Going from Schematic to PCB Layout in KiCad (using Cvpcb)

NOTE: This tutorial was written in 1847, and kicad has changed a lot since then! Check out this awesome free kicad video series tutorial from Contextual Electronics for a more up-to-date version. They also have a small course on building your first pcb that includes everything from circuit board design in kicad to manufacturing the pcb.

 

This section will explain the process of going from the schematic to pcb layout in KiCad. The process is a little bit more involved than in Eagle, and requires 4 steps:

  • First, make sure all components are annotated (numbered).
  • Generate a netlist that contains all the components and their connections.
  • Use cvpcb to assign pcb footprints to all the components (not necessary if new components have not been added.)
  • Load the netlist in pcbnew.

Netlist Generation:

generating a netlist in kicad

Assuming your schematic is already annotated (numbered), click the "Netlist Generation" button.

generating a netlist in kicad

Just click the "Netlist" button unless you want to generate one for a different layout program or circuit simulator.

Assigning PCB Footprints to Components using Cvpcb:

run cvpcb in kicad

Now run Cvpcb.

cvpcb in kicadfiltered component list in cvpcb

Click the filter button to only show capacitor footprints.

assigning a module or footprint to a component

Double click on the footprint (module) to assign it to the schematic component.

Inspecting Footprints:

previewing modules in kicad's cvpcb

We'd like to use a cylindrical upright electrolytic cap for C2, but clicking the preview button reveals that none of the choices in the filtered list look right.

After clicking "display footprints list documentation", we can look through all of the built-in footprints and pick a better choice. Turn off the filtered list and choose C1V8.

Continue mapping the components, and then click Save to store the mappings in the netlist.

But wait, if it's saving with the same name (.net) that was used when eeschema made a netlist, won't it overwrite the original file?

When either eeschema or cvpcb saves a netlist, it doesn't overwrite a pre-existing netlist, but rather adds or changes info inside one.

before and after cvpcb saves a netlist

The above picture shows the netlist (.net) file before and after cvpcb maps the modules. There are "noname" placeholders that get filled in by footprints after cvpcb runs.

Loading components in Pcbnew:

run pcbnew to begin making the pcb layout

Now that modules have been assigned to the components, run Pcbnew to begin designing the circuit board.

read netlist in pcbnew

First, click the "read netlist" button.

click the read net list button to load components

Click the read netlist button to load components.

You'll do this same procedure when you make changes to the schematic:

  • annotate
  • write netlist (from eeschema)
  • run cvpcb (if new components were added)
  • read netlist (from pcbnew)
It's a little tedious, that's how the system works (to the best of my knowledge--add a comment if wrong!)

 

Some of the options when reading in a netlist can be dangerous. I'd recommend backing up your .brd layout file before reading from any netlists, as there's no undo in pcbnew yet.

Say, for instance, you've added screw holes that aren't in your schematic or netlist. If you check "Remove Extra Footprints" it will delete those screw holes when you read in the new list.

 

 

 

components loaded into pcbnew from netlist all on top of each other

 

 

<-Back                                                                                       Next->