Up to ​KiCAD Notes

Let's use this schematic as an example:

Here are the essential steps to get to layout:

• Annotate the schematic
• Assign properties to all the symbols
• Assign Footprints (create missing footprints as needed)
• Create a Netlist
• Open PCB layout

Here are some details:

Annotate the Schematic

In principle this is easy. It changes all the references from e.g. C? to C3.

Menu Tools->Annotate Schematic in the schematic. Leave default settings (entire schematic, sort by X, keep existing, use first free number after 0). Click Annotate then Close.

Now your schematic should look like this:

Assign properties

For each symbol, you should set properties based on the ​BOM fields description.

The "value" property should be set:

• Set to the value for passives. For example "0.01uF" for capacitors and "1.2k" for resistors.
• For other parts, use the part number or a short descriptive name

The "Reference" property (e.g. C2) you should generally not edit.

Look up each part on a supplier website (​DigiKey is a good start). You will be given some guidance on this, but once you find a part, you can fill in the Mfg, MfgNo, Vendor and CatNo fields.

As one example, see the capacitor with DigiKey number M39014/01-1496-ND. You would set the properties as:

• CatNo = M39014/01-1496-ND
• Supplier = DigiKey
• MfgNo = M39014/01-1496
• Mfgr = Kyocera

You can do this spreadsheet-style using menu Tools->Edit Symbol Fields.

Assign Footprints

Menu Tools->Assign Footprints

This will give you a table with all your parts in the middle. The game here is to find a footprint for every part and assign it. It can be very challenging at the beginning to figure this out, but here are some hints:

• Resistors: Select either Resistor_SMT or Resistor_THT for surface-mount or thru-hole parts. Figure out the size and pick it from the library. It helps to have the datasheet drawing or an instance of the part in hand
• Capacitors: Select Capacitor_SMD or Capacitor_THT likewise, and figure it out from the dimensions.
• Integrated circuits: The datasheet may give you the name of a standard package (e.g. DIP-16 or SO-16) which you can find in the libraries.
• Connectors: Someone will have to tell you. One clue is that the very common "tenth inch" headers are in the library Connector_PinHeader_2.54mm library.

When you are done all the parts should have footprints, like so:

Create Netlist

Menu: Tools->Generate Netlist File. The defaults are fine. Click Generate Netlist and Save.

Open PCB layout

Menu: Tools->Open PCB Editor

Then in the PCB editor, menu Tools->Load Netlist and if necessary navigate and select the .net file. Click Update PCB and Close.

You should have a cluster of parts attached to the cursor. Click to put them down somewhere inside the frame.