Working with PCB Libraries

This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer and a connected Altium 365 Workspace. Check out the FAQs page for more information.


Parent page: Working with File-based Component Libraries

The real-world component that gets mounted on the board is represented as a schematic symbol during design capture, and as a PCB footprint for board design. Altium NEXUS components can be:

  • Created in and placed from local libraries or
  • Placed directly from a connected Workspace, accessible for the entire design team.
This document outlines the creation and management of PCB libraries (*.PcbLib). To learn more about creating a PCB footprint itself, refer to the Creating a PCB Footprint page.

Footprints can be copied from the PCB editor into a PCB library, copied between PCB libraries, or created from scratch using the Footprint Wizard or drawing tools.

Creating a New PCB Library

To create a new PCB library, select the File » New » Library command from the main menus and select the PCB Library option from the File region of the New Library dialog.

After clicking Create, a new PCB library document named PcbLib1.PcbLib is created and shown in the Projects panel, and an empty component sheet called PCBComponent_1 displays.

The content of the library is shown in the PCB Library panel.

You are now ready to add, remove, or edit the footprint components in the new PCB library using the PCB footprint editor commands.

If you have a PCB design with all the footprints already placed, you could use the Design » Make PCB Library command in the PCB editor to generate a PCB library that includes only those footprints.

Creating a New PCB Footprint

Any number of PCB footprints can be created in a PCB library. To create a new PCB footprint in an existing library, you would normally select Tools » New Blank Footprint.

Since a new library always contains one empty PCB footprint, you can also rename Component_1 to get started on creating a footprint. To do this, select PCBComponent_1 from the Footprints list in the panel then click the Edit button in the panel or double-click PCBComponent_1 to open the PCB Library Footprint dialog. Type the new footprint name that uniquely identifies it in the Name field then click OK.

Creating a Footprint Using the IPC Footprint Batch Generator

In addition to the techniques described on the Creating a PCB Footprint page, the IPC Footprint Batch Generator can be used to generate multiple footprints at multiple density levels. The generator reads the dimensional data of electronic components from an Excel spreadsheet or comma-delimited file then applies the IPC equations to build IPC-compliant footprints. Support for the IPC Footprints Batch Generator includes:

  • Package type blank template files are included in the \Templates folder in the Altium NEXUS installation.
  • Package input files can contain the information for one or more footprints of a single package type and can be either an Excel or comma-delimited (CSV) format file.

 The IPC Footprints Batch Generator has options to either create all the footprints in the open PCB footprint library or generate a single library based on either an input file or footprint name.
The IPC Footprints Batch Generator has options to either create all the footprints in the open PCB footprint library or generate a single library based on either an input file or footprint name.

Adding Footprints from Other Sources

PCB Components can be copied from other PCB Libraries and then renamed and modified within the destination library to match the specifications required. There are a number of ways to execute this function.

  • Select placed footprint(s) in a PCB document then copy (Edit » Copy) and paste them into an open PCB library using Edit » Paste Component.
  • Select Edit » Copy Component when the footprint to be copied is active in the PCB Library Editor, change to the open PCB destination library then select Edit » Paste Component.
  • Select one or more footprints in the list in the PCB Library panel using the standard Shift+Click or Ctrl+Click, right-click then choose Copy. Switch to the target library, right-click in the list of footprint names then choose Paste.

Validating Component Footprints

There are a series of reports that you can run to check that the footprints have been created correctly and identify which components are in the current PCB library. To validate all components in the current PCB library, run the Component Rule Check report. The Component Rule Check tests for duplicate primitives, missing pad designators, floating copper, and inappropriate component reference. To run the Component Rule Check:

  1. Save your library file before running any of these reports.
  2. Select Reports » Component Rule Check (shortcut R, R) to open the Component Rule Check dialog.

  3. Check all the boxes available then click OK. A report titled PCB<libraryfilename>.ERR is generated and opens in the Text Editor. Any errors will be noted.
  4. Close the report to return to the PCB footprint editor.

Updating a PCB Footprint

Updating a PCB Footprint from a PCB Library can be done in two ways: "Pushing" the PCB from the PCB Library, or by "Pulling" from the PCB Editor. Pushing a PCB Footprint update takes a selected footprint(s) from the PCB Library and uses it to update all open PCB documents containing that footprint. This first method is the best option when a complete replacement is desired. The second option allows you to review all the differences between the existing footprint and the footprint in the library before the update is performed. You can also select which objects are to be updated from the library. This second method is the best option when you need to figure out exactly what has changed between the footprint on the board and the footprint in the library.

Pushing Footprint Updates from the PCB Library

From the PCBLIB Editor, use the Tools » Update PCB with Current Footprint or Tools » Update PCB With All Footprints command. From the PCB Library panel, right-click in the Components region of the PCB Library panel then select Update PCB with [Component] or Update PCB with All. Running these commands opens the Component(s) Update Options dialog from which you can select the primitives/attributes to be updated.

The selected updates will be pushed to correlating footprints in all open PCB documents.

Pulling Footprint Updates from the PCB Editor

From the PCB editor, use the Tools » Update From PCB Libraries command, which, in turn, opens the Update From PCB Libraries - Options. Click OK to open the Update From PCB Libraries dialog.

PCB Library Panel

The PCB Library panel enables you to browse footprints stored in the active PCB library document and edit their properties. When a PCB Library document is active, the panel becomes populated with information pertaining to the constituent footprints of that library. The panel also offers the ability to pass on any changes made to them directly to the PCB design document.

The PCB Library panel
The PCB Library panel

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