Altium Designer Documentation

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

Created: July 27, 2015 | Updated: January 17, 2017
現在、バージョン 17.0 をご覧頂いています。 最新情報については、バージョン 21 の をご覧ください。

Parent page: Schematic Objects

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


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.


Pins can only be placed in the Schematic Library Editor. Use one of the following methods to place a pin:

  • Click Place » Pin from the main menus.
  • Click (Place Pin button) on the Utility Tools drop-down of the Utilities toolbar ().
  • Click the Add button in the Pin List section of the SCH Library panel.
  • Click the Add button in the Component Pin Editor dialog (accessed by clicking the Edit Pins button in the Library Component Properties dialog)


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 the pin is held by.
  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 access an associated properties dialog, from where properties for the pin can be changed on-the-fly.
  • 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 counter-clockwise 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 respectively.
While attributes can be modified during placement (Tab to bring up associated properties dialog), keep in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Create the Library component near the origin (center) of the Library Editor sheet, which is marked by dark cross-hair lines. Typically a pin or the corner of the component body is placed at the sheet origin.

The pin number (Designator) must be defined as this is what is used to establish the connectivity. The Electrical Type is also important as this is used in the Schematic Editor for the Electrical Rules Check (ERC).

Adding Pins in the Component Pin Editor

Pins can also be added through the Component Pin Editor dialog, which is accessed via the Edit Pins button in the Library Component Properties dialog.

Access the Library Component Properties dialog by clicking Tools » Component Properties. Alternatively, double-click the entry for the component in the Components region of the SCH Library panel or select the entry and click the Edit button.

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. When you click OK to close the dialog, the new pin(s) are placed on the sheet to the bottom right of the component, ready to be positioned.

Notes on Pin Numbering

For many components there will be a series of pins that have numerical names and numbers. The auto-increment feature 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 settings on the Schematic - General page of the Preferences dialog.

 Enter the Display Name and Designator pin properties.

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

Use the auto-increment feature to speed the placement of pins.

Graphical Editing

To move a pin, click and hold on it - 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 respectively).

If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic – Graphical Editing page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double-click on the locked object directly and disable the Locked property or disable the Protect Locked Objects option to graphically edit the object.

Non-Graphical Editing

Via an Associated Properties Dialog

Dialog page: Pin Properties

This method of editing uses the Pin Properties dialog to modify the properties of a pin object.

The Pin Properties dialog

The Pin Properties dialog can be accessed prior to entering placement mode, from the Schematic – Default Primitives page of the Preferences dialog. This allows the default properties for the pin object to be changed, which will be applied when placing subsequent pins.

During placement, the dialog can be accessed by pressing the Tab key.

After placement, the dialog can be accessed in one of the following ways:

  • Double-click on the placed pin object.
  • Place the cursor over the pin object, right-click then choose Properties from the context menu.
  • Click Edit » Change from the main menus then click once over the placed pin object.

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.

The font used for the pin Display Name and pin Designator (number) - for a component placed on a schematic sheet - is defined at the document level in the Document Options dialog. Click the Change System Font button to set it.

The default system font for a schematic library document is Times New Roman, 10pt, Regular. This is fixed and cannot be changed. When a library component is placed on a schematic sheet, this same default font is applied, but is not fixed, and can be changed as required. Keep in mind that the system font used for a schematic sheet applies to other objects as well, including Power Ports, Ports, and the X, Y region markers in the schematic sheet border.

For pins, these system-level settings of position and font can be overridden locally. Controls for customization of the position and font for a pin's Name and Designator can be found on the Logical tab of the Pin Properties dialog when editing a pin in either the Schematic Library or Schematic Editor. While the controls themselves are the same for both attributes, separate sets of controls allow them to be customized independently of each other.

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

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

The preview window updates dynamically as you make changes in order for you to immediately see the effects of your changes without closing the dialog.

Example customized positions for pin Display Name and Designator.

Use the Use local font setting option to change from following the default system font, to an overriding, customized font. To do so, simply click on the font control to the right of the option to access the standard Font dialog. The control doubles as a notification for the font currently chosen, or 'in-force'.

Example customization of the font for a pin's Display Name.

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 property - available in the Symbols region of the Pin Properties dialog - to determine the width of the line used to draw these symbols. Choose from either Small or Smallest.

Use Line Width to choose Small or Smallest Pin symbol line width.

Via an Inspector Panel

Panel pages: SCHLIB Inspector, SCHLIB Filter

An Inspector panel enables the user to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with appropriate filtering - by using the applicable Filter panel or the Find Similar Objects dialog - the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

Via a List Panel

Panel pages: SCHLIB List, SCHLIB Filter

List panel allows the user 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 the designer to target and edit multiple design objects with greater accuracy and efficiency.

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.



We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: