Working with a Pad Object on a PCB in Altium Designer

Parent page: PCB Objects

Pads are used to provide both mechanical mounting and electrical connections to the component pins.

Summary

A pad is a primitive design object. Pads are used for fixing the component to the board and for creating the interconnection points from the component pins to the routing on the board. Pads can exist on a single layer, for example, as a Surface Mount Device pad, or they can be a three-dimensional through-hole pad, having a barrel-shaped body in the Z-plane (vertical) with a flat area on each (horizontal) copper layer. The barrel-shaped body of the pad is formed when the board is drilled and through-plated during fabrication. In the X and Y planes, pads can have a circular, rectangular, octagonal, or rounded rectangular shape. Pads can be used individually as free pads in a design, or more typically, they are used in the PCB Library editor, where they are incorporated with other primitives into component footprints.

Availability

Pads are available for placement in both the PCB and the PCB Library editors in one of the following ways:

• PCB Editor:
  • Choose Place » Pad from the main menus.
  • Click the Pad button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
  • Right-click in the design space then click Place » Pad from the context menu.
  • Click the  button on the Wiring toolbar.
• PCB Library Editor:
  • Choose Place » Pad from the main menus.
  • Click the Pad button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
  • Click the  button on the PCB Lib Placement toolbar.
  • Right-click in the design space then select Place » Pad from the context menu.

Placement

After launching the command, the cursor will change to a crosshair and you will enter pad placement mode.

1. Position the cursor then click or press Enter to place a pad.
2. Continue placing further pads or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement are:

• Press the Tab key to pause the placement and access the Pad mode of the Properties panel from where its properties can be changed on the fly. Click the 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. 

Graphical Editing

Pads cannot have their properties modified graphically other than their location.

• To move a free pad and also move the connected tracks, click, hold and move the pad. The connected routing will remain attached to the pad as it is moved.
• To move a free pad without moving the connected tracks in the PCB or PCB Library Editor, select the Edit » Move » Move command, then click, hold, and move the pad.

The following methods of non-graphical editing are available:

Via the Pad Dialog or Properties Panel

Properties page: Pad Properties

This method of editing uses the associated Pad dialog mode and Properties panel to modify the properties of a Pad object. 

  The Pad dialog on the left, and the Pad mode of the Properties panel, on the right

During placement, the Pad mode of the Properties panel can be accessed by pressing the Tab key. Once the Pad is placed, all options appear.

After placement, the Pad dialog can be accessed by:

• Double-clicking on the placed Pad object.
• Placing the cursor over the Pad object, right-clicking then choosing Properties from the context menu.

After placement, the Pad mode of the Properties panel can be accessed in one of the following ways:

• If the Properties panel is already active, by selecting the Pad object.
• After selecting the Pad object, select the Properties panel from the Panels button at the bottom right of the design space or select View » Panels » Properties from the main menu.

Editing Multiple objects

The Properties panel supports multiple object editing, where the property settings that are identical in all currently selected objects may be modified. When multiples of the same object type are selected manually, via the Find Similar Objects dialog or through a Filter or List panel, a Properties panel field entry that is not shown as an asterisk (*) may be edited for all selected objects.

Editing via the PCB List Panel

Panel page: PCB List, PCB Filter

The PCB 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 PCB 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.