2
\$\begingroup\$

I only have the Gerber files; can I open them in Altium, and somehow generate a .pcbdoc file that I can work with (route signal, pour copper planes, place components, etc.)?

\$\endgroup\$
2
  • \$\begingroup\$ Let us know when you find one, please. \$\endgroup\$
    – jay
    Nov 8, 2021 at 16:28
  • \$\begingroup\$ Gerber files provide you with several layers of routing of a circuit and is mainly the end product of schematic design and PCB design. If you're looking at going "the other way" then it'll get very impractical and time consuming, not worth the trouble. Better to just start from scratch really ... \$\endgroup\$
    – citizen
    Nov 8, 2021 at 16:33

3 Answers 3

3
\$\begingroup\$

Not directly in Altium, however it's bundled with Camtastic which can be used:

This is the simplified process.

File ► New ► CAM Document 
File ► Import ► Gerber(s) 
File ► Import ► Drill (Browse to drill file) 
If you don't have a drill file you can create one by placing a via on a new PcbDoc then export it as NC drill
Tables ► Layers (assign the layer types)
Tables ► Layers Order (Confirm the logical & physical Layer order is correct) 
Tables ► Layers Sets (ensure your drill span shows up here)
Tools ► Netlist ► Extract 
File ► Export ► Export to PCB 

Then a lot of work if you want it to be a normal set of Altium files.

\$\endgroup\$
2
  • 1
    \$\begingroup\$ That is already half way done! I gotta change to Altium. \$\endgroup\$
    – jay
    Nov 8, 2021 at 16:33
  • \$\begingroup\$ @jay You can get a free trial and see if it's actually practical in your particular situation. \$\endgroup\$ Nov 8, 2021 at 16:43
3
\$\begingroup\$

It isn't as simple as importing the files and editing them directly - Altium cannot, with gerber files alone, determine information such as which pads make up a single component footprint.

Altium does have a help page detailing how you can reverse engineer from the gerbers, though.. See this page for their documentation, as it's pretty involved.

\$\endgroup\$
3
  • \$\begingroup\$ Generally one can tell a pad vs trace by the soldermask or lack thereof. \$\endgroup\$
    – crasic
    Nov 8, 2021 at 16:40
  • \$\begingroup\$ @crasic I do agree that was a terrible example. Perhaps a better one would be ability to tell which pads/silkscreen elements make up a single footprint? \$\endgroup\$
    – ZapTap
    Nov 8, 2021 at 17:01
  • \$\begingroup\$ This is true, and a huge limitation of Gerber format even for its intended purposes. However modern production format ODB++ files is also supported by the reverse engineering tool of Altium. This is improvement on current process where I think almost everywhere common practice is to provide cad files and Gerbers , so generally you will have access to that data in some other format. Exception is when dealing with PCB fabrication only, that is, without assembly. \$\endgroup\$
    – crasic
    Nov 8, 2021 at 17:26
1
\$\begingroup\$

Altium PCB does not have a gerber import facility, it is possible to use an external tool and convert to DXF (for example using FlatCAM).

\$\endgroup\$
6
  • 4
    \$\begingroup\$ Welcome! Can you elaborate on your answer (e.g. by directing readers to the right menu option to start the process)? My last recollection of KiCAD (early 6.0) was that it had its own .kicad_pcb format that could be exported to Gerber, and it had the ability to view gerbers, but not edit them. \$\endgroup\$
    – nanofarad
    Jan 30, 2023 at 19:05
  • 1
    \$\begingroup\$ I just skimmed through the documentation. But I believe it may be possible using Gerbview -> Export to Pcb Editor, and then using Pcb Editor to edit the data. @RobAnderson can you confirm and/or elaborate on this? \$\endgroup\$
    – Velvet
    Jan 30, 2023 at 19:44
  • 1
    \$\begingroup\$ Yes that is the way it works, use Gerbview->export to pcb editor. I just used it yesterday for editing a gerber. Of course it is only for editing the gerber, there are no links to a schematic representation. I used it to change the board shape. \$\endgroup\$ Jan 31, 2023 at 23:03
  • 1
    \$\begingroup\$ @RobAnderson I didn't dislike your initial proposal of using KiCAD. The only issue was that it didn't contain much information. IMO you can still promote KiCAD, but then describe how exactly it can be done using KiCAD. That would be worth an upvote from me. \$\endgroup\$
    – Velvet
    Feb 1, 2023 at 6:50
  • \$\begingroup\$ I am more used to Altium, I have used it for years. But it was easy to use Gerbview to convert the gerbers to a file that could be edited in Kicad. I spent quite a while trying to do this in Altium but didn't get anywhere. I have not used KiCAD for anything before this. \$\endgroup\$ Feb 2, 2023 at 16:39

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.