Ready to start PCB layout, but missing some footprints?
New to Altium Designer and struggling to get your design from schematic capture to PCB layout? Perhaps you're staring at a list of missing footprints, and wondering what's the best way to sort it out. Enter the Footprint Manager.
Validating the footprints
The Footprint Manager in the schematic editor (Tools menu) is ideal for tracking down and resolving missing footprints. The Footprint Manager details the footprints attached to every component in the entire design and includes a Validate feature, which checks if the footprint is present in one of the currently Available Libraries. But it is much more than a simple validation tool, with the ability to select an alternate library or even an alternate footprint, for one or multiple components!
Where does the footprint come from?
In Altium Designer, the footprint is specified in the component symbol. Apart from the footprint name, this reference can also detail if the footprint must come from a specific library, as shown in the image below, where the resistor footprint must come from the specified chip resistor library. If the PCB library option is set to Any, then all available libraries are searched for a footprint of that name. Keep this in mind when you're checking the footprint status - can the missing footprint come from any library, or must it come from a specific library?
This footprint must be sourced from the specified library.
Tracking down the missing footprints
When you open the Footprint Manager, it lists all components in the entire design. Right-click on the left of the dialog and Select All the components, right-click in the right of the dialog and Select All footprints, then click the Validate button to identify those footprints that cannot be found.
The Footprint Manager details the status of all footprints across the entire design.
Once the Footprint Manager has identified which footprints can not be found, you can work through the list and find them, selecting the specified library, an alternate library, or an alternate footprint as required.
When the specified library is a PcbLib
Remember when I said that it was important to appreciate how the symbol-to-footprint linking also details where the footprint must be found? The PCB Library column in the Footprint Manager tells you where the footprint must come from. If the footprint must come from a specific PcbLib, then you can select that footprint in the list, click Edit to open the PCB Model dialog, click the Browse button to open the Browse Library button, click the ... button to open the Available Libraries dialog, then click the Install button to find and install that library.
Phew, got all that? Once you've walked through it once, it's easy. Oh, and don't forget to click the Accept Changes button in the Footprint Manager before you close it.
When the specified library is Any
If there is no library name specified, then you'll have to search for a footprint. Going through a similar sequence, select the footprint in the F ootprint Manager and click Edit to open the PCB Model dialog. Copy the Name string (to save typing it later), then click Browse to open the Browse Libraries dialog.
This time, click the Find button to open the Libraries Search dialog, enter the name of the footprint you're after in the Value field, and set the Field to Name and Operator to contains. Set the search Scope to Libraries on Path, and if you want to restrict the search to supplied footprint libraries only, set the path to C:\Program Files\Altium Designer Winter 09\Library\pcb, or wherever your company stores the Altium Designer footprints.
Use the Search feature to locate suitable footprints.
Any matches will be detailed in the Browse Libraries dialog. When you select one and click OK you'll be prompted to install the library, which you must do to make the footprint available.
When the specified library is an IntLib
If the specified library is an IntLib, then you'll need to close the Footprint Manager and install the IntLib via the Libraries button at the top of the Libraries panel.
What to do when you can't find a footprint?
Firstly, if the footprint is configured to come from a specific library and you don't have that library, then you can change the setting in the PCB Models dialog to Any, and try and search for the footprint in all libraries. If any IntLibs come up in the search results you can use footprints from them, even though the PCB Models dialog will continue to show the footprint as not found.
If there is no matching footprint available, then you'll have to create it yourself. If you are creating it from scratch, check out the wizards in the Tools menu of the PCB Library editor.
How long do you need to keep the footprint libraries available?
Once you have transferred the design to PCB layout, the footprints are stored in the board file. That means you no longer need to keep those libraries available.
Watch the video:
