Altium Designer Documentation

Component Properties

Modified by Phil Loughhead on Sep 15, 2020
All Contents

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 workspace). 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 workspace.

  

If the Double Click Runs Interactive Properties option is disabled (default) on the PCB Editor - General page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open. 
While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly. 

In the below properties listing, options that are not available as default settings in the Preferences dialog are noted as "Properties panel only".

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 workspace 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. You make click the Designator hyperlink to be taken 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 user-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 and select the Update PCB With <ComponentName> command from the context menu.
    • You can also user-define the area of a component already placed on a PCB; select the component, and enter the value in the Area field of the Component mode of the Properties panel (this field).
    • To switch from a user-defined area to a calculated area for a component placed on a PCB, delete the value in the Area field in the Properties panel; 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; or 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 of the images below shows 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.

  • The edge of the Courtyard is the centerline of the outline tracks and arcs that form the Courtyard boundary.
  • A curved component Courtyard shape can be created using arcs, as shown in the upper of the images above, where the Courtyard curves around pad 3.

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 - this field states the current revision state of the placed component. Draft will appear for an component revision that is not up to date, while Up to date appears for a component that is.
  • Height - a height field for the component, this field was used before the introduction of the 3D Body object, which provides a superior method of defining the component height.
  • 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. 
Select the clickable clicks of the Designator and Comment from the Component mode of the Properties panel to be redirected to those objects respective Properties panels, where you may edit their options.

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)

Schematic reference information is transferred from the schematic to the PCB editor when the design is initially transferred. To refresh this data at a later stage, click the Perform Update button in the Edit Component Links dialog.
  • 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.
Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.