Redesigning an existing circuit board

[Bernie]

Hello,
I use KiCad 7.0 and I want to change a small PCB from a remote control of a RC model with a placement of a switch and a button and connectors.
The new board can look different but the switches have a certain distance and this should be kept. On the new board should be additionally a switch-off delay with a capacitor and a trim potentiometer and with their two connections then connected.
I do not know with which function I can design this.
I would have to measure the old board because of the distances of the switches/buttons.
Do you have an idea how I can realize this?
Thank you greetings Bernie from Germany

[hmk]

I reverse-engineered / drew schematics of a couple of boards recently with KiCad 7.0, in short with the following workflow.

• Take a good sharp picture of the board, from each of the two sides. Perpendicular to the board if possible.
• Make corrections to the pictures so it has the right perspective, i.e. is “flat” and to scale in both X and Y directions. This can be done in Gimp or any other good equivalent application.
• Flip one of the pictures so both have the same orientation of the assembled components.
• Take note of how many pixels correspond to a certain known physical distance on the board. Double check that the, PPI, pixels per millimeter or whatever reference you use is the same in X and Y direction.
• Export a PNG.
• Insert the pictures, after they have been processed, in a user layer in the Board editor of KiCad, use a separate layer for front and back side of the board.
• Draw outline of the board, make sure the measurements and image match.
• Start putting symbols into the schematic editor, corresponding to the components on the board. Keep the same references as are already present on the board.
• Pick footprints for the symbols that match the actual footprints on the board. You might have to modify or make your own footprints.
• Update PCB from schematic in menu “Tools”. Do this every time new symbols with footprints have been added.
• Place the new footprints in the board editor to match the placement on the picture.
• Once you have placed all the components, you can double check and fine tune the sensitive measurements.
• Go through the symbols and connect them in the schematic according to the traces on the board, until you have a complete schematic.
• Route according to either the original layout, or a different routing pattern.

I hope that can be to some help, with suitable adaptions of the above workflow.
When you have drawn the original schematic and layout, you can make a “Save as” of the project and start modifying in a new project.

[Heath_Raftery]

It might be worth figuring out whether the existing board is more than 2 layers or not (maybe by cutting one and seeing if you can see copper within the board?). If it’s more, then there are internal layers that you’ll have a hard time reverse engineering. In that case, you might be better off reverse engineering the circuit, and starting from scratch with the schematic. If it’s only two layers, then you might want to remove all the components and stick it in a flatbed scanner. You can then graphically edit the scans to the point you can use “Image Converter” in KiCad to recreate the tracks. From there you can edit the tracks and place your extra components, and possibly get away with not having to create the schematic.

Either way, hmk’s suggestion of a high quality, distortion free photo is a good one. The fallback method is a set of calipers and a lot of time measuring from one point to another. But if you have to-scale photo you can trace over that will probably be quicker.

[Bernie]

I now came up with 2 other possibilities:
1 . Only a capacitor 10uF and a trim potentiometer must be soldered on, I could solder that on simply and interrupt a conductor track.
2. I solder out the switch / trim potentiometer and connecting leads and design a new board for button and trim potentiometer with spacing of 14mm.
That would probably be the easiest variations.
Thanks for your ideas and help,
Greeting Bernie from Germany