Contents:

PDF → PCB → footprint conversion

What you need

Step 1: Get a footprint image

Step 2: Clean the image

Step 3: Fine tune the conversion

Step 4: Editing in PCB

Step 5: Convert to footprint

Step 6: Design the board

Step 7: Prototyping, testing, manufacturing

Related: Sharp Zaurus SL-C3200 and its hardware modifications and extensions, my gedasymbols.org page.

PDF → PCB → footprint conversion

When designing a PCB, you often have a data sheet, but the parts library lacks the footprint. You can draw the footprint from scratch, or you can base your work on an existing data.This manual shows conversion from an image in the data sheet to the PCB footprint.

What you need

Pstoedit has several new options:

pcb:			.pcb:	pcb format 	(/usr/lib64/pstoedit/libp2edrvstd.so)
This driver supports the following additional options: (specify using -f "format:-option1 -option2")
[       -grid	: double	: attempt to snap relevant output to grid (mils) and put failed objects to a different layer]
[   -snapdist	: double	: grid snap distance ratio (0 < snapdist <= 0.5, default 0.1)]
[    -tshiftx	: double	: additional x shift measured in target units (mils)]
[    -tshifty	: double	: additional y shift measured in target units (mils)]
[       -grid	: double	: attempt to snap relevant output to grid (mils) and put failed objects to a different layer]
[         -mm	: boolean	: Switch to metric units (mm)]
[   -stdnames	: boolean	: use standard layer names instead of descriptive names]

Step 1: Get a footprint image

In my case the source of the drawing was the data sheet of Hosiden Multi-Pole Rectangular Connectors.

PDF in Evince

Step 2: Clean the image

You have several ways to clean the source:

  1. Open source directly, edit and print to ps file.
  2. Print to file and use psutils to get selected area.
  3. Convert selected page using pstoedit:
    pstoedit -page 5 e_c06_kaku_takyoku.pdf TCX3106.svg

I did the last one. After few minutes of work in Inkscape, I extracted only data related to the footprint.

Converted to Inkscape

Step 3: Fine tune the conversion

Most footprints need placing of pads to the grid. That is why the pstoedit pcb output can snap lines to grid. Grid size and shapping strength are user definable.

The conversion is redundant and a simple heuristic tries to generate each element in all possible menanings (via, soldering pad, copper plate, silk). You should delete all these elements except the correct one.

pstoedit -xscale 0.555632727 -yscale 0.555632727 -f "pcb: -stdnames -tshiftx -0.0947 -tshifty -0.886 -grid 0.1 -mm -snapdist 0.4" TCX3106.ps TCX3106-%d.pcb

Raw PCB output

Notes:

Step 4: Editing in PCB

Now you need to verify correctness of all dimensions and eventually fine tune the silk layer drawing.

Final PCB output after cleanup

Step 5: Convert to footprint

Following the PCB manual, you will have to convert the result to the footprint format.

Final view of the footprint

Step 6: Design the board

Finally, you are ready to desing your printed circuit board using your new footprint.

Final view of the footprint

(The image shows work in progress.)

Step 7: Prototyping, testing, manufacturing

I abandoned this board and decided to build a different design.