Is there an easy way to overturn a PCB into a new one?

hello all,

as per title, I have to make two identical PCBs (identical schematic for both). One is done, call it the left channel. Now I have to make the right channel (it is a valve preamplifier) that should be overturned in respect to the other. In other words, the two B.Cu sides must face each other, and the left side of the PCB in one becomes the right side of the other PCB:

Screenshot - 27_02_2024 , 16_40_21

In other words: take the PCB on the left of this image and suppose that the topmost valve is V1. Now imagine to lay down the PCB in KiCad, you will have V1 on the left of the screen, like the PCB that I have already done:

The other overturned PCB, when laid down in KiCad will have V1 on the right instead, front will become rear and vice versa. Of course, all must be overturned, including traces, holes and silkscreen.

Of course the two circuits are electrically equal, only symbol assignments will change.

I hope that an easy way exists, instead of redoing all from scratch for the second PCB.

Thank you.

1 Like

The simplest way would be to do just nothing, and order two of the same PCB’s. But I’ll assume you find the aesthetics important enough to spend another half a day on it…

First, save it under a new name, as you will be creating a new PCB, and therefore it needs it’s own project. And then:

  1. Select everything on the PCB and then press F to flip the PCB. This mirrors the PCB, but all parts are now also on the back side.
  2. PCB Editor / Edit / Swap Layers to change the copper layers back to where they were.
  3. Use flip again on individual footprints to get them back to the front.

Do note that this only works “properly” for 2-pin parts. Polarized parts such as diodes need a bit of care. Connectors are a bit more troublesome, because their pinout gets mirrored too, and as a result you will have to modify the PCB to accommodate for this. (Or you have to fix this in the wiring itself). For bigger parts such as the valves (9 pins in a circle) it also does not work. You can’t mirror the parts themselves, so you will have to make modifications to the PCB to make the wiring fit again.

And in the end. DRC is your friend. When you are messin’ about on your PCB (especially moving footprints) you will almost certainly create some shorts. KiCad gets ever better in fixing such errors. In V8 you can usually drag a track out of the “shorting position”. But don’t be afraid to delete some tracks if needed. If you run DRC at the end and it stopped complaining, then you are pretty close to a working PCB again (Unless of course you just set all DRC stuff to “ignore” :slight_smile: )

1 Like

hello Paul,

The simplest way would be to do just nothing, and order two of the same PCB’s.

this is not possible because the two PCBs have the solder sides faced each other, and the components must be in the same positions, for example V1 of the left channel must face V1 of the other channel, and so on.

But tomorrow I’ll give a try to your suggestion. Now I still have to repair the mess caused by KiCad 8.0 but luckily it has been installed into a separate folder.


The valves are the problem. I can see from your PCB that the pinout is not symmetrical, so mirroring the PCB will require changing the tracking to them.

As already said your board and components don’t have an axis of symmetry so you can’t flip the layout. However you can still keep the components in their original locations and redo the tracks so it isn’t totally from scratch.

Yes indeed - Routing traces takes no time, but placing components does, could you lock the components and just re route ?

yes, true, but it’s enough that the majority of the tracks are flipped. Then I’ll have to change a few ones and the associated components around the valve sockets. As Paul wrote, two pins footprints should be flipped without problems.


I will try with a copy. In the worst case nothing will be lost.


mmmmh, it could be an idea. I will try it as well.


hello Paul,

I have successfully flipped the PCB (point 1)…

…but why Edit | Swap Layers (point 2) does nothing? It doesn’t matter if the board is all selected or not. It does nothing:

It is funny that I cannot select something on the left and the opposite on the right, only same layer or all.


Application: KiCad x64 on x64

Version: 8.0.0, release build

wxWidgets 3.2.4
FreeType 2.12.1
HarfBuzz 8.3.0
FontConfig 2.14.2
libcurl/8.5.0-DEV Schannel zlib/1.3

Platform: Windows 11 (build 22631), versione 64-bit, 64 bit, Little endian, wxMSW

Build Info:
Date: Feb 23 2024 02:24:15
wxWidgets: 3.2.4 (wchar_t,wx containers)
Boost: 1.83.0
OCC: 7.7.1
Curl: 8.5.0-DEV
ngspice: 42
Compiler: Visual C++ 1936 without C++ ABI

ok, don’t mind, I noticed now the drop down boxes on the right side of the dialog :slight_smile:

But only traces have changed side, footprints and silkscreen remain all on the back.


Yes, that is correct. You will have to flip the footprints one by one, and re-locate them on the right position. While doing this, wiring changes that need to be made will also become clear.

Probably the “most comfortable” way to fix the footprints is:

  1. Hover over pad of a footprint.
  2. Press m to move the footprint. It now gets attached to the mouse cursor.
  3. Move the mouse to somewhere outside the PCB. No clicking! (At least the first few times, to more easily see what you are doing).
  4. Press f to **flip the footprint to the other side.
  5. Move it to the end position and do a left click there. When you started the move by grabbing it by a pad, the pad center has become the “move origin”, and you can snap the pad to the end of the left over track.

Footprints can be flipped all at once. Select footprints (and only footprints) and just change their layer in the Properties panel (available from View menu if not visible already).

1 Like

Indeed. Changing the layer of the footprints in this way works without moving the footprints themselves (In contrast to flipping multiple footprints at the same time). I forgot about that function.

hello all,

thank you for all the useful suggestions. At the end I had to rearrange some footprints and change some tracks but the work is done. At least I have kept all the relevant vertical positions intact.

The following image shows the left channel, made in the usual way:

And the following is the right channel “flipped and rearranged”:

Notice that the right channel has one added component (C35) and one connector less (J17) than the other.


Also Mirror image of the entire PCB