Intel® Quartus® Prime Pro Edition User Guide: PCB Design Tools

ID 683768
Date 11/04/2020
Public
Document Table of Contents

4.5.1.1.2. Import and Export Wizard

After starting the Cadence Allegro PCB Librarian Part Developer tool, use the Import and Export wizard to import your pin assignments from the Intel® Quartus® Prime software.

Note: Intel recommends using your PCB Librarian Expert license file. To point to your PCB Librarian Expert license file, on the File menu, click Change Product and then select the correct product license.

To access the Import and Export wizard, follow these steps:

  1. On the File menu, click Import and Export.
  2. Select Import ECO-FPGA, and then click Next.
  3. In the Select Source page of the Import and Export wizard, specify the following settings:
    1. In the Vendor list, select Altera.
    2. In the PnR Tool list, select quartusII.
    3. In the PR File box, browse to select the .pin in your Intel® Quartus® Prime project directory.
    4. Click Simulation Options to select simulation input files.
    5. Click Next.
  4. In the Select Destination dialog box, specify the following settings:
    1. Under Select Component, click Generate Custom Component to create a new component in a library,

      or

      Click Use standard component to base your symbol on an existing component.

      Note: Intel recommends creating a new component if you previously created a generic component for an FPGA device. Generic components can cause some problems with your design. When you create a new component, you can place your pin and signal assignments from the Intel® Quartus® Prime software on this component and reuse the component as a base when you have a new FPGA design.
    2. In the Library list, select an existing library. You can select from the cells in the selected library. Each cell represents all the symbol versions and part fractures for a particular part. In the Cell list, select the existing cell to use as a base for your part.
    3. In the Destination Library list, select a destination library for the component. Click Next.
    4. Review and edit the assignments you import into the Cadence Allegro PCB Librarian Part Developer tool based on the data in the .pin and then click Finish. The location of each pin is not included in the Preview of Import Data page of the Import and Export wizard, but input pins are on the left side of the created symbol, output pins on the right, power pins on the top, and ground pins on the bottom.

Did you find the information on this page useful?

Characters remaining:

Feedback Message