Disclaimer: Screenshots taken from version 5.1.4
KiCad determines which symbol belongs to which footprint via the footprint field of the symbol. This symbol field can be set either already in the library (fully specified symbol) or sometime during the schematic design process. This tutorial lists all options you have to assign a footprint to your symbols.
At schematic design time
This workflow is less work for library maintenance and allows for selecting exact components late in the design process.
Using the assign footprints tool (In the past known as CvPcb).
Found in eeschema: Tools->assign footprints to components (Might be called differently in your version of kicad.)
This tool allows you to edit the footprint field of all your components in a tabular form.
If you want to assign a footprint to a component, select this component in the middle column and click on the desired footprint in the right column. What is shown in the right column is determined by the filter settings.
Filters of the assign footprints tool
Only footprints that fulfil all footprint filters with respect to the currently selected target symbol are shown in the rightmost column. There are 4 filters available.
- Filter by the symbols footprint filter(s) uses the filters set in the footprint properties within the library (see below).
- Filter by pin count shows only footprints that have the same number of pads as the symbol has pins. (There is no check if the identifiers agree. Duplicated pin numbers or pad numbers are not counted)
- Filter by selected library uses the library selected in the leftmost column of the tool
- The manual filter uses the same syntax as the symbols footprint filter (see below)
Activate previews in the assign footprints tool
It is possible to have a preview of both the footprint and it’s assigned 3d model. The preview windows are separate and can be placed anywhere on your screen.
They will loose focus (get pushed to the back) as soon as you select a new footprint. So place them somewhere outside the space taken up by cvpcb for easy usage.
Setting the footprint for a single placed symbol in its properties dialog (footprint browser)
Hover your mouse above the symbol you want to assign a footprint and press e to reach the symbol properties dialog (or right click -> properties -> edit properties).
This dialog allows filling out the footprint field for the active symbol. Click in the text input area of the footprint field to get a button that allows opening the footprint browser. You can also manually enter the footprint reference into this field (Syntax: <library nickname>:<footprint name>)
In the footprint browser you need to select the footprint lib in the leftmost column and the footprint in the middle column. (Single clicking updates the preview, double clicking assigns the footprint.)
The symbol field editor of eeschema (footprint browser)
Version 5 introduced the footprint field editor. It allows to edit all fields of all placed symbols in a tabular view. This includes the footprint field. It is found in tools -> edit symbol fields.
You can assign the same footprint to multiple symbols by making use of the grouping options. The same footprint browser shown in the previous section can be reached by using the button that shows in the footprint field when you click on it.
In KiCad v5 (or nightly), directly in the component selector.
KiCad v5 has an experimental feature to allow footprint preview and selection when browsing symbols. It must be enabled:
- Open Preferences → General Options.
- On the Display tab, enable “Footprint previews in symbol chooser (experimental)”.
The feature should be considered in “beta”, as performance is a bit poor and a few features are still missing, but what is there should work.
In this selection dialog the following options are available:
- By default the footprint set in the symbols footprint field is selected.
- The option “Other…” opens the footprint browser.
- In addition to the default footprint, all footprints that result from the footprint filter defined in the symbol are shown as well.
Specified in the library
This workflow is a bit more work on the library side and requires you to select the exact component while selecting the symbol. (You can exchange the symbol later on and could even use the same tools as with the previous workflow to overwrite the library settings.)
Setting the default footprint for symbols. (Library editor)
More detailed description in the https://forum.kicad.info/t/tutorial-how-to-make-a-symbol/13336
You can setup your lib such that your symbols have their footprint pre assigned. This is called a fully defined symbol. (This footprint will be automatically assigned in KiCad v4. In KiCad v5 you can change the assignment using the new symbol selector dialog.)
Setting footprint filters for symbols. (Library editor)
The footprint filters are used in CvPcb if you set the filter that way. (see above)
They are also used in the KiCad v5 symbol selector dialog to show alternative footprints.
Footprint filters can include wildcards:
- ?: Exactly 1 character (1)
- *: Any number of characters (0…n)