStop layer (grey hatchings) - in other words, something appears golden or silver on the PCB because there's a trace there (Top) and because the soldermask is not applied on top of it (tStop).
  8. Use the Print command to print a 1:1 PDF of your board.
  9. Import the PDF in Illustrator or any other vector graphics program. Create all your type/artwork on top of it.
  10. Export the result as a 600 dpi BMP file. Process it in Gimp / Photoshop to get a 1-bit bitmap. I start by going into Greyscale mode, then use Curves to get a high contrast B&W image, then convert to bitmap with 50% thresholding - don't use dithering - it won't look good and will make huge Gerber files. Depending on the PCB fab, your resolution on the silkscreen is in the 200-400 dpi range only because it will bleed. The soldermask/traces are a bit more precise, but some PCB houses will run a simplification process on the soldermask (tStop) layers to remove small islands.
  11. Use "run import-bmp" to import your artwork in Eagle. Pick the first color in the first dialog box shown by Eagle (I am not sure if I understand how this step works or if there's a bug in the Eagle script - I often have to pick the black when I want to import the white! - so if you get your artwork in negative try again with the other color!). In the next dialog box, input the correct DPI value to have the graphics imported to scale (otherwise there's a lot of trial and error to align it with the board, and you can't resize it in Eagle once it's imported). The text will be added to a new layer. Select everything and move it to the tPlace layer.
  12. Bonus trick: if you have elaborate graphics in gold/silver, you can have a uniform polygon ("ground plane") on Top under the area taken by the graphics, and use only the tStop layer for the graphics - rather than having two copies of the artwork, one on Top and one on tStop. This can help with the Gerber file size.