How to Create a PCB Footprint in OrCAD X | Cadence

December 2, 2024

Cadence PCB Solutions

Key Takeaways

Symbol Creation: Start by referencing the component datasheet to accurately assign pinouts in OrCAD Capture.
Footprint and 3D Model Download: Download the correct 2D footprint and 3D model from sites like SnapEDA for integration into your project.
Assigning and Editing Footprints: Use the Edit Properties option to assign or edit footprints, ensuring proper alignment with the symbol.

View of component footprint in OrCAD X — *How to create a PCB footprint in OrCAD X is a fairly straightforward process. You can also select the 3D model in the properties panel of the footprint.*

When designing a PCB that requires particular parts, you may need to learn how to create a PCB footprint in OrCAD X. The process involves creating a symbol based on the component's datasheet, assigning the correct pinouts, and then linking the footprint and 3D model to the symbol. In OrCAD X, this workflow is streamlined, providing designers with advanced tools for managing footprints, symbols, and component properties. Read on to learn how!

How to Create a PCB Footprint in OrCAD X

Step	Description
Create the Symbol	Open the component datasheet to understand the pinouts (e.g., Ground, Output, etc.). Create a new project in OrCAD X Capture and a schematic page. Use the Place and Part options to create the symbol, ensuring all pins are correctly assigned based on the datasheet.
Padstack Creation	In OrCAD X, pads are created independently of the footprints to allow for faster reuse. Create the padstack based on the datasheet requirements, then assign it during the footprint creation process to ensure it matches the symbol pinout.
Download Footprint & 3D STEP Model	Download the footprint and STEP model from the manufacturer or trusted source, or use an MCAD software to create them if necessary. Ensure to download both the 2D footprint and the 3D model. Save the files (PSM, STEP) in your project folder under appropriate subdirectories.
Assign the Footprint	In the schematic, right-click on the component and select Edit Properties. Scroll down to the footprint section, and assign the downloaded footprint (PSM file) by entering its name. Save the changes to link the footprint to the symbol. Verify that the footprint is correctly mapped.
Switch to PCB Design	Once you have your board, with design rules like spacing, and define package/route keep-in areas., import the netlist using Import Logic to bring in the components and connections.
Add the 3D Model	For OrCAD X Presto: Add the 3D model directly in the Properties Panel of the footprint as seen in the image above. For OrCAD X Professional: Copy the STEP model to the Cadence folder (C:\Cadence\SPB_17.4\share\pcb\step). Use the Step Package Mapping option to associate the STEP model with the footprint in PCB Editor. Rotate or adjust the model as needed for proper alignment.
Visualize in 3D	After importing the STEP model, view the 3D model in PCB Editor to verify proper alignment. Use the 3D view to ensure the footprint and STEP model are correctly placed on the solder pads. This helps avoid issues during manufacturing and ensures correct positioning of the component on the PCB.

*Editing a footprint can be done with right click > Edit Footprint.*

Editing a Footprint in OrCAD X

Once you know how to create a PCB footprint in OrCAD X, you may need to further edit a footprint down the line as well. To edit a footprint in OrCAD X Presto, begin by selecting the component and right-clicking to choose "Edit Footprint." If the footprint is stored in your library, it will open in the Footprint Editor. If it’s not in your library, you’ll be prompted to export the footprint from the database to your working directory for editing.

Once exported, a new Footprint Editor window opens alongside your original layout database, where edits are applied. After making adjustments, such as moving pins, updating place bounds, or replacing pad stacks, save the changes and close the editor. The layout editor will then recognize the updates and prompt you to apply them. Options will include updating text, removing fanout, or refreshing pad stacks. Once confirmed, the updated footprint is applied across the entire layout, reflecting the changes in every instance of that component.

*OrCAD X Footprint Editor with properties panel on the right.*

OrCAD X Footprint Authoring

The OrCAD X footprint editor is designed for efficient and detailed footprint creation. The Properties panel offers a comprehensive overview of a footprint, including the number and type of electrical and mechanical pins, the reference designator, 3D model access, and a list of pad stacks, which can be updated or replaced as needed

Additionally, the panel includes a change history log for tracking modifications. When adding pins, you can search your pad stack library, view detailed pad stack parameters, and select the appropriate one for your design. If a new pin is required, you can create a pin pad stack parametrically by specifying dimensions for surface-mount or through-hole pin types. Pins can be placed using adjustable grids or by snapping to specific points in the design, with the Properties panel automatically updating to reflect the new additions.

Adding Multiple Footprints In OrCAD X

To add multiple footprints to a component in OrCAD X Capture, start by placing a component that supports multiple footprints.

In the Component Explorer, search for your part via description or part number.
If prompted, enter your credentials.
Once selected, view the available footprints in the properties tab, where you can see all associated symbols and footprints.
Place the component in the schematic, adjusting the reference designators if necessary to avoid conflicts. For example, if you have multiple instances of the same component, make sure to update the reference designators to unique values.

*Adding alternate symbols in OrCAD X, make sure to create the ALT_SYMBOLS property before editing it.*

In OrCAD X Capture, right-click the component and select "Edit Properties" to assign alternate footprints. In the Property Editor, add a new property labeled ALTSYMBOLS, entering the alternate footprint values. Once applied, use Ctrl to select multiple components and repeat the process for additional instances.

To sync the alternate footprints with the PCB layout, save your design and select "Update Layout." This opens OrCAD X Presto, where you can apply the changes. After syncing, place the components on the board using the placement tool, selecting each footprint from the dropdown in the properties panel. This ensures that the alternate footprints are correctly applied for different board form factors or variations.

As a whole, knowing how to create a PCB footprint in OrCAD X is important when using particular components. OrCAD X features an advanced footprint editor and integrated design environment to streamline the process, making it easier to manage even the most complex designs. Explore more about Cadence's PCB Design and Analysis Software and see how OrCAD X can enhance your PCB design workflow.

Leading electronics providers rely on Cadence products to optimize power, space, and energy needs for a wide variety of market applications. To learn more about our innovative solutions, talk to our team of experts or subscribe to our YouTube channel.