Back on our kicad_schematic_entry page we talked about placing symbols, wiring them up, annotating reference designators, and so on. The next step is mapping each component symbol on the schematic to a footprint that will be positioned on the circuit board. Remember, symbols are just the abstract idea on the schematic, while footprints are the physical holes and copper pads that we solder to on the board.
Assign PCB footprints
There's an important dialog for this: The “Assign PCB Footprints to Schematic Symbols” tool. (toolbar or menu TODO picture)
Remember from the video there are three filter-control buttons on the toolbar
of “Assign Footprints” Select the “#” (match number of pins) and “L”
(match library) filters
Our connectors, J1 through J4, are generic symbols - they aren't associated with an actual connector that we can buy or place on a board. Take a moment to notice where J1 through J4 are located on the schematic. If you used the defaults for “annotate”, J1 should be on the left, J2, J3, and J4 on the right.
For the connector on the left, we want a female or socket type that lays down against the board. Look in the Connector_PinSocket_2.54mm library, and select the footprint “PinSocket_1x03_P2.54mm_Horizontal” for J1.
Next go to the Connector_PinHeader_2.54mm library. Of the three on the right, set J2 to PinHeader_1x03_P2.54mm_Horizontal. For the remaining two on the right, J3 and J4, use PinHeader_1x03_P2.54mm_Vertical.
Set the footprint for both LEDs to “LED_D5.0mm”, found in the LED_THT library.
For all of the resistors, use the Resistor_THT library. Set the footprint for R1 and R2 to R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal
When you're done, the dialog should look like:
After doing the assign footprints, don't forget to save!
Create Netlist
Push the green Create Netlist (“Net”) button, and accept the default name. that's it! you should be able open up the pcb editor, hit “read netlist”, and see all of your parts - but that's getting ahead.
Continue with the kicad pcb layout page.