Quartus® Prime Pro Edition User Guide: PCB Design Tools

ID 683768
Date 4/01/2024
Document Table of Contents Updating FPGA Symbols

As the design process continues, you must make logic changes in the Quartus® Prime software, placing signals on different pins after recompiling the design, or use the Quartus® Prime Pin Planner to make changes manually. The board designer can request such changes to improve the board routing and layout. To ensure signals connect to the correct pins on the FPGA, you must carry forward these types of changes to the circuit schematic and board layout tools. Updating the .pin in the Quartus® Prime software facilitates this flow.

Figure 21. Updating the FPGA Symbol in the Design Flow

To update the symbol using the Cadence Allegro PCB Librarian Part Developer tool after updating the .pin, follow these steps:

  1. On the File menu, click Import and Export. The Import and Export wizard appears.
  2. In the list of actions to perform, select Import ECO - FPGA. Click Next. The Select Source dialog box appears.
  3. Select the updated source of the FPGA assignment information. In the Vendor list, select Altera. In the PnR Tool list, select quartusII. In the PR File field, click browse to specify the updated .pin in your Quartus® Prime project directory. Click Next. The Select Destination window appears.
  4. Select the source component and a destination cell for the updated symbol. To create a new component based on the updated pin assignment data, select Generate Custom Component. Selecting Generate Custom Component replaces the cell listed under the Specify Library and Cell name header with a new, nonfractured cell. You can preserve these edits by selecting Use standard component and select the existing library and cell. Select the destination library for the component and click Next. The Preview of Import Data dialog box appears.
  5. Make any additional changes to your symbol. Click Next. A list of ECO messages appears summarizing the changes made to the cell. To accept the changes and update the cell, click Finish.
  6. The main Cadence Allegro PCB Librarian Part Developer window appears. You can edit, fracture, and generate the updated symbols as usual from the main Cadence Allegro PCB Librarian Part Developer window.
Note: If the Cadence Allegro PCB Librarian Part Developer tool is not set up to point to your PCB Librarian Expert license file, an error message appears in red at the bottom of the message text window of the Part Developer when you select the Import and Export command. To point to your PCB Librarian Expert license, on the File menu, click Change Product, and select the correct product license.