Can I convert Gerber X1 to Gerber X2 or Gerber X3?

[rkulkarni]

I have Gerber files (.pho and .fph) files provided by the customer. I need to convert these Gerber files to Gerber X3 format. For a PCB which I have designed, I can export the design file to Gerber X2. But the customer has provided only Gerber files to us which I need to convert to Gerber X3. What can I do to achieve this? Is this possible in KICAD? If not, Is there any add on or a plugin which I can use for this?
Thank you for all the help in advance.

[retiredfeline]

Not as far I know, KiCad is not a Gerber editor or converter.

[Naib]

Unfortunately not. GerberX3 includes additional information associated with assembly (ie centres and rotation…) and thus needs to be generated at the design stage from the rich file formats specific to the CAD package.

you would need the pick and place file to stand a chance of generating an X3 but there is no “conversion” but you might be able to if you were to convert GERBERS to a pcbnew file and then “place” components onto the “pads” to recreate the rich file information to then generate an X3 datapack

[rkulkarni]

Just to summarize for my understanding, I can convert the gerbers to a design file, then place the footprints of the components on their designated place and then generate gerber x3 from that ‘design’ file.
Right?

[Naib]

That is correct. The 1st step would be to just generate the X3 data and re-use your GERBER-X2 files… to generate an entirely new dataset using this method has additional risks. you might need to do a full generation but 1st start with the safer, limited generation.

1. open Kicad Gerber viewer
2. load the GERBER files
3. File → Export to PCB Editor
4. associate GERBER files with pcbnew layers - you only need todo F.Cu, B.Cu for this activity
5. open pcbnew
6. open saved design
7. MANUALLY add footprints which are the same as the design intent footprint and align with the pads.
8. Save and generate ONLY the GERBER-X3 information (File → Fabrication Outputs → Component placement) and select Gerber (experimental)
   
   
   
9. bundle together the previously generated GERBER-X2 with the new X3 files and load into the gerber viewer and ensure all footprints have the diamond centre+pin1 indicator

It maybe tempting to generate all of the gerber files again and have a fresh complete kicad generated set but I am 100% certain that the kicad footprints and the original footprints will differ causing GERBER artifacts on F.Cu B.Cu. Likewise you might not have place EXACTLY causing additional copper artifacts. The X3 information is stored in separate new files but standard GERBER grammar and thus you can use your previous GERBERS and just the assembly information in these new files and even if they were off, the reflow process will pull the parts into alignment (within reason…)

Step 7 is the riskiest step and it might be impractical if you have lots of components