Parent page: PCB Objects
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.
Pads are available for placement in both the PCB and the PCB Library editors in one of the following ways:
After launching the command, the cursor will change to a crosshair and you will enter pad placement mode.
Additional actions that can be performed during placement are:
Pads cannot have their properties modified graphically other than their location.
The following methods of non-graphical editing are available:
Properties page: Pad Properties
This method of editing uses the associated Properties panel mode to modify the properties of a Pad object.
During placement, the Pad mode of the Properties panel can be accessed by pressing the Tab key.
After placement, the Pad mode of the Properties panel can be accessed in one of the following ways:
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.
Dialog page: Pad
This method of editing uses the Pad dialog to modify the properties of a pad object.
The Pad dialog can be accessed from the Netlist Manager dialog (Design » Netlist » Edit Nets) by clicking the Edit button under the Pins in Focused Net region.
The hole can be round, square (punched), or a circular-ended slot. It can also be plated or unplated. Separate drill files are generated for each hole kind (Round, Rect and Slot) as well as for plated and non-plated holes (as defined by the Plated checkbox). That means there can be up to six different drill files generated.
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 one during placement if the initial pad has a designator ending with a numeric character.
The Layer drop-down is used to select the layer on which the pad is placed. 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
The Net field is used to define to which net this 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.
If it is not physically possible (or desirable) to implement all connections as routing, for example, on a single-sided PCB, then 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 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 connections are shown as curved connection lines in the PCB editor. The Design Rules Checker will not report jumper connections as unrouted nets.
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.
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 Paste Mask Expansion and Solder Mask Expansion settings. Typically paste mask openings are smaller than the pad, while solder mask openings are larger than the pad, however, 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 defined directly in the Properties panel, 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.
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.