Configuring Schematic Part Object Properties in Altium Designer

Parent page: Part

Schematic 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 Part object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic - Defaults page of the Preferences dialog (access 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 Part object properties are available for editing in the Properties panel when a placed Part is selected in the workspace.

  The Part default settings in the Preferences dialog and the Component mode of the Properties panel

General Tab

Properties

• Designator - enter the designator. Toggle  or  to show/hide the designator. Use the  icon to lock/unlock the designator. 
• Comment - enter the name. Toggle  or  to show/hide the name. Use the  icon to lock/unlock the name. 
• Part xx of Parts (Properties panel only) - displays the number of the selected part and the total number of parts. Use the drop-down to select the number of the associated part then enter the total number of parts. Click  to lock/unlock the fields.
• Description - the component/part description.
• Type - Select one of the following component types for the component footprint here. The available types are:
  • Standard - components that 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 - components that 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 - components that 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) - components that are used to short two or more different nets together, 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 (No BOM) - components that are used to short two or more different nets together, 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) - components that 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 want to exclude from the BOM.
  • Jumper - components that 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 - click  to open the Component Search dialog to select the desired item. Once selected, this field will display the full Design Item ID for the Component Item.
• Source - displays the name of the source library. Click  to search for and select the desired library.
• Revision State - displays the revision state of the part.

Location (Properties panel only)

• (X/Y)  
  • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current workspace origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
  • Y (second field) - The current Y (vertical) coordinate of the reference point of the object, relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
• Rotation - use the drop-down to select the rotation. Choices are: 0 Degrees, 90 Degrees, 180 Degrees, and 270 Degrees.

Links

•  Grid - displays all links for the selected component. Use the  to edit the selected link and  to delete the selected link. Click Add to open the following additional options to add a link: 
  • Add Link
    • Name - enter the desired name of the link.
    • Url - enter the URL of the desired link. Once the link is added, the Name appears in the grid as a link. 

Footprint

• Name - select the footprint name.
• Preview image - displays an image of the footprint for the selected component. Use the 2D or 3D control to toggle between the two modes.
• Add - click to open the PCB Model dialog in which you can choose the desired footprint. Use the  to edit the selected footprint and  to delete the selected footprint.

Models

• Name - the name of the model.
• Type - the model type.
• Add - click to select a model type to add. Choices include: Pin Info, Simulation, Ibis Model, and Signal Integrity.
•  - click to open a dialog to edit the selected model. Use  to delete the selected model.

Graphical

• Mode (Properties panel only) - use the drop-down to select the desired mode. 
• Mirrored (Properties panel only) - enable to mirror the part.
• Local Colors - check to enable the following options:
  • Fills - click on the color box to access a drop-down from which you can select the default color.
  • Lines - click on the color box to access a drop-down from which you can select the default color.
  • Pins - click on the color box to access a drop-down from which you can select the default color.

Parameters Tab

Parameters

• Grid - lists the Name and Value of the parameters associated with the currently selected component. Use  to lock/unlock a listed parameter.
• Font - click on the displayed font to change the font style.
• Other - click to open a drop-down to change additional options:
  • Show Parameter Name - enable to show the parameter name.
  • Allow Synchronization with Database - enable to synchronize with the database.
  • X/Y - enter the X and Y coordinates.
  • Rotation - use the drop-down to select the rotation. Choices are: 0°, 90°, 180°, and 270°.
  • Autoposition - check to enable auto-positioning.
• Add - click to add a parameter. Use the trash can   to delete a selected entry from the table. Use the pencil available in the Rules section to open the Edit PCB Rule (From Schematic) dialog.

Pins Tab (Properties panel only)

Pins

This region lists the Pins and Name for all the pins of the selected component. Use  or  to show/hide the pin. Use  to lock/unlock the pins.

• Add - click to add a parameter. Use the trash can   to delete a selected entry from the table. Use the pencil to open the Component Pin Editor dialog.