How to check if 2 PCBs will fit together

Hallo there,

I am realy new to KiCad and love it. I am drawing my first simple circuits but need it to be a stacked 2 pcb board. I read the threads on how handle multi PCB projects in KiCad in general so no need for help on this. Will use 2 seperate projects. What I like to know ist how I can be sure if my 2 boards will fit together in the end. Especially the socket / header connection should be exact. What is the best way to check this?

Bring them both into FreeCAD using the StepUp FreeCAD plugin, perhaps?


As you have 2 independent pcbs, make sure the connectors are at the same distances.
I usually make a footprint with the contour and connectors of the daughter pcb and add it to the mother board.


You can Avoid using FreeCAD (though I do recommend learning it) to do what you want…

In Kicad:
• Make PCB#1 (with desired connectors/etc)
• Make PCB#2 (with desired connectors/etc)

Export PCB#2 as STEP.
Make a Footprint with that STEP

Now, in PCB#1, load the newly made Footprint and mate it to PCB#1.

Several ways to do this sort of thing

Look at my Posts in this link where I posted similar here


For design made of 4 stacked PCBs I have first done the KiCAD project containing only PCB file but without PCB itself. I have there only drawings of case (it is intended for flush-mounted electrical box so some PCBs are round and front with keyboard is square). Except case drawing I also marked there positions of all connections between stacked PCBs and also LED and key positions.
Then each od that project PCB I start from copying that empty project under the new name. The graphic layer I make visible only when I draw the PCB Edge.Cuts and position the footprints that need to be correlated between PCBs or with case itself. When it is done I hide graphic layer I used for that.

1 Like

I assume this is a simple design, in which both connectors have the same foorptins, just as for example in the good old PC104. For such a project I would work with a template.

In KiCad you can export any project as a template, and later you can use the template to start new projects. In such a template you can put anything that is as in any other KiCad project, such as a PCB outline, connectors and their locations, a partial schematic.

You can also combine the essential parts inside the template in a block so they do not move relative to each other. Although, if you have a male connector on the top of one PCB, then you probably want a female connector on the bottom of the other PCB. Parts inside a block can be changed, but I do not have much experience with that. Parts with essential locations are also much easier to manage if they are on a coarse grid with nice round coordinate numbers. That way they either fit perfectly, or are so far off it’s obvious.

You can also use: PCB Editor / File / Export / SVG and then PCB Editor / File / Import Graphics / SVG in the other project to check if things can still be lined up. Although aligning the graphics with the project is a bit cumbersome, but it’s doable.


Hi @bcppcb

You could always use the simple copy/paste.

Draw your edge cuts, position your connectors and any other critical footprints in one project (board).
Create the second project (board).
Select and copy the first board.
Paste it into the second board.

As a final check when both boards are complete, copy one and hold it over the other to check alignment of footprints requiring connection between boards.


I use a different way:

  • I put the base point on both pcb in the same place (e.g. pin 1 of the connector that is to go to its counterpart on the second pcb),
  • I generate gerber files of both pbc,
  • I open gerber files of both pcb in gerber viewer.

I think this is the easiest way to check if everything fits.


Super thankful for all of the answers. I had no idea that there are so many good approaches for this task.
I have some experience with freecad so this should work for me. Simply generate gerber files for both and open it in gerber viewer sounds also handy.
The connectors will not have exactly the same footprint. On one side it will be through-hole socket on the other side it will be a smd header. But they should have visually some difference to align them properly.
I also like the svg or simply copy and paste approach. Will try all of them :). Thank you all!

I realized I also have to draw some holes in one of the pcbs to put some audio jacks through there which get screwed from the other side. How can I get sure that my holes are the right size for the thread of the jack. Datasheet says 6mm is the diameter of the outer thread. Does someone have experience on how much bigger the hole should be?

Use a Tap/Drill Chart… Here’s a link to one of many…

Find a chart for Metric if that’s what you want…

ADDED: Not all Charts will show Minimum Clearance diameters - that is primarily a Judgement call/dimension based on Materials and Form-Fit-Function needs.
The Chart (link posted) shows them but, you need to decide for yourself. Also, Shouldered Screws/Bolts are different so Consider that…

1 Like

Thanks, that helps. Will find myself a metric one…

Also: Mating the connectors together while soldering helps with making a proper alignment. Mating connectors can also help for reducing deformations when you let the plastic get too hot during soldering.

You mean I should use something like a 2x5 connection or similar depending on my needs instead of using single connections? My plan was to do so.

Print them both onto paper, put on on top of the other, then hold them up to the light!


Can you explain what “paper” is? My grandparents once told me something about that stuff but i’m not exactly sure what it is. I seem to recall they even killed trees to make it. How brute!

It is apparently also quite dangerous. If you let it accumulate in stacks, then you can get hypnotized by it and stare at it for hours at a time. :slight_smile:


Create a symbol and a footprint for the board-to-board connections.

1 Like

Low-tech, but should do this anyway regardless. Print them on A4/Letter paper (ensure you’re setup for the exact one you’re actually printing on), and then hold them together against a window (with backlight) to see if they line up.

It’s always helpful to have a printed view of the pads, holes, etc. to make sure you’ve got the right footprints. I normally don’t catch anything this way, but when I do, I’m always happy I caught it!

1 Like

The link to the printable charts has both imperial and metric:


1 Like

I’d say the fewer the connectors, the less likely you are to have alignment problems - ie one 6-pin connector rather than 6 1-pin connectors. But as suggested mate a pair before soldering as that holds all pins in perfect alignment should the heat from soldering soften the plastic.


1 Like

For what it is worth, I have access to a drawing package that acepts dxf files. PCB editor can create dxf files. Design your 2 PCBs. Choose which layers to create and make a dxf for both PCBs. I usually use bottom copper or Silk screen.

Open #1 PCB with the drawing package and put the dxf on a layer. Open a new drawing file and open #2 PCB. Copy #2 PCB with a reference point and paste it to #1PCB, not over the board. Change the colour and layer of #2 PCB then move it using a reference point to the same point on #1 PCB. The boards should line up perfectly. Either layer can be turned off if needed. Save the layers as a dwg file at each change.

This has the advantage that any metalwork or enclosure can also be added on another layer and drill points marked from the PCB directly. If the metalwork or enclosure is being sent for drilling, it can be done easily from the drawings of the metalwork layer only by turning off the PCB layers. Some CNC machine companies can use dxfs directly, but check first.