6 Dec
2011
6 Dec
'11
3:44 p.m.
From: "Richard"; Tuesday, December 06, 2011 10:52 AM
I've got a bunch of Nuclear Data peripheral
circuit boards that I need
to reverse engineer. They are simple circuit boards with all the
tracings visible (i.e. no internal layers) and the parts are all 7400
series logic in standard DIP packaging.
If I were to do this manually, I would take high resolution
photographs of both sides of the board. From the photographs, I would
try to recreate engineering drawings: part placement and circuit
topology.
I've used Eagle for this -- the back-annotation feature makes things
reasonably easy. Assuming I have no other information about the
board, here's what I do:
In the schematic editor, add all the components. At each input or
output pin, place a wire going nowhere, and add a label to identify
the signal name. These will start out as N$1 through N$<whatever>.
If you know the connector pin-outs, use the NAME command to
give those signals the correct names. Similarly, go ahead and enter
any other information you already have, In the Eagle board editor,
draw some dimension lines and place the components in their
approximate positions.
Take your (straight, flat) photographs of the top and bottom layers,
quantize them down to two colors, rotate and scale them for, say,
150dpi or so and the correct orientation for "from the top" view.
Save them in BMP format.
In the board editor, use import-bmp.ulp to import the bitmaps
for the bottom layer. You can turn on and off layers to select
stuff and move things around until the bitmap lines up with the
dimension lines. Tweak the component locations, then use the
WIRE command to trace over the traces in the image. When
you connect nets, Eagle will ask which name to keep, so pick
the lowest numbered N$ name or any nice names you
introduced earlier.
Repeat for the top layer. If a component obscures the traces,
you will have to measure to see where it goes. Also, beware
of traces that connect pairs of IC pins which lie entirely under
the chip. You can often detect these by the shape of the
solder ball on top, which is often different if there is a trace
there from when there isn't.
Use ERC when you think you are done to see if there's anything
obvious (to Eagle, anyway) that you've missed.
Don't forget to save your work :-).
Return to the schematic editor, and "pretty it up". A whole
bunch of IC's with bristles sticking out of them isn't usually
the most helpful way to leave the schematic :-).
I've done this for a dual-height Qbus board and a few DEC
flip-chips for which I had no documentation at all, and it
isn't really very difficult.
The worst part, actually, is getting decent straight, flat images
in as few colors as possible that accurately indicate where the
traces are after you import them. If the boards are small, it
can actually be easier to skip the images and just freehand
draw what you see.
Vince