Enabling Pin Swapping on the PCB
Pin swapping is enabled on the PCB side. This is performed using one of the following methods:
- Access the Configure Swapping Information In Components dialog (Tools » Pin/Part Swapping » Configure), and enable the Pin Swap option for the required component.
- Access the properties dialog for the PCB component footprint. In the Swapping Options region, enable the Enable Pin Swaps option.
- Select the component footprint in the workspace and enable the Enable Pin Swapping option, using either the PCB Inspector or PCB List panels.
In addition to enabling pin swapping, you must also specify the method(s) used to execute the swapping with respect to the FPGA component on the schematic (in the PCB project). These can be found on the Options tab of the Options for PCB Project dialog (Project » Project Options) and are illustrated in Figure 1.
Figure 1. Define method(s) by which pin swapping is executed on the schematic.
Both options are enabled by default, although it is advisable to disable the Changing Schematic Pins option. Use of this option is more of a 'hardwired' approach and does not lend itself to future updates of the schematic symbol from the source library. The Adding / Removing Net Labels option is far more suited to FPGA components and essentially just means that net labels are swapped, rather than the pins themselves. (Note that this is only possible provided that connectivity to the pins of the FPGA on the schematic is made using net labels, and not fixed wiring!).