Pin | Online Documentation for Altium Products

Old Content - visit altium.com/documentation

Modified by Admin on Nov 6, 2013

Parent page: 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. Use one of the following methods to place a pin:

Choose Place » Pin [P, P] from the Schematic Library Editor main menu.
Click the 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 via the Library Component Properties dialog)

Placement

New pins are added to the component that is currently visible in the Schematic Library Editor, select the required component in the SCH Library panel.

Using one of the first 3 techniques described above, invoke the pin placement process. 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, and it is always this end the pin is held by.
Since there is often numerous pins on a component, it is more efficient to edit the properties of each pin as they are being placed. To do this, press Tab while the pin is floating on the cursor.
Edit the pin properties as required, typically this will include at least the Display Name, Designator and Electrical Type (refer to the image of the Pin Properties dialog shown down the page). Note that you can move between these fields using the Tab key to step forward, or Shift+Tab keys to step backward. You can also accept the dialog settings by pressing the Enter key on the keyboard, making it possible to define the dialog settings without touching the mouse.
Press the Spacebar rotate the pin if required. Rotation is anti-clockwise in steps of 90 degrees.
Position the pin, then click or press Enter to place the pin in the Library Editor workspace.
Continue to place pins, or press right-click or Esc to terminate pin placement.

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.

If the display pans rapidly as you move the floating pin around use the Z, A shortcut keys to re-center the component on the screen.

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 in the Component Pin Editor dialog, which is accessed via the Edit Pins button in the Library Component Properties dialog.

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 Component Pin Editor dialog. Note that multiple pins can be added and their properties 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 incrementing alpha and numeric values, and decrementing numeric values.

Configure the Auto-increment settings in the Schematic - General page of the Preferences dialog.

Enter the Display Name and Designator pin properties.

Note the incrementing alpha pin name and decrementing numeric pin number.

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

Non-Graphical Editing...

The following methods of non-graphical editing are available:

...via an Associated Properties Dialog

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

Edit the properties of the Pin in the 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-clicking on the placed pin object.
Placing the cursor over the pin object, right-clicking and choosing Properties from the context menu.
Using the Edit»Change command and clicking once over the placed pin object.

Pin Name and Designator Position and Font

The location of the pin Name and pin Designator (number) is defined globally by the Pin Margin settings in 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 Name and pin Designator (number) is defined at the document level in the Document Options dialog, click the Change System Font button to set it. Note that as well as the Pin Name and Pin Number, the text strings for a number of other objects are also classified as System Fonts, including: Power Ports, Ports, Off Sheet Connectors 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, using the Position and Font settings in the Pin Properties dialog. The image below shows how both the pin Name and Number have been rotated on a vertical pin.

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

...via an Inspector Panel

An Inspector panel enables the designer to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with appropriate filtering, the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

...via a List Panel

A List panel allows the designer to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. When used in conjunction with a Filter panel, 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.

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.

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.