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 version 3.46 and later that features enhanced pcb support. This version significantly improved conversion of PostScript or PDF to gEDA (EDA = electronics design CAD) pcb format. It contain heuristrics for conversion of rectangles to soldering pads and allows snap to grid.
• Optionally any vector editor capable to save PostScript or PDF files or psutils.
• If your source footprint is a scanned document or bitmap, you may consider using of bitmap → vector conversion utility, e. g. potrace.

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.

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.

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

Notes:

• pstoedit core features -xscale and -yscale. It's useful for out-of-scale drawings.
• For fine adjusting of the layout into the grid you may prefer pcb specific -tshiftx and -tshifty using target pcb units (mil or mm) without any calculations instead of pstoedit core -xshift and -yshift using source units.
• Conversion of rectangles to pads does not take in account thickness of boundary lines. Non-zero thickness of these lines is most probably a mistake of the datasheet creator. Thickness of lines in all other cases is respected.
• Default setup of pstoedit provide descriptive layer names. For the final run, you can use -stdnames to get standard names of layers.

Step 4: Editing in PCB

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

Step 5: Convert to footprint

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

Step 6: Design the board

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

(The image shows work in progress.)

Step 7: Prototyping, testing, manufacturing

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