The Altium Designer Pin Mapper dialog allows you to create a link between an external pin file (such as one exported from FPGA or Microcontroller (MC) tools) with a schematic component, and then compare the pin signals between those two domains (FPGA and PCB).
As a result of this pin comparison, any changes or updates in the external pin file can be transferred to the schematic, or the pin data from the schematic can be passed back to the pin file. The main purpose for using the Pin Mapper is to obtain additional information about component pins from external tools (particularly FPGA and MC), so this data can used for Pin Swapping in the Configure Pin Swapping dialog. It replaces the need to manually transfer pin data between the two domains.
Currently, the Altium Designer Pin Mapping feature directly supports two FPGA vendors – Altera and Xilinx. The intention is to expand this vendor list in the future. Also supported is Altium's own Pin Info file format, which can be used as a FPGA/MC pin description for any third party FPGA tools, or for other types of components.
Source Pin data file from FPGA tools
For Altera Quartus® II v13.1:
Open project in Quartus.
Select Assignments » Pin Planner.
Select File » Export and save csv file for use in Altium Designer.
For Xilinx Vivado® 2017.4:
Open project in Vivado.
Select File » Export » Export I/O Ports.
In the Export I/O Ports dialog, specify csv as type of I/O port to generate, and click OK.
Access FPGA/MC data from the external pin file in Altium Designer:
Right click on a schematic component part and select Pin Mapping from the context menu, which opens the Pin Mapper dialog.
The Pin Mapper dialog contains the following parts (see image labels):
Shows the file name and path of the source FPGA/MC pin file. The link is established through the file browser ().
The Pin Table, where source pin assignment changes can be found and applied to the Schematic component, or back.
The Footprint preview, where the selected pins are highlighted and pins can be displayed by groups (Bank Number, IO Pins, etc)
The Component Part Selection, which filters the table by part. This also indicates if a part is placed on the schematic, and if each part is synchronized to match the external file data (see details below).
Choose an external pin file in the Pin Mapper dialog:
Click the button to browse to and select a pin file from a local drive. Only temporary Xilinx or Altera Pin files (*.csv) can be selected.
Depending on the previous action, the Pin Mapper dialog will offer solution options for each pin:
(Synced) – Pins net names are synchronized, no changes are required.
(Update Pin File) – Transfer net name from the schematic to the external FPGA pin file (which is updated).
(Update Schematic) – Change the schematic net name to match the Signal name in the external FPGA pin file (schematic is updated).
(Ignore) – Reject changes, no updates will be performed.
(Warning) – There is a non-critical difference in pin name matching between the schematic and external (FPGA) file. If desired, select an update option (or Ignore) from the drop-down menu.
(Fatal Error) – There is a critical difference in pin name matching between the schematic and external (FPGA) file. Note that this Fatal Error must be resolved before making any updates.
Choose the appropriate action from the icon drop-down menu for each entry (row) in the table and select Apply.
When the action is selected, net names from the Schematic will be copied to the Signal names in the FPGA pin file – the source csv pin file is rewritten.
When the action was selected, net labels in Schematic will change to match to the source FPGA Signal names.
Note that the right-click menu for a table entry offers a range of bulk selection options for pin name updates.
The dialog's Part Selection allows the pins that are listed in the mapping table to be filtered by the selected Part. You can also check for Parts that are not placed in the schematic, and Parts that are not synced with the external FPGA file (red indicator).
If there are multiple component parts linked with the external file, the Pin Mapper dialog allows you to switch between options for this kind of component.
If there are pins where different net names are assigned in the Schematic and FPGA sides, then this can be checked in an ERC where they are displayed as violation in the Messages panel (not yet implemented).
If you would like to start the work flow with a FPGA pin file from the schematic side, then an Altium Pin Report file can be generated – select the Export button in the Pin Mapper dialog.
Currently, only general pin parameters can be copied, however support for more advanced data such as Swap group etc is planned. Swapping must be defined manually at the moment by importing changes from the FPGA pin file data.
Since the external pin file is linked to a component, a new component model (Pin Info) is created and shown in the Models list in the Component Properties panel. In the future, this will provide an easy way to add FPGA pin data to a Library component. The panel's Models section also allows the Pin Info to removed or modified.
When a component has model Pin Info, additional pin parameters and options will be available for that component in the Configure Pin Swapping dialog.