kicad-source/pcbnew/dialogs/panel_setup_rules_help_8expression_functions.md

### Expression functions

All function parameters support simple wildcards (`*` and `?`).


    A.enclosedByArea('<zone_name>')
        True if all of `A` lies within the given zone's outline.

        NB: this is potentially a more expensive call than `intersectsArea()`.
        Use `intersectsArea()` where possible.


    A.existsOnLayer('<layer_name>')
        True if `A` exists on the given layer.  The layer name can be
        either the name assigned in Board Setup > Board Editor Layers or
        the canonical name (ie: `F.Cu`).

        NB: this returns true if `A` is on the given layer, independently
        of whether or not the rule is being evaluated for that layer.
        For the latter use a `(layer "layer_name")` clause in the rule.


    A.fromTo('x', 'y')
        True if the object exists on the copper path between the given
        pads. `x` and `y` are the full names of pads in the design, such as
        `R1-Pad1`.


    A.getField('<field_name>')
        The value of the given field. Only footprints have fields, so a field is only returned if
        `A` is a footprint.


    A.hasComponentClass('<component_class_name>')
        True if the set of component classes assigned to `A` contains the named
        component class.


    A.hasNetclass('<netclass_name>')
        True if `A` has had the given netclass assigned to it, either by an explicit netclass label
        or through a pattern match assignment.


    A.inDiffPair('<net_name>')
        True if `A` has a net that is part of the specified differential pair.
        `<net_name>` is the base name of the differential pair.
        For example, `inDiffPair('/CLK')` matches items in the `/CLK_P` and `/CLK_N` nets.


    A.intersectsArea('<zone_name>')
        True if any part of `A` lies within the given zone's outline.


    A.intersectsCourtyard('<footprint_identifier>')
        True if any part of `A` lies within the given footprint's principal courtyard.


    A.intersectsFrontCourtyard('<footprint_identifier>')
        True if any part of `A` lies within the given footprint's front courtyard.


    A.intersectsBackCourtyard('<footprint_identifier>')
        True if any part of `A` lies within the given footprint's back courtyard.


The `footprint_identifier` listed above can be one of the following:

1. A reference designator, possibly containing wildcards `*` and `?`
2. A footprint library identifier such as `LibName:FootprintName`. In this case,
   the library identifier must contain the `:` character to separate the library
   name from the footprint name, and either name may contain wildcards.
3. A component class, in the form `${Class:ClassName}`.  The keyword `Class` is not
   case-sensitive, but component class names are case-sensitive.



    A.isBlindBuriedVia()
        True if `A` is a blind/buried via.


    AB.isCoupledDiffPair()
        True if `A` and `B` are members of the same diff pair.


    A.isMicroVia()
        True if `A` is a microvia.


    A.isPlated()
        True if `A` has a hole which is plated.


    A.memberOfGroup('<group_name>')
        True if `A` is a member of the given group
        The name can contain wildcards.
        Includes nested membership.


    A.memberOfFootprint('<footprint_identifier>')
        True if `A` is a member of a given footprint
        (for example, a pad or graphic shape defined inside that footprint).
        The various ways of specifying `footprint_identifier` are described above.


    A.memberOfSheet('<sheet_path>')
        True if `A` is a member of the given schematic sheet.
        The sheet path can contain wildcards.


    A.memberOfSheetOrChildren('<sheet_path>')
        True if `A` is a member of the given schematic sheet, or any of its child hierarchical sheets.
        The sheet path can contain wildcards.