I’m encountering challenges in identifying the front copper and silkscreen layers in KiCad. On the front side of the PCB, I only have copper traces, and I used a CNC machine to cut these traces. Consequently, the components must be inserted from the back to facilitate soldering on the front side. While the front silkscreen displays the components, I require this information to be present on the rear side.
If you can hear an air of disappointment in my tone, it’s because I got all the way, solder mask, drilled, all components on the board and I was just putting in the final IC’s and realised that symmetry was no longer on my side.
Should I have placed all the routing on the back copper layer? Can i copy the front copper layer to the back copper layer and mirror? I would like to repair this.
If I may also ask, what should I have done in the first place?
So you’re using the silkscreen as an assembly guide? Could you plot that and mirror the PDF before printing?
Edit: Or do you mean you have placed the B.Cu of THT footprints on F.Cu without mirroring? Then your footprints are mirrored for ICs and have to be inserted from the front and soldered on the legs, which is doable. If that’s not acceptable you have to redo your layout.
It is not exactly clear what you have (done) and therefore what the problem is or how to “repair” it.
KiCad has: PCB Editor / View / Flip Board View if that helps.
You can’t just mirror (multi pin) footprints. That would also imply you have to mirror the physical parts. There have been some historical IC’s which could be bought in two versions, with the pins on the package were bent “upwards” or “downwards” to create the mirrored footprint, but those are rare and it not very useful.
I do recognize that Front / Back of the PCB and mirroring can be confusing. To avoid most of the confusion, it is usually best to keep close to the most common conventions, which is that THT parts are inserted from the top of the PCB. The footprints in KiCad are also designed in such a way that their silkscreen corresponds with the side from which the footprints are inserted. If footprints are flipped to the back of the PCB, KiCad takes care of “mirroring” the view, because you are now looking though the PCB at the bottom of those footprints. If you have footprints with text (Such as the KiCad Logo) those texts also look mirrored when viewed in KiCad.
It is also common convention for all Gerber layer output to show them as viewed from the top of the PCB. KiCad has an option to mirror plot outputs, but for gerber files this is (rightly so) disabled. For home etching with for example the “Toner Transfer Method” you want mirrored outputs and this can be done with for example, .SVG output. If you are milling the PCB, you can also use the “Toner Transfer Method” for putting silkscreen on the PCB after milling.
if you want to swap the copper on top and bottom layer, then the easiest method is probably to first enable some internal layers, and then:
Select all copper on top layer.
Press e for edit, and set it to an internal layer.
Select all copper on back layer, move it to the front layer.
Move the copper from the inner layer to the back layer.
This works for THT parts if you still want to insert them from the same side, but not for (multi pin) SMT parts, because you have to turn them around to solder them on the bottom. But KiCad can flip copper tracks to the other side just as easily as footprints. Just make a selection and press f for Flip.
If in project you have components at top and tracks at top then tracks should be at top and components should be inserted from top side. Of course 2-pin components (resistors, capacitor, coils, diodes) you can insert from back but with any 3+ pin components (with their footprints pads not in straight line) inserting them from back if in project they are at top mirrors their pins what is not what you probably want.
You should place routing at that layer at what you want it. Most of THT components can be soldered classically (from the other side then they are inserted) but also can be soldered form that side that they are inserted. So you can use both sides for routing. Component pin can even be soldered from both sides allowing you to have one net at both sides even not using vias.
If you have done project with elements at top and connections also at top and you want to move connections to bottom you should copy copper layer (probably possible - I have never had such need so not sure, and I am now at PC without KiCad here) but you need not to mirror it.