pin for Symbols

The pin statement in the pcb-symbol context is used to define the connection points of a schematic symbol.

Signature

; Point Form
pin <Ref> at <Point>

; Annotated Line Form
pin <Ref> at <Point> with:
  direction = <Dir>
  length = <Double>
  number-size = <Double|False>
  name-size = <Double|False>
  • &lt;Ref> - Name of the pin that will be constructed.
    • The Ref can be a standard identifier like VIN or it can be an indexed reference like D[1], D[2], etc.
  • &lt;Point> - An instance of type Point.

Usage

The pin statement is used to define the connection points on a schematic symbol. There are two forms for the pin connections:

  1. Point Form - In this form, the connection point does not have a line associated with it.
    1. Further, the name and pad number are hidden by default.
    2. This can be useful for constructing symbols where a line might get in the way or prevent the formation of geometry in the preferred way.
  2. Annotated Line Form - In this form, the connection point has a line associated with it by default.

Annotated Line Form

Here is an example pin statement in annotated line form: 

  pin VIN at Point(0.0, 0.0) with: 
    direction = Left
    length = 3.0
    name-size = 0.85
    number-size = 0.85

Here is rendering of the anatomy of a symbol pin:

Symbol Pin Anatomy

In this view:

  1. The text p[0] is the pad ref - this is what pad/hole on the component landpattern that this pin maps to.
  2. The text VIN is the pin ref - this is the name of this pin in the circuit and as shown on the schematic.
  3. This pin has a direction that points to the left.
    1. Notice that the symbol body is on the right and that the pin's direction is direction it points out from the symbol body.
  4. The red X at the tip of the pin is the connection point where schematic wires will be drawn to/from.

Optional Pad and Pin Ref Text

In the annotated line form, you can optionally drop the name-size and number-size parameters from the pin statement. This will cause the pin ref and/or pad ref to be hidden by default: 

  pin VIN at Point(0.0, 0.0) with:
    direction = Left
    length = 3.0
    number-size = 0.85

In this case, the pin would be shown as:

Hidden Pad/Pin Ref

This is useful for constructing more idiomatic schematic symbols where the pin name is not typically shown - for example, in an op amp symbol:

Opamp Symbol Pin