Working with a Pin Object on a Schematic Library Sheet in Altium Designer

Parent page: Schematic Objects

The schematic Pin represents the physical component pin in the schematic design space.

Summary

A pin is an electrical design primitive. Pins give a component (part) its electrical properties and define the connection points on the part for the incoming and outgoing signals.

Availability

Pins can only be placed in the Schematic Library Editor using one of the following methods:

• Click Place » Pin from the main menus.
• Click  on drop-down of the Utilities toolbar ().
• Right-click then choose Place » Pin from the context menu.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter pin placement mode. Placement is made by performing the following sequence of actions:

1. Click or press Enter to anchor the pin. Note that the floating pin is held by the electrical end, which must be positioned away from the component body. Only one end of the pin is electrical; it is always this end that the pin is held.
2. Continue placing additional pins or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement – while the pin is still floating on the cursor, and before the electrical end of the pin is anchored – are:

• Press the Tab key to pause the placement and access the Pin mode of the Properties panel from where its properties can be changed on-the-fly. Click the workspace pause button overlay () to resume placement.
• Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement.
• Press the Spacebar to rotate the pin counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in increments of 90°.
• Press the X or Y keys to mirror the pin along the X-axis or Y-axis.

Adding Pins in the Component Pin Editor

Pins can also be added through the Component Pin Editor dialog, which is accessed by clicking the  button on the Pins tab of the Properties panel in Component mode.

Add one or more pins in the Component Pin Editor dialog.

Click the Add button to add a new pin, then define the properties in the dialog. Note that multiple pins can be added and defined. You can also use Tab and Shift+Tab to step between the fields. 

Notes on Pin Numbering

For many components there will be a series of pins that have numerical names and numbers. The Auto-Increment During Placement feature on the Schematic - General page of the Preferences dialog can be used to speed the placement of these pins. Auto-increment is invoked automatically if the pin properties are edited before placement (press Tab while the pin is floating on the cursor). The feature works for both the Designator and the Display Name - the pin Designator uses the Primary auto-increment field and the pin Display Name uses the Secondary auto-increment field. It supports ascending alpha and numeric values, and descending numeric values.

Configure the Auto-Increment During Placement settings on the Schematic - General page of the Preferences dialog.

Note the increasing alpha pin name and decreasing numeric pin number.

Graphical Editing

To move a pin, click and hold - the cursor will jump to the electrical hotspot end of the pin - then move it to the new location, placing it with the electrical end away from the component body.

While dragging, the pin can be rotated (Spacebar/Shift+Spacebar) or mirrored (X or Y keys to mirror along the X-axis or Y-axis).

Non-Graphical Editing

Pin Display Name and Designator - Position and Font

The location of the pin Display Name and pin Designator (number) is defined globally by the Pin Margin settings on the Schematic - General page of the Preferences dialog. This is an environment setting, meaning it applies for the PC where the setting is defined. The settings define a relative distance the text is away from the non-electrical end of the pin.

Set the distance of the pin text (Pin Margin) in the Preferences dialog.

For pins, these system-level settings of position and font can be overridden. Controls for customization of the position and font for a pin's Designator and Name can be found in the Pin mode of the Properties panel.

The font and location of the pin Designator (number) and Name can be modified for individual pins, if required.

Use the Custom Position option to change the default settings for the position to an overriding, customized position. For the Margin, enter a new value directly in the associated field. For the Orientation, use the drop-down to choose the angle (0° or 90°) and the To reference (Pin or Component).

Use the Custom Settings option to change from following the default system font to an overriding, customized font. 

Pin Symbol Line Width

When representing a component in the schematic editing domain, each pin defined as part of that device's schematic symbol can have one or more symbols displayed. These are symbols displayed on the Inside, Inside Edge, Outside, or Outside Edge in relation to the main component symbol outline, as required. Examples might include a Clock symbol on the Inside Edge, or a Dot symbol on the Outside Edge. Such symbols greatly improve the readability of the design through visual indication of the purpose of the signal traversing a particular pin.

Use the Line Width setting in the Symbols region of the Properties panel to specify the width of the line used to draw these symbols. Choose from either Small or Smallest.

Via a List Panel

Panel pages: SCHLIB List, SCHLIB Filter

A List panel allows you to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the applicable Filter panel or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing you to target and edit multiple design objects with greater accuracy and efficiency.