Easily Loading PCB Footprints in Allegro PCB Editor
Learn how a good PCB footprint starts with a well-made padstack.
Understand how to build and load PCB footprints into Allegro.
Find additional tools and resources to help populate your footprint library.
Some surface mount components
There is a room in my house that I value quite a lot because it has bookshelves built into the walls. Reading seems to have lost a lot of its appeal in this digital age, but I still appreciate being able to relax with a good book in my hands. And since I’m the one who bought, arranged, and continually manages all of those books, I know exactly where each one is shelved whenever I want to revisit a classic story.
Knowing the benefits of a well-organized library, it is always painful to me when I have difficulty accessing the parts I need in a PCB design CAD system. Not only does the lack of an efficient library make finding the correct footprints difficult, but organizing new parts can be a real challenge too.
On the other hand, working with an organized library for loading PCB footprints into your design tools is a real joy. Here are some examples of ways to work footprints and libraries into Allegro’s PCB Editor so that they will be easy to find and use in your next PCB layout.
PCB Footprints First Start With a Padstack
Before we look at ways to create and load PCB footprints into Allegro, we have to first start with the padstack that will make up the foundation of the footprint. As with many of the design elements used in PCB layout, the padstack can either be imported or built. For our purposes, we are going to look at the process of building it in Allegro’s Padstack Editor. But before we start that, we need to ensure that the right library paths are set up within the Allegro PCB Editor for the work that we are going to do.
In the picture below, you can see the Setup > User Preferences pulldown menu. This menu is used for multiple settings, but the ones we are interested in here are the library paths. Within the library category of the path settings are two paths that need to be set for the libraries to work: the “padpath” and the “psmpath.” By saving or placing the pads and package symbols in the directories that these paths point to, you will have access to them within the PCB editor.
The Library Paths category in the Users Preferences Editor
With our paths correctly set, the next step is to open the padstack editor. Cadence’s Padstack Editor is a standalone tool, and although it can be opened from within the Allegro PCB Editor, it is simpler to use the Windows Start button to invoke it from the Cadence PCB Utilities. Once the padstack editor is open, set the units, decimal places, and what type of padstack that you are going to build. For our example, we are building a 75 mil by 25 mil rectangle to use with a surface mount footprint.
As you can see below, we are working in the Design Layers tab of the editor, and we have already input the values for our rectangular SMD pad on the “BEGIN LAYER.” Since this is a surface mount pad, we won’t be setting up any drill sizes or symbols, but we will add solder and paste mask layer data in the appropriate tab. Also, note that we have specified oversized thermal and antipad values along with the regular pad values. This instructs Allegro to increase the clearance around the pad when the footprint is surrounded by a solid metal plane.
Cadence’s Padstack Editor being used to build a rectangular SMD pad
To finish the pad, go to File > Save As, and save it out to the location that you previously set up for your library padpath. Now you are ready to use this pad when building a PCB footprint.
Building PCB Footprints to Load Into Your Layout
To create a footprint using the pad that we just created, open up the Allegro PCB Editor and go to File > New. In the New Drawing pop-up menu, select Package Symbol as the drawing type, and since we are going to create a simple fourteen pin IC, give it a drawing name of SOIC-14. Once you’ve OK’ed the dialog box, it will open a new window for creating the footprint. Before you start creating the part however, make sure that your parameters are set up the way you want by going to the Setup > Design Parameters menu. In the design tab are the settings for sizes and extents that you may want to adjust. You also have the choice of using the Design Workflow window to access the setups, and in this case, we will click on Grids to adjust their size and enable their display.
Now we will add some pins by going to the Layout > Pins pulldown menu. In the options window, make sure that the pin type is set to Connect, and click on the 3 dot browser button to select a padstack to use. Since our padpath was only set up for the directory that we saved our 75x25_smd pad in, that is the only padstack displayed in the pop-up browser. Double click on the padstack that you want to use, and continue to set up the remainder of the options. In our case, we want to place seven pins going down with a spacing of 0.050 inches between them. Now you can move your cursor into the correct location for the first pin, and click the mouse button to place all seven pins.
Placing pins in a surface mount footprint
In the picture above, you can see the first seven pins that have been placed, and the next row of pins is ready to be placed in the lower right corner. With the pin order in the options changed from down to up and the pin number starting at 8, all we have to do is to click the mouse button to place the next column of pins.
As with any footprint you will want to add various graphics and attributes. These can include silkscreen and assembly drawing shapes, pin 1 indicators, and component minimum and maximum heights to name a few. You do need to add a boundary outline for the part, however, and at least one of the layers needs to have a reference designator on it. Once all of this is completed, you can save the part. Remember, like the padstack, you will want this package symbol or footprint, to be saved into the directory that is specified by your “psmpath” so that the Allegro PCB Editor can find it later.
Loading PCB Footprints From Your CAD Libraries
With our footprint now created, we can load it into the PCB editor. In Allegro this is done by going to the Place > Manually pulldown menu. If you are working on a layout that already has other footprints in it, you will see them all in the Package symbols list of the Placement pop-up menu. Click on the Advanced Settings tab and disable the display of the database symbols, and then click back into the Placement List tab. Now you will only see the footprints saved to the library directory that you have specified in your library path, just as we have done in the picture below.
Using the Placement menu in Allegro PCB Editor to place the SOIC-14 footprint we just created
In the picture above we have selected our SOIC-14 from the placement menu to demonstrate how a footprint is loaded into the PCB editor. You can see the new part just to the right of the pop-up menu. If we had created additional parts, they would have been listed here in the placement menu along with the SOIC-14. Together with the library path setups, this system of footprint creation gives you precise control over your library as well as the footprints that you load into the layout tools. But manually building padstacks and symbol packages isn’t the only way to load new footprints into Allegro. There are some other options as well, which we’ll explore in the next section.
Footprint Building Tools and Resources
When we created our new footprint, we used the Package Symbol option in the New Drawing pop-up menu. If we had selected the Package Symbol (wizard) option instead, Allegro would have built the new footprint for us. The wizard provides an interface for you to specify the required PCB component package style as well as the desired padstack names, layer preferences, and unique dimensions. Once all of the information is entered into the interface, Allegro will create the part for you, saving a lot of time and effort.
The Unified Parts Search menu in Allegro’s schematic capture tools
Another option is to use the unified part search utility in the schematic editor. This feature allows you to search for parts based on their names, types, package styles, or any number of other identifying attributes. Once found, the browser will display all of the part data that it has including values, tolerances, manufacturing information, life cycle status, and even package illustrations as you can see in the picture above. It will also allow you to immediately add the part to your schematic while at the same time downloading the accompanying PCB footprint into your library.
Cadence has many other productivity enhancement features built into their tools, as well as helpful information on a wide range of topics such as this E-book on schematic library symbols.
If you’re looking to learn more about how Cadence has the solution for you, talk to us and our team of experts.