Manual FPGA-PCB Linking - Detection of the FPGA Component on the Schematic Sheet

Frozen Content

Modified by Admin on Sep 13, 2017

The FPGA Workspace Map dialog is used to maintain synchronicity between linked PCB and FPGA projects. Access to this dialog is provided by choosing the command of the same name from the Projects menu, or by pressing the button on the Projects panel.

Figure 1 shows an example of how the dialog appears when only the FPGA project exists.

Note: An FPGA project can only contain one physical FPGA device. If the PCB project includes multiple FPGA devices, each of the FPGA sub-projects should be opened in the Projects panel, in order to see the full workspace 'picture'.

Figure 1. FPGA Workspace Map dialog with only FPGA project existing.

When you create the PCB project and the schematic sheet for the FPGA component used is not auto-generated, the FPGA component that is placed on the sheet must be recognized and supported by the software.

The range of supported devices are shown in the Browse Physical Devices dialog (Figure 2). With a Devices view active (View » Devices Views), access to this dialog is made by selecting Tools » Browse Physical Devices from the menus.

Figure 2. Use the Browse Physical Devices dialog to verify device support.

Available (and supported) devices will have a pin number value entered in the main device availability grid as well as information made available in the Selected Device region of the dialog. Devices that do not exist are represented by a hyphen character '-'.

Alternatively click on the Device Support Report button, at the bottom-left of the dialog, to generate a full report (AltiumDesignerDeviceSupport.Txt) listing all physical devices supported by Altium Designer. Devices are listed by vendor and device family. You will be given the option to include or exclude device details (package, pin count, user I/O pins, etc) for the report as required. Once generated, the report will open as the active document in the main design window.

The component placed on the schematic sheet has to be verified against the list of supported devices in some way, before it is recognized and displayed in the FPGA Workspace Map dialog. This is achieved using the Design Item ID field, in the Library Link region of the Component Properties dialog for the FPGA component symbol on the PCB schematic. To be a recognized device, the entry in this field must be identical to that in the Device field for the corresponding device in the Browse Physical Devices dialog (Figure 3).

Figure 3. The placed component is verified using its Design Item ID.

With Altium Designer Release Winter09 a new possibility to was added.
Altium Designer's component libraries are already setup to use this information, the FPGA component detail is looked up in a database based on the component library name, for example XC3S1500-4FG676C. For new components, the part can either be named in the same manner, or a parameter called NexusDeviceID can be added to the schematic component, with the same data. Altium Designer will then be able to look up the new component in its database of FPGA parts.

Once recognized as a supported device, the FPGA component on the schematic sheet and PCB (if it exists at this stage) will be displayed in the FPGA Workspace Map dialog, as shown in Figure 4.

Figure 4. FPGA component recognized in PCB project (schematic and PCB).

As can be seen in Figure 4, the two projects exist, but they have yet to be linked. The entry No linked configuration is displayed under the FPGA project's entry in the dialog. Indeed, it is the use of a configuration that supplies the key when linking the projects.