HOPE: Moving to KiCad Layout

Now to get to the real meat of designing PCBs: board layout.


The first step in taking you schematic to the physical realm is to match each component to a corresponding footprint. Footprints are a physical representation of an electrical component on an PCB, like a footprint that the component makes on the board. Many footprints can correspond to a single schematic symbol exactly because many different components can correspond to a single schematic symbol. Think about it, how many different kinds of resistors are there? They all share the same squiggle symbol, but are of all different kinds of shapes and sizes.

Note: An important characteristic of this symbol-to-physical conversion process is knowing what parts to use comes first. Your circuit's components must be specified before you can move on to layout. We won't cover how to choose which part to use here, but will come back to this topic later.

Footprint assignment is done in the schematic editor. You can see that the tool icon for it is a combination of the KiCad icon for part symbols and that for footprints.

Assign footprints tool icon

The Assign Footprints window is notoriously bad at being clear on what things do. The basic process is to filter and search for the footprint you want by library, number of pins, by filters the symbol has specified, or by keywords.

Footprint assignment walkthrough.
"Assign footprints" window
  • A This is the list of symbols in your schematic, and their assigned footprint if they have one. If you want to assign multiple components with the same footprint, select multiple components using SHIFT-select.

  • B This is the component library window, listing all footprint libraries associated with your current project. Just like symbol libraries, the standard footprint libraries for KiCad are also organized by some kind of relation. For example, for components C1 and C2, you would probably choose either libraries "Capacitor_SMD" (surface-mount capacitors) or "Capacitor_THT" (through-hole capacitors). You can filter your footprint search by library.

  • C These are your footprint search filters. Enable/disable filters: library ("L"), number of pins ("#"), from symbol (the paper looking one), and search by keyword.

  • D These are the footprints that have passed through your search filters. Make sure to double-click the footprint in the right panel to assign it.

  • E Preview selected footprints.


Now that all the components have been given a physical representation, it is now safe to move on the other half of KiCad and start actually making a board. There are a couple of ways to move the schematic to layout, but any method you choose will involve 2 steps:

  1. opening the layout editor Pcbnew GitHub Logo
  2. updating the layout from the schematic

Here is one way to do it straight from the schematic editor in one click:

Update PCB from Schematic

If a PCB layout file for your project has not yet been created, you will be prompted by KiCad for confirmation of creating the file.

Layout files DNX prompt

This is KiCad's layout editor:

Visually, it is very similar to the schematic editor, with the most notable changes being that the background of the main work pane is black, and the addition of a new side panel on the right. We'll discuss the most important tools in a moment..

Updating from the schematic should bring up this popup. For first time updates, none of the additional options on the top will matter, but for iterative updates, these options will define how KiCad may deal with potential conflicting changes from the schematic or additional cleanup of the layout.

Update PCB from Schematic prompt

When there are new parts to be added to the layout from the schematic (such as in the first update from schematic), "Update PCB" will add in the new footprints to the layout, and put you immediately into block placement mode.

Block manipulation works just the same as it does in the schematic editor. In fact, much of the general feel and interaction (i.e. selection, component manipulation, properties, shorcuts, etc.) in the layout editor is very similar or identical to the that of the schematic editor.

ECAD Basic Terminology

  • plated through hole (PTH): a hole through the board that is plated with a conductive material. Can carry connections between copper layers in a PCB.
  • pad: a block of copper or a PTH associated with a part's pin
  • track: a strip of copper, usually electrically connecting two or more pads of the same net together
  • pour: a "pool" or large shape (pour) of copper, typically associated with some net

ECAD Layout Core ideas:

  1. Everything is built on a grid (again): Just like the schematic, the layout is also built on a grid system. However, this time the grid size translates directly to real-life dimensions, so...
  2. Using the proper grid size and units is essential: There are two parts to this:
    1. Units on the grid matter, as if the grid dictates that two wires are 10mm away from each other, then when you get that board manufactured, those two wires will be 10mm away from each other. There are two different units used by KiCad (and most other PCB ECADs):
      • mil: thousandths of an inch
      • mm: millimeters
    2. You will most likely need to change the grid size. For example, lining up two big parts may be easier with a big grid, but drawing tiny wires next to each other may be easier on a small grid. Changing the grid does not affect the component footprints in any way; it only changes at what refinement of a layout they can snap to.
  3. Footprints are directly correlated to the physical part: As stated above, footprints represent real parts, but unlike symbols, are not abstractions of them! Physicality of the part is partially represented by the footprint.
  4. Connections in layout are made with copper: Any of the tools in the layout editor that make connections, is either copper or some other conductive-element.
  5. Layout layers correlate to physical board layers: Unlike the schematic, in the board layout, connections between components cannot cross over each other, but instead can actually be made through multiple layers instead. This is because, once again, when performing layout, you are now designing around the physical aspect of real board.
  6. The schematic-generated netlist is determines the ratsnest: The netlist basically says that two pads (pins in the schematic) must be connected. How they are connected, is your job as the PCB engineer. The ECAD program will assist you by showing ratsnest lines that indicate which pads need to be connected together with copper in the layout.
Layout walkthrough.

Using KiCad's layout editor


As already mentioned, manipulation and working with selection blocks is exactly the same as in the schematic editor! One important aspect of this in the layout editor though is: selection also follows the grid. This means a smaller grid size will allow for finer selection.

This also applies to the schematic editor actually, but since the grid should not really be changed in the schematic editor, it's unlikely that you'll use this fact there


The following is a short list of some of the tools you will likely use the most during layout, found on the left hand toolbar. As always, you can find more info about these and the other tools in the KiCad manual.

Highlight net selected by clicking on a track or pad.

Display local ratsnest (Pad or Footprint).

Placement of tracks.

Placement of vias

Placement of zones (copper planes).

Draw Lines on technical layers (i.e. not a copper layer).

Delete element pointed to by the cursor

Note: When Deleting, if several superimposed elements are pointed to, priority is given to the smallest (in the decreasing set of priorities tracks, text, footprint). The function "Undelete" of the upper toolbar allows the cancellation of the last item deleted.

The image below is of an example completed board layout for the first lab board.

The red lines in the layout are called tracks or traces. They represent the physical connections defined by the connections made in the schematic doc.

Similarly, the red polygonal shapes are called fills, and represent large spans of copper that are also a way to represent wires in the schematic (usually power related wires).

The turquoise lines denote the silkscreen, which will be explained a bit more in depth in a later article. Basically, they are the white text you see on PCBs and are useful for assembly and verification purposes, among other things.

Example Final Routing