Interfacing to the TASKING Tools
The TASKING Pin Mapper provider extension provides bi-directional communication between Altium Designer's PCB Editor and your TASKING toolset's Pin Mapper tool. This allows you to interactively perform pin-swapping within the Altium Designer PCB design workspace, and dynamically synchronize changes with your TASKING Pin Mapper tool. This ensures that your TASKING embedded source code is kept in-sync, without the need to export and import change files.
TASKING Pin Mapper Wizard
To synchronize pin mapping data from your microprocessor design - designed using your TASKING toolset - to your PCB design project in Altium Designer, without the need for transferring such data by hand, and therefore removing the need for exporting and importing files manually, the TASKING Pin Mapper wizard is used. The wizard facilitates data synchronization from the TASKING toolset’s own Pin Mapper to an Altium Designer schematic document. The resulting schematic document will reflect the device pin configurations that have been assigned and saved in a nominated Pin Configuration file (*.pincfg).
The TASKING Pin Mapper wizard is accessed from the schematic editor by choosing the Tools » Tasking Pin Mapper command from the main menus.
The following pages of the wizard lead you through the process of creating a schematic from a specified TASKING Pin Mapper file.
Select the TASKING Pin Mapper File
Use this page of the wizard to specify the source pin configuration file (*.pincfg) to be used - this is the file generated from the TASKING toolset’s Pin Mapper.
Select Component
This page of the wizard will, if possible, populate with available options for the processor device.
If the Tasking pin mapper file has specified an explicit processor type, the system will attempt to locate it in the available Altium Designer libraries. Alternatively, if the pin file defines a processor family (say, the ST Microelectronics STM32_T2 family of ARM Cortex processors) the list will contain all compatible types from the Altium Designer library - select the desired processor variant from the list.
The processor list will be blank if a compatible processor library is not loaded or available in Altium Designer. Use the Install library button to locate and install a suitable Integrated library.
To select a different processor from that offered by the list, use the Other component button to open the Browse Libraries dialog. Select the desired library from the Libraries drop down menu and choose a suitable processor component from the list.
Configure the Sheet
This page of the wizard defines the properties and behavior of the generated processor schematic.
Since the source pin mapper file defines both the pin functionality and external connections, its representative schematic needs to be configured to present that information in a way that is compatible with the target PCB design project. As such, this means basic name settings through to how pins, ports and compiler directives are handled.
Place
This, the final page of the wizard, provides a summary of the selected settings. After clicking the Finish button, the new processor schematic document is added to the current project and opened in Altium Designer's schematic editor. The schematic will contain your microprocessor, with all of your original pin signal names and configurations.
TASKING Pin Net Swapping
A component pin is swappable with another pin in that component when both pins have the same Pin Group. The swapping feature supports more than just pins; it also supports swapping a partially routed net. This is ideal if you are working on a dense board and escape routing from the components at both ends of a connection. When you perform a pin swap any connected routing is also swapped to the target net.
The PCB editor includes commands to interactively perform pin-swapping within the PCB design space, and dynamically synchronize changes with your TASKING Pin Mapper tool.
- The Tools » Pin/Part Swapping » Interactive TASKING Pin/Net Swapping command accessed from the main menus of the PCB editor is used to interactively perform pin-swapping within the PCB design space. After launching the command, everything in the PCB workspace is masked (faded) except those pins that are swappable. Keep an eye on the Status Bar. It will prompt you for the next action: Choose Sub-Net to move. After clicking on a swappable pin, you will be prompted to choose a target net for the sub-net to swap. All possible target pins that can be swapped will be highlighted. Click on the target pin to complete the swap action. You will then be ready to perform another pin swap, if required.
- The TASKING PinSwap command accessed from the PCB editor by right-clicking over the required pad of a component and selecting the command from the context menu is used to interactively perform a single pin swap for the component pin (pad) currently under the cursor. After launching the command, everything in the PCB workspace is masked (faded) except those pins that are swappable. Click on the target pin to complete the swap action.
As you make pin swaps within the PCB document, those changes are passed dynamically to your TASKING Pin Mapper tool, courtesy of the bi-directional communication support provided through the TASKING Pin Mapper Provider software extension. This ensures that your TASKING embedded source code is kept in-sync without the need to export and import change files.