BOM & CPL files

[LS120nz]

i need to make a BOM and CPL file and i only have Gerber’s and not the original Cad files to make them in KIcad… is there a way to do this??

[paulvdh]

There is a lot of difference between “Gerber Files” and “Gerber Files”. The latest versions of the Gerber file format can include netlist and footprint info, but it’s optional, and KiCad has a Gerber Viewer, and Viewing is (almost) all it does. It does have an export feature to make a KiCad PCB out of a set of Gerber files, but the process is not complete and needs manual touch-up.

Recently I wrote:

Reverse engineering KiCad project from Gerber files

2021-09-06Txx:xx Work in Progress. Incomplete! 2021-09-06T15:15 It’s fairly complete now. Time for something completely different. Some help with proofreading and finding missing or unclear parts is appreciated. The goal of this reverse-engineering tutorial is to re-create a complete KiCad project from partial information. I assume the only information available is a schematic in some readable, (but not EDA form, such as a .pdf or a .png picture, and a set of gerber files. In short, the step…

But it assumes you do have a schematic in some format.
Re-creating the schematic from the copper tracks laid in copper can be done if you have a complete PCB and know resistor values and IC type numbers, but it’s an iterative process and quite time consuming. The process would sort of be:

• Put one IC on the schematic, label it’s pins and update the PCB from the schematic.
• Put the IC Footprint on the right spot so the attached copper tracks get the net names of the labels.
• Follow a track to some other footprint.
• Put the schematic symbol belonging with that footprint on the schematic, and draw that connection in the schematic.
• Repeat this process until the PCB is free of DRC violations.

In KiCad, the schematic is the reference, and the only BOM tools in KiCad work from the schematic. Going back from Gerbers to a KiCad PCB and then back to a schematic is a quite involved process.

If you only want the BOM, then it’s quicker to do it manually, but you can get a bit of help from KiCad:

1. Load the Gerber files in Gerbview.
2. Make a PCB out of it.
3. Hide all layers except the front silkscreen layer.
4. Open a spreadsheet or text editor.
5. Type a BOM entry for a single footprint on the PCB.
6. Remove the graphics for that footprint in Pcbnew (It’s just graphics at this stage).
7. Goto step 5 untill done.
8. Repeat for the bottom layer if the PCB has footrpints on both sides.

Re-creating the placement data will need real footprints on the PCB. and this is a part of the reverse-engineering FAQ article I made.

[LS120nz]

thanks for that i do have the scmatic and gerbers so that is where i will have to go i think this is one of the pdf i got back from them… 01-XY location does not match with the assembly drawing.pdf (561.7 KB)

[LS120nz]

that’s is awesome… thanks… it will help heaps.

[LS120nz]

i have a question in that the schematic i have is pdf?? do i need to re make it in schema to get the components?

thanks