Regarding the Gerber files of a 4 layer PCB with 2 inner layers:

  • Top layer: Analog signals
  • Inner layer 1: Digital signals (SPI and I2C)
  • Inner layer 2: Power planes (+3.3V and +12V)
  • Bottom layer: GND plane

For better isolation between analogue and digital signals and to prevent digital noise from coupling back into analog signals, I would like to swap the two inner layers, so that there is a power layer between analogue and digital.

Unfortunately, my EDA software (KiCAD) does not permit to reorder the stack.

This is why I'm wondering if it would be possible to simply rename the two Gerber files before sending them to the producer, so that the layers get swaped?

My guess is that the layers are only connected through vias and PTH's for THT components. Am I missing something here, that might break the PCB, if I manually rename the files ?

  • 8
    \$\begingroup\$ When you look to changing the layer order I would strongly suggest that you consider swapping the bottom GND and the inner layer 1. The GND is a far better reference plane for your analogue signals than an inner power plane which is often broken up into multiple zones for various power rails. \$\endgroup\$ Commented Feb 2, 2018 at 19:45
  • 4
    \$\begingroup\$ @MichaelKaras also, burying the signal layer like that makes it a great deal harder to: test, troubleshot, and modify. Probably mandates excessive vias too. \$\endgroup\$ Commented Feb 2, 2018 at 20:28
  • \$\begingroup\$ @BrockAdams - My suggestion was to not bury a signal layer and instead move the GND plane in its place!! So your comment should probably have been addressed to the OP. \$\endgroup\$ Commented Feb 3, 2018 at 0:15
  • \$\begingroup\$ @MichaelKaras Thank you for the suggestion. Actually I'm using the large area GND layer as a heatsink for H-bridges. This is the reason why I placed the GND plane to an outer layer, hoping, that it would dissipate more heat to environment that way.. \$\endgroup\$
    – Fry
    Commented Feb 7, 2018 at 11:00
  • \$\begingroup\$ Note that you cannot realistically move a layer between the inside and outside via a file rename; interior and exterior features are typically different geometrically. \$\endgroup\$ Commented Sep 1, 2018 at 16:38

4 Answers 4


The Gerber files do not specify the order of layers. As long as you don't use blind or buried vias, the layers can be stacked in any order.

The file names for the individual Gerber files may vary between different CAD systems, and may or may not imply the desired stack-up order.

I always included a "readme" file with my PCB order specifying the desired stack-up order.


If you want to swap the layers directly in KiCAD, the option you need is Edit -> Swap layers.

After swapping the layer contents, you can update the layer names in Design rules -> Layer setup.


To make sure that you didn't make mistake, install an external Gerber file viewer (not connected to or produced by KiCAD). Then, after renaming, view the project in this viewer and imagine what others would see. Assuming you corrected the vias accordingly, yes, you can rename the files the way you want in order to change the layer.

  • 3
    \$\begingroup\$ +1 Good advice in general. This will pick up not only human errors but errors in the EDA software itself. One example of this that I have personally experienced is that OrCAD 16.6 has a very nasty bug with regard to "R" codes. This error didn't show up in OrCAD but Kicad's gerber viewer showed it clear as day. Had we gone straight to manufacture we'd have blown up a $70 BGA! It's a great feeling to find a mistake before you have to spend real money fixing it. \$\endgroup\$
    – user98663
    Commented Feb 2, 2018 at 19:56

I go one further than Peter in the other answer and include both a "ReadMe.Txt" file and a FAB drawing with each PCB order. The FAB drawing is very detailed and includes information related to stackup, board dimensions, fabrication notes including solder mask and silkscreen ink colors and any special requirements for:

  1. Breakaways
  2. Bare board testing requirements
  3. Non-plated hole locations and dimensions
  4. Dielectric thickness specifications between layers.

Do note that you have to be careful what vendors that you order your first boards from. Some prototype PCB houses think they do not have to look at your FAB drawing and will try to build your PCBs to some standard recipe and you will end up with something different than you expect. I have had first hand experience with this from at least one USA prototype PCB vendor that refused to look at the FAB and made boards that were totally useless. I have had very good luck with using vendors in China that followed my FAB and made exactly what I wanted.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.