Hello,
I have a PCB drawing (in PDF) that I would like to reproduce to manage a Gerber file.
Is it possible to manually draw a PCB without editing a schematic?
That is, to trace the PCB from an image of an existing PCB?
Thanks.
Alain
it’s possible but not advisable.
1 Like
Sure it’s possible but as poster said above not advisable. You won’t be able to run any design rule checks and it’s open to way too many errors.
You will be laying out a PCB design blind.
Thank you for your advice
Alain
I tend to agree with the advise of both Claudio.Lorini and gmc. I also used to give this same advise, and in a lot of situations it is the right advice.
However, KiCad’s ability to draw a PCB without a schematic and the netlist it produces has also been improved, and it is at least “doable” in KiCad V8. The general workflow is:
- Place footprints on the PCB. (All pads are of the <No_Net> type.
- Draw a track between two or more pads. KiCad lets you freely draw tracks between pads which are part of the <No_Net> net.
- Give the net a name, by editing the properties of a track segment and adding a new / unique name in the “search box”.
After step 3 all connected copper (and the pads) now are part of this newly create net, and this net will also maintain a clearance from other nets.
But still. Whether this is a good workflow for you remains to be seen. Can you post the PDF which has the PCB view?
I’ve seen others post when trying to do this and it tends to not end well. Some even posted back that they eventually just put in the schematic and did it the proper way. If your PCB is fairly simple, it likely won’t take to long. May even be faster than trying to do it just on a PCB.
A schematic is preferred but, not absolutely required.
If not wanting to go the Schematic route, keep reading…
There are many Programs and ways to get a PNG from a PDF.
Kicad can use PNG in the PCB. Of course Color is important - you want to be able to see it.
Once having the PNG loaded into the PCB-Editor, you can Trace the Tracks as desired and add Terminals/etc…
Quick, crudely made Video shows two of the many ways to get PDF to PNG and then use in Kicad. I did not make the effort required for an Academy Award…
First: Loaded the PDF into Gimp - did not bother to video the Exporting or setting background color to Transparent (and that doesn’t matter as long as you can see the traces to do your layout).
Second: I loaded the Exported PNG into simple drawing program and Inverted the color (the program default is set to Transparent background) then saved.
Finally, loaded it into Kicad PCB and dred example Track and placed a Treminal…
I used Gimp only because some folks use it (I don’t like it). Inkscape also works… the list goes on…
You can use Kicad for any board without a schematic. You need to set the interactive router settings via the Route menu to “Allow DRC violations” and ensure that “Highlight collisions” is also checked. You will find that connections between unnamed nets cause a green warning highlight but you can ignore it. The highlighting is useful to ensure clearance when routing in close proximity to other items.
Source:
https://www.pcbway.com/project/question/Draw_PCB_without_schematic.html
That is pretty old info. The method I described earlier in this thread creates a nestlist during drawing of the tracks, and this gives KiCad to maintain clearances without any DRC violations. And therefore it’s a much better solution, but it needs a fairly recent KiCad version. It works in V8, maybe in V7, but probably not in V6 or earlier.
Thanks everyone.
Attached is the first PCB I’d like to reproduce without the schematic (PNG version, bottom view), measuring 218 x 79 cm.
I’ll try your solutions, otherwise I’ll re-edit the entire schematic and replace the components in the same order as the old PCB.
Alain
Sorry, not cm but 218*79mm
Alain
Now that is a weird picture.
Left is as viewed on the forum.
Center is as viewed in the “picture view” in my browser.
Right view is as viewed in “original size”.
Without much effort I found other screenshots of this, and also (presumably) the complete schematic.
If the schematic is available, then very likely the best way to proceed is to enter the schematic first. You can load a picture of the schematic (Is it this one: https://www.mhumhirecords.org/DIYpics/Green/gren_pre_cct4.gif ) as a background in the schematic editor and place symbols on top of it. Making the background transparent may help (but I’m not sure KiCad supports this).
Entering the schematic is simply the most efficient way to create the netlist. If you start with the PCB, you have to create net names for each net manually, and it is difficult to verify your work and make modifications. If you enter the schematic first, it gives you a full netlist, and you also have a double check / verify with the track layout on the PCB.
Also, there seem to be quite a lot of options / variants and texts written about “1176 Rev D” Apparently it’s sort of famous in some circles, but you probably knew that already.
Hello paulvdh,
I think that re-entering the diagram is certainly the best solution and that’s what I’m going to do.
I’m not a Kicad expert and I thought it might be easier to copy a PCB rather than going back to the schematic, but all the posts show me the opposite.
Yes, the PCB includes options that aren’t shown on the schematic (display circuit with an LM339, and phase inversion circuit).
No problem for me; I’m an electronics engineer and I know how to reconstruct the schematic.
Thank you for your help.
BR Alain
1 Like