Pad
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 to create 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 editor and the PCB Library editors by clicking Home | Place | 
from the main menus. Placement
After launching the command, the cursor will change to a crosshair and you will enter pad placement mode.
- Position the cursor then click or press Enter to place a pad.
- Press the Tab key to access an associated properties dialog, from where properties for the region can be changed on-the-fly.
- Continue placing further pads, or right-click or press Esc to exit placement mode.
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 then 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 Editor - select the Tools | Arrange | Move » Move Object command, click, hold then move the pad.
- In the PCB Library Editor - select the Home | Arrange | Move » Move Object command, click, hold then move the pad.
Non-Graphical Editing
The following methods of non-graphical editing are available:
Editing via an Associated Properties Dialog
Dialog page: Pad
This method of editing uses the following dialog to modify the properties of a pad object.
Edit the properties of the Pad in the Pad dialog.
The Pad dialog can be accessed during placement by pressing the Tab key.
After placement, the dialog can be accessed in one of the following ways:
- Double-click on the placed pad object.
- Place the cursor over the pad object, right-click then choose Properties from the context menu.
Quickly change the units of measurement currently used in the dialog between metric (mm) and imperial (mil) using the Ctrl+Q shortcut. This affects the dialog only and does not change the actual measurement unit employed for the board as determined by the 
and 
buttons in the Home | Grids and Units area of the main menus. Setting the Hole Size
The hole can be round, square, or slotted, and can also be plated or unplated. Separate drill files (NC Drill Excellon format 2) are generated for plated and non-plated holes (as defined by the Plated checkbox). That means there can be up to two different drill files generated.
Incrementing the Pad Designator
Each pad should be labeled with a designator, which is usually a component pin number. The designator can be up to 20 alphanumeric characters in length. Pad designators will auto-increment by 1 during placement if the initial pad has a designator ending with a numeric character. Press Tab to change the designator of the first pad prior to placement.
Setting the Layer
The layer drop-down is used to select the layer on which the pad is located. When designing a surface-mount component footprint, set the Layer to Top layer even if the component is intended to be used on the bottom side of the board. The software will automatically flip the pad's layer when the component is flipped to the bottom side of the board. For a standard, through-hole pad, set the Layer to Multi-Layer.
Connecting to a Net
The Net field is used to define to which net the pad is to connect. Pads automatically connect to any internal power planes that are assigned to the same net. The pad will connect to the plane in accordance with the applicable Power Plane Connect Style design rule. If you do not want a pad to connect to power planes, add another Power Plane Connect Style design rule targeting the required pads with a connection style of No Connect. Pads connect to polygon pours in accordance with the applicable Polygon Connect Style design rule.
Setting the Jumper ID
If it is not physically possible (or desirable) to implement all connections as routing, for example, on a single-sided PCB, jumpers can be used. Within a component footprint, label the pads that are to be connected by a jumper with the same, non-zero, Jumper ID value. Pads that share the same Jumper ID and Net name tell the system that these pins will be connected by a physical jumper during PCB assembly if that component also has a Type of Jumper.
Jumper connections are shown as curved connection lines in the PCB editor. The Design Rules Checker will not report jumper connections as unrouted nets.
Wire-link style jumpers can be defined by setting matching JumperID values in both pads.
Testpoint Settings
Use the Testpoint Settings to define this pad as a testpoint for Fabrication and/or Assembly. A testpoint is a location where a test probe can make contact with the PCB to check for correct function of the board. Any pad or via can be nominated as a testpoint. When this is done, the component to which the pad or via belongs automatically gets locked.
Mask Expansions
An opening in the paste and solder mask is automatically created by the software and is the same shape as the pad. This opening can be larger (a positive expansion value) or smaller (a negative expansion value) than the pad itself as defined by the Mask Expansion settings. Typically paste mask openings are smaller than the pad, while solder mask openings are larger than the pad, but there are exceptions to this. The default is for the pad to use the Expansion value from rules (the Paste Mask Expansion rule and the Solder Mask Expansion rule). This can be overridden and local values can be defined directly in the Pad dialog, if required.
The term tenting means to close off. If a tenting option is enabled then the settings in the applicable Solder Mask Expansion design rule will be overridden, resulting in no opening in the solder mask on that solder mask layer for this pad. When this option is enabled, the Expansion value from rules and the Specify expansion value options are ignored.
Editing via an Inspector Panel
An Inspector panel enables you 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.