Altium CircuitStudio
...
PCB
Commands
Netlist Tools
Created: December 16, 2024 | Updated: August 23, 2018
Parent page: Commands
Summary
Every PCB design includes an internal netlist that defines the connectivity in the design. As the design evolves and changes are made, it is possible for the internal netlist to no longer match the placed components and routing. CircuitStudio includes a range of commands that can help manage the internal netlist and how it is mapped to the routed board.
Details
Netlist tools are available in the Tools | Netlist group on the Ribbon.
Use the netlist tools to manage the internal design netlist.
Use these tools to perform the functions in the table below.
| Command | Behavior |
|---|---|
| Edit Nets | This command opens the Netlist Manager dialog, where you can Add nets to and Delete nets from the design and Edit the properties of existing nets. Refer to the Netlist Manager dialog page for more information. |
| Clean All Nets | This command is used to clean all routed nets by removing duplicate (stacked) track segments, and breaking track segments at T-junctions and vias, if required. Note that excess stacked segments are only removed if they are the same width and length and are on the same layer. |
| Clean Single Net | This command is used to clean the chosen routed net by removing duplicate (stacked) track segments and breaking track segments at T-junctions and vias, if required. Note that excess stacked segments are only removed if they are the same width and length and are on the same layer. |
| Configure Physical Nets | This command is used to launch the Configure Physical Nets dialog. When the command is run, the entire design is analyzed resulting in a detailed list of every net and with every primitive in that net. The dialog is interactive; click on a net or primitive to cross probe to that object. Right-click or click the Menu button to access the available commands. Note that the dialog can also be configured to Only Show Errors; it may be in this mode if the dialog appears empty. Every pad in the design and its connected copper will be listed as a net. Pads that do not have a net assigned will be assigned a system-generated net name. Use this to resolve errors in footprints that have copper touching pads, but those pads are not used in the current design. Refer to the Configure Physical Nets dialog page for more information. |
| Update Free Primitives From Component Pads | This command is used to re-synchronize the net name of the routing primitives to the net name on the pads to which those primitives connect. After launching the command, a confirmation dialog appears asking whether you want to update free primitive nets from the component-pad nets. After clicking Yes, starting from each pad, the connected copper is selected and the net name of each routing primitive is set to match that of the pad to which it connects. This command is useful after renaming a net in the schematic and updating the change to the PCB since the update process will only update the net names for the pads in the net. It can also be used to assign net names to extra copper added into a footprint. Note that this command does not update copper connected to pads that have no net name (are set to No Net). To resolve this, use the Configure Physical Nets command. |
| Export Netlist From PCB | This command exports the internal PCB netlist to a file that is written into the same folder as the PCB file. The netlist is written out in the Protel format and is automatically opened. The upper section of the netlist details each component; the lower section details the nets and the nodes in each net. |
| Create Netlist From Connected Copper | This command creates a netlist file based on the connectivity created by the routing in the current design. The netlist is written out in the Protel format and is automatically opened. The upper section of the netlist details each component; the lower section details the nets and the nodes in each net. |
| Clear All Nets | This command is used to clear all nets from the current design document, essentially flushing the internal PCB netlist. Use this command when you have changed net information in the source schematic documents and you want to fully re-synchronize your PCB with the source schematic. After launching the command, a confirmation dialog will appear alerting you to the fact that this operation will clear all net information from the PCB. After clicking Yes, all net information is removed from the PCB. Routed tracks will remain routed but will have a net assignment of No Net. Any unrouted logical connections will be removed. Once the PCB has been re-synchronized with the schematic, you will need to run the Update Free Primitives From Component Pads command or the Configure Physical Nets command to re-apply net names to the routing. |