PCB layout - Mechanical Keyboard

Now you move from the logical schematic to the physical board. Go back to the KiCAD project window and open the PCB Editor.

#Import from the schematic

In the PCB Editor, go to Tools → Update PCB from Schematic (or press F8).
Click Update PCB. All your components will appear as a pile in the center of the screen.
It will look messy at first. That's normal.

#Board outline

#Draw the outline on Edge.Cuts

Before placing components, draw the outer edge of your PCB on the Edge.Cuts layer.
In the right panel, select the Edge.Cuts layer.
Use the Draw Rectangle tool (or Draw Line for custom shapes) to draw the outline of your board.
A standard 60% keyboard is roughly 285mm × 95mm, but size it to fit your layout.

#Placing components

#Place the Pico first, then switches

Start by placing the Pico, then build out from there.
Click and drag components into position. Use R to rotate.
Place the Pico at one edge of the board so its USB-C port hangs slightly off the PCB. This makes it easier to plug in a cable.
Place switches according to your layout. Use a consistent spacing. MX switches use a 19.05mm grid.
Place stabilizers directly under their corresponding wide keys.
Place diodes near their switches, typically just below or above each one.
You can use whatever spacing works for you, just keep it consistent.

#Renumber by position

If you copy-pasted footprints, their reference numbers may be out of order. Use Geographical Reannotate to renumber them by their physical position on the board:
Go to Tools → Geographical Reannotate.
Choose your preferred order (left-to-right, top-to-bottom).
Click OK. The references update to match position, and KiCAD will sync this back to your schematic.

#Routing traces

Routing is the process of drawing the copper traces (wires) that connect all the pads together. The thin "ratsnest" lines show you which pads still need to be connected.

#Route the matrix

Press X to activate the Route Track tool.
Click a pad to start a trace, then click the destination pad to complete the connection.
Use the F.Cu layer (front copper) for traces going in one direction and B.Cu (back copper) for the other direction. This keeps things organized and avoids most crossings.
Press / to switch between front and back copper mid-trace (this adds a via, a small hole that connects the two layers).

Full wiring Pico routing General routing

The USB port of the Pico should hang off the PCB edge slightly so a cable can plug in:

USB overhang

#Ground fill (optional)

A ground fill floods any empty copper area on the board with a solid GND connection. It's optional but good practice.

#Add filled zones on both layers

Select the F.Cu layer.
Go to Place → Add Rule Area or use the Add Filled Zone tool.
Draw a rectangle covering your entire board outline.
In the dialog, set the net to GND and click OK.
Press B to fill all zones.
Repeat on B.Cu.

#3D preview

You can attach 3D models to footprints to visualize what your board will look like. Many footprints already include a model. For others (like the Pico), download a STEP file from GrabCAD and link it in the footprint properties.

To view your board in 3D, press Alt+3 or go to View → 3D Viewer.

3D preview

#DRC

#Run the design rule check

Before exporting, run a DRC to catch any mistakes:
Go to Inspect → Design Rules Checker.
Click Run DRC.
Review any errors. Common ones are unconnected pads (ratsnest lines you missed) or traces that are too close together.
Fix all errors before exporting.

#Exporting gerbers

Now that the PCB is finished, it's time to get it fabricated. Gerber files are the production files you send to a PCB manufacturer.

#Export fabrication outputs

Save your PCB, then go to File → Fabrication Outputs → Gerbers (.gbr) and export everything in that dialog.
If you want a known-good starting point, here are the exact settings to use.

Include these layers:

F.Cu, B.Cu, F.Paste, B.Paste, F.Silkscreen, B.Silkscreen, F.Mask, B.Mask, Edge.Cuts

General options:

Option	Setting
Plot drawing sheet	off
Subtract soldermask from silkscreen	off
Indicate DNP on fabrication layers	on, set to Cross-out
Sketch pads on fabrication layers	off
Check zone fills before plotting	on
Drill marks	None
Scaling	1:1
Plot mode	Filled

Gerber options:

Option	Setting
Use Protel filename extensions	off
Generate Gerber job file	on
Use extended X2 format (recommended)	on
Include netlist attributes	on
Disable aperture macros	off
Coordinate format	4.6, unit mm

#Plot and zip

Once your settings match, click Plot to generate the Gerbers.
Then click Generate Drill Files and click Generate Drill File to export the .drl file.
Finally, zip the entire output folder. That zip is what you send to the manufacturer, and you should commit it to your project alongside your bom.csv and KiCad project files.

#StepImport from the schematic

#Board outline

#StepDraw the outline on Edge.Cuts

#Placing components

#StepPlace the Pico first, then switches

#StepRenumber by position