I need to reverse engineer the entire PCB design.
I have made a PCB, but on the left side. This is a PCB for the rear lamp in a car.
I need to mirror the left PCB of the board 1 to 1 to the right side.
How can I do this?
Usually, you simply can’t do this, as most connectors, components, chips etc aren’t available in a mirrored variants or you would connect the wrong pins when simply mirrored, and you need position and/or routing adjustments.
However if you’re just interested in mirroring tracks, outline, etc, you could select all relevant items, press “f” and then move items back to the correct layer using copy/paste or the object properties.
1 Like
Do not mirror the PCB. KiCad can’t even do this. It might sort of work with symmetric 2 pin footprints, but you can’t mirror IC packages.
Instead, for reverse engineering do this:
- Make photographs of both front and back of the PCB. It is best to use a large physical distance and then zoom in. This reduces barrel distortion in the picture. Using a flatbed scanner is also possible. It may also help if you put a ruler near the PCB (at the same distance from the camera) for easy scale comparison.
- Possibly post process the images in a graphical program. Crop, contrast enhancement, rotationan other distortion corrections and such things. You can also mirror the image for the backside here, but KiCad can do it too and so it is not important and you can skip this image processing step completely.
- PCB Editor / Place / Add Image and then load each of the images onto a layer. You can combine them directly on a copper layer, but if you put them on one of the user layers, then it is easier to turn them on or off.
- Select the image that is made from the back side of the PCB and press F to flip it. This shows the mirror image of the image.
- You can also move and scale the image, either by dragging it with the mouse, or by editing it’s properties and entering numbers.
- You can also add transparency with Appearance Manager / Objects / Images (On the right side of the PCB Editor Canvas).
With this setup, you create the PCB in the normal way. So you view the backside of the PCB “through” the PCB and you work on it’s mirror image.
Some people like to use PCB Editor / View / Flip Board View, but I have never found this a very useful feature.
If I understand the original post correctly, it seems he has reverse engineered and created the PCB for the rear lamp on one side of the car, but now he doesn’t want to go through the whole process once more but just flip it in order to create the second PCB for the other side of the car, which is the mirror image.
I don’t like guesswork, but if this is the case:
Then:
- Move the layer you want to change to some empty area.
- Select all tracks and via’s you want to modify and press f to flip them to the other side.
- Select all the tracks, then press e to edit their properties, and put them on the other side of the PCB (Either F.Cu or B.Cu). Make sure that during this step only tracks and via’s are selected, because otherwise KiCad gets confused and it does not show the **Edit Track & Via Properties dialog.
Or, use the Properties panel to change layers.
Or, flip all board items using F, then do Edit > Swap Layers…
Exactly. I made a PCB design for the left side of the car.
I don’t want to do the same thing twice, only on the right side.
Therefore, I need to mirror the PCB on the left side to get the finished PCB on the right side.
In this way, I will have two PCBs made for the left and right sides from one target design that I made for the left side.
You can not directly mirror whole PCB’s in that way, because you can’t mirror the physical parts. So IC’s will not fit anymore on the mirrored PCB.
But you can mirror the outline and tracks, and both dsa-t and me have written how to do that. After the mirroring / layer swapping you will have to make more modifications so the footprints will fit again. Some footprints such as resistors, capacitors and other parts which have all their pins in a straight line can be mirrored, but a lot of other parts can not.
Original board with LED, RIGHT side.
I need to make a mirror image to show the left side of the PCB.
As below in the post
What is that rectangle in your first screenshot?
Also, consider using THT LEDs. Then you can also simply insert the LED’s from the other side. It is also quite easy to design your PCB with 6 LED’s on each side, and then only solder the LED’s on either the top or bottom side of the PCB. Both these methods make it possible to use the same pcb design for both the left and the right side.
This is the place for the sticker.
There must be SMD diodes to dissipate heat.
We have given several methods to do this, but it is up to you to choose between those methods and actually do it. Your PCB won’t flip itself no matter how many screenshots you post.
I suggest you make a backup (or a copy) of your project and start experimenting with the methods already mentioned.
You really should start with finding out what are the physical requirements for the PCB. How will it be attached to the surrounding parts? How much is there room below the top and bottom planes of the PCB? Is it mounted with mounting screws through mounting holes, or are there some kind of protrusion in the surrounding keeping it in place which may be asymmetrical top/bottom-wise? How is the original left/right design made?
Is it possible to actually just use almost identical design and just swap the whole physical PCB so that only the LEDs must be changed to the other side? In that case you can just flip the LEDs and do a little bit of rerouting around them. Otherwise you need to flip all components individually (the Properties panel of KiCad is your friend for multiple selection), flip all tracks and reroute all the incompatible tracks.
As Paul said, there’s enough information here already about how to do flipping/swapping/mirroring in KiCad. You have to choose your strategy based on the physical requirements and then you can decide how to do it in KiCad. In the latter phase we can give more advice for KiCad if you need it.
Thank you friends for your valuable advice/tips.
I will try to do what you wrote.
We’ll see what the effect will be.
Could you not just create the project as normal, then just rename the gerber files? Swap top copper for bottom copper; top silkscreen for bottom silkscreen etc?
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.