Configuring PCB Component Object Properties in Altium Designer

Parent page: Component

PCB Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

• Pre-placement settings – most Component object properties, or those that can logically be pre-defined, are available as editable default settings on the PCB Editor - Defaults page of the Preferences dialog (accessed from the  button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

• Post-placement settings – all Component object properties are available for editing in the Properties panel when a placed Component is selected in the design space.

General Tab

Location (Properties panel only)

The  icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status. 

• (X/Y) 
  • X (first field) - the current X (horizontal) coordinate of the reference point of the component, relative to the current design space origin. Edit to change the X position of the component. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. The reference point for a component footprint is set in the Library Editor.
  • Y (second field) - The current Y (vertical) coordinate of the reference point of the component, relative to the current origin. Edit to change the Y position of the component. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. The reference point for a component footprint is set in the Library Editor.
• Rotation - the component's angle of rotation (in degrees), measured counterclockwise from zero (the 3 o'clock horizontal). Edit to change the rotation of the component. Minimum angular resolution is 0.001°.

Properties

• ​​Layer - sets the layer on which the component is placed. Components can be assigned to the Top layer or Bottom layer. Use the drop-down to select a different layer. Changing the layer status swaps all of the component primitives to each layer's respective opposite layer. For example, moving a Top layer component to the Bottom layer means: single layer pages are swapped from the Top to the Bottom layer, primitives on the Top Overlay are reassigned to the Bottom Overlay, and primitives on a paired mechanical layer are swapped to the other mechanical layer in that pair. The orientation of the component will be flipped along the X-axis and the component overlay text will read from the bottom. 
• Designator (Properties panel only) - the designator of the component is an alphanumeric string of up to 255 characters. Each component must have a unique Designator string. Toggle  or  to show/hide the designator. Click the Designator hyperlink to open the Parameter Properties dialog.
• Comment (Properties panel only) - the comment of the component is an alphanumeric string of up to 255 characters. Toggle  or  to show/hide the comment. You make click the Designator hyperlink to be taken the Parameter Properties dialog.
• Area - the area of the placed component, displayed in the current board units. The area can be user-defined, if it is not it is automatically calculated from the component's selection area:
  • To define the component area, edit the Area in the PCB Library Footprint dialog in the PCB library editor. To push an updated footprint to an open PCB, right-click on the footprint name in the PCB Library panel then select Update PCB With <ComponentName> from the context menu.
  • You can also user-define the area of a component already placed on a PCB by selecting the component then entering the value in this field.
  • To switch from a user-defined area to a calculated area for a component placed on a PCB, delete the value in this field; the field will automatically be re-populated with the auto-calculated value.
  • The automatically calculated area is the area that highlights when you click to select the component. The selection area is determined from the geometries on the Courtyard layer, i.e. when that layer is not present, the combination of the geometries on the Silkscreen, 3D Body objects, and Copper layers (strings are excluded). The upper images displayed below show the component's area when there is an outline defined on the courtyard layer; the lower image shows the area when it is calculated from the geometries on the Silkscreen, 3D Body objects, and Copper layers.

► Learn more about how the selection area is calculated, and the other modes available to determine the selection area.

► Learn more about Working with Mechanical Layers.

• Description - enter the desired description.
• Type - select one of the following component types for the component footprint here. The available types are:
  • Standard - these components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. An example is a standard electrical component, such as a resistor.
  • Mechanical - these components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are included in the BOM. An example is a heatsink.
  • Graphical - these components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are not included in the BOM. An example is a company logo.
  • Net Tie (in BOM) - these components are used to short two or more different nets together. They are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked - it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper within the component.
  • Net Tie - these components are used to short two or more different nets together. They are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked - it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper in the component.
  • Standard (No BOM) - these components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. An example is a testpoint component that you wish to exclude from the BOM.
  • Jumper - these components are used to include wire links in a PCB design, for example, on a single-sided PCB that cannot be fully routed on one layer. For this component type, the component footprint and pins are synchronized between the schematic and PCB but the net assignments are not, and the component is included in the BOM. As well as selecting this option at the component level, both of the pads in the component must have their JumperID set to the same non-zero value. Jumper-type components do not need to be wired on the schematic; they only need to be included on the schematic if they are required in the BOM. If they are not required in the BOM, they can be placed directly in the PCB where the Component Type is set, the JumperIDs are set, and the Nets manually assigned for the pads. 
• Design Item ID (Properties panel only) - displays the Design Item ID for the selected component. This field is not editable.
• Source (Properties panel only) - displays the source document of the component. Click to open a dialog to browse and select a different source document.
• Revision State - shows the state of the revision of the managed component in terms of its lifecycle state and also its revision status, i.e. whether it is the latest released revision of that component (Up to date) or is an earlier revision (Out of date).

• Height - a height field for the component. This field defined the height of the PCB component before the introduction of the 3D Body object, however the 3D model provides a superior method of defining the component height for tasks such as 3D collision detection. Note that the value defined in this Height field is used by Altium MCAD CoDesigner, not the height of the 3D model (learn more).
• 3D Body Opacity - enter the desired opacity percentage or use the slider bar.
• Primitives - click the associated lock icon to lock/unlock.  - lock all the primitives of the component so that it can be treated as a single object.  - unlock to modify the individual primitives that make up the component. After editing, the component primitives should be re-locked. Note: Component pad properties can be modified without unlocking the primitives by double-clicking directly on the pad. 
• Strings - click the associated lock icon to lock/unlock.  - lock all the strings of the component. ​ - unlock to modify the strings of the component. 

Footprint (Properties panel only)

• Footprint Name - displays the name of the footprint corresponding to the chosen component.
• Design Item ID - the identification of the chosen component.
• Source - displays the name of the server in which the chosen component has been placed.
• Description - displays the description of the component, which can also be seen in the Components panel.

Swapping Options

• Enable Pin Swapping - check to allow the pin swapping function.
• Enable Part Swapping - check to allow the part swapping function (e.g., four parts of a 74 series IC).

Schematic Reference Information (Properties panel only)

• Designator - the designator of the schematic component to which this PCB component has been matched.
• Hierarchical Path - displays where, in the hierarchical structure of the schematic, this component can be found.
• Channel Offset - when a design is first transferred from schematic to PCB, each component on each schematic sheet is given a unique channel offset.

Parameters Tab

• Table - displays the Name, Value, and Source of each listed parameter.