Working with a Pad Object on a PCB in Altium Designer

Вы просматриваете версию 16.1. Для самой новой информации, перейдите на страницу Working with a Pad Object on a PCB in Altium Designer для версии 21


Parent page: PCB Objects

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


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 3 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 editor and the PCB Library editors, by selecting Place » Pad from the main menu, or by clicking the button in the wiring toolbar.


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

  1. Position the cursor and click or press Enter to place a pad.
  2. Press the Tab key to access an associated properties dialog, from where properties for the pad can be changed on-the-fly.
  3. Continue placing further pads, or right-click or press Esc to exit placement mode.

A pad will adopt a net name if it is placed over an object that is already connected to a net.

While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement. 

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.

If you click and drag a selection rectangle around component pads, they will not select as they are actually child objects of the component. To sub-select just the pads, hold Ctrl as you click and drag the selection window.

An object that has its Locked property enabled cannot be selected or graphically edited. Double click on the locked object directly and disable the Locked property, to graphically edit the object.

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 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-clicking on the placed pad object.
  • Placing the cursor over the pad object, right-clicking and choosing 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.

Setting the Hole Size

The hole can be round, square (punched), or a circular-ended slot. It can also be plated or unplated. Separate drill files (NC Drill Excellon format 2) are generated for each hole kind (Round, Square 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.

Use the Hole Size Editor (a mode of the PCB panel) to examine and rationalize the hole sizes used in a completed PCB design.

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.

Multiple pads can share the same designator, if required.

Setting the Layer

The layer drop-down is used to select the layer that the pad is present on. 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 pads' 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 which net this pad is to connect to. 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, 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 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 that the pad or via belongs to, automatically gets locked.

Mask Expansions

An opening in the paste and solder mask is automatically created by the software, 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 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.

Paste and Solder mask layers are shown in the negative, that is, when you see an object on one of those layers it is actually a hole or opening in that layer.

If your component needs paste or soldermask shapes that are different from the pad shape, then you can place design objects, such as fills, regions, tracks or arcs, directly onto the top solder or paste mask layer in the library editor, to create the required shape.

Editing via an Inspector Panel

Panel pages: PCB Inspector, PCBLIB Inspector

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.


If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

Набор доступных функций зависит от вашего уровня доступа к продуктам Altium. Ознакомьтесь с функциями, включенными в различные уровни Подписки на ПО Altium, и функциональными возможностями приложений, предоставляемых платформой Altium 365.

Если вы не видите в своем ПО функцию, описанную здесь, свяжитесь с отделом продаж Altium, чтобы узнать больше.