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.

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 <x> 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 - this field lists the name of the component selected. Click  to open the Replace Component (Managed) dialog or Replace Component (File-based) dialog, depending on whether the component is managed or non-managed. This dialog grants access to full details of the selected component (Parameters, Models, Part Choices, Supplier data, etc.,), component comparison, and the ability to replace the current component with another, among other possibilities. If another component is selected as a replacement, this field will then display the full Design Item ID for the newly selected component. Click the Validate button to see information regarding where the component resides. If it is non-managed, the file path in which it is saved on your computer will appear. If it is managed, the information will indicate that the component was simply found.
• Source - displays the name of the source library of the component. Click  to search for and select the desired library.
• Revision State - this field displays the revision state of the part. Select the Up to date  icon to update the part's revision state. The SPN (Supplier Part Number) contains the following information:
  • Colored tile banner showing the supplier name and price. The color reflects the risk associated with choosing that supplier. The risk can change at any time based on the availability and price data received from the Altium Parts Provider.
    • Green = Best
    • Orange = Acceptable
    • Red = Risky
  • Supplier part number (linked to the part on the Supplier's website)
  • Last updated icon with details displayed in the tooltip, color indicates:
    • White/Gray = Default, updated less than one week ago
    • Orange = 1 week < last update < month ago
    • Red = last update > 1 month ago
  • Country code for the Supplier location (ISO alpha 2); colored red if unknown.
  • Part source, details displayed in the tooltip.
  • Stock quantity; red if no stock available.
  • Unit price, red if no price available. Unit price includes currency icon, currency is determined by the location of the supplier.
  • Available price breaks, with Minimum Order Quantities.

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.

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.

Part Choices

• Part Name - click to be lead to further information about the part, provided directly from the supplier.
• Datasheet - click this button to be lead to the product's latest information, directly from the supplier's website.
• SPN(s) - an SPN (Supplier Part Number) contains the following information:
  • Colored tile banner showing the supplier name and price. The color reflects the risk associated with choosing that supplier. The risk can change at any time based on the availability and price data received from the Altium Parts Provider.
    • Green = Best
    • Orange = Acceptable
    • Red = Risky
  • Supplier part number (linked to the part on the Supplier's website)
  • Last updated icon with details displayed in the tooltip, color indicates:
    • White/Gray = Default, updated less than one week ago
    • Orange = 1 week < last update < month ago
    • Red = last update > 1 month ago
  • Country code for the Supplier location (ISO alpha 2); colored red if unknown.
  • Part source, details displayed in the tooltip.
  • Stock quantity; red if no stock available.
  • Unit price, red if no price available. Unit price includes currency icon, currency is determined by the location of the supplier.
  • Available price breaks, with Minimum Order Quantities.

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. This option is used to control if the comment can be updated. By default, these options are enabled to always allow synchronization with the source library/database. You may disable this option to prevent that comment from being included in an update process.
  • 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, meaning that the text will remain in the chosen position as the component is moved and rotated.
• Add - click to add a parameter, such as a footprint, model, or rule, among others. Use the bin  to delete a selected entry from the grid. Use the pencil icon to edit the parameter via the parameter's respective dialog.

Pins (Part Dialog only)

Click the Pins button, located in the bottom left corner of the dialog, to open the Component Pin Editor dialog, from where you may view all pins for either the component in the active schematic library document or a placed component (or part thereof) in the schematic editor.

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 pin. Use the trash can   to delete a selected entry from the table. Use the pencil to open the Component Pin Editor dialog.