PCB_Cmd-NetlistNetlist_AD

Applied Parameters: Action=EditNets

Summary

This command is used to run the Netlist Manager dialog in which you can manually edit the current internal netlist for the document.

Access

This command can be accessed from the PCB Editor by:

• Choosing the Design » Netlist » Edit Nets command from the main menus.
• Pressing O in the main design workspace to access the Options pop-up menu, and choosing the Edit Nets command.

Use

After launching the command, the Netlist Manager dialog will open. Use this dialog to edit the internal netlist for the current document as required.

Nets can be added, edited, or deleted as required, and the pins (or rather pads) of the components in those nets also can be edited with respect to their properties. Access to other netlist management tools is also provided through this dialog, including the ability to create the netlist based on connected copper on the PCB and the ability to export the netlist from the PCB.

Tips

1. The properties of a net are edited through the Edit Net dialog.
2. The properties of a component pad associated to a chosen net are edited through the Properties panel.

Applied Parameters: Action=UpdateFreePrimitiveNets

Summary

This command is used to resynchronize the net name of the routing primitives to the net name on the pads to which they connect.

Acces

This command is accessed from the PCB Editor by choosing the Design » Netlist » Update Free Primitives From Component Pads command from the main menus.

Use

After launching the command, a confirmation dialog opens asking whether you want to update free primitive nets with the component-pad nets. After clicking Yes and starting from each pad, the connected copper is selected and the net name of each primitive is set to match that of the pad.

Tips

1. This operation does not affect the internal PCB netlist.

Applied Parameters: Action=ClearAllNets

Summary

This command is used to clear all nets from the current design document, essentially flushing the internal PCB netlist. This may be desirable if you have changed net information in the source schematic documents and you want to fully resynchronize your PCB with the source schematic netlist information.

Access

This command is accessed from the PCB Editor by choosing the Design » Netlist » Clear All Nets command from the main menus.

Use

After launching the command, a confirmation dialog will open alerting you to the fact that this operation will clear all net information from the PCB. After clicking Yes, all net information will be removed. Any routed track will remain routed but will have a No Net assignment. Any unrouted logical connections will be removed.

Tips

1. You can verify that all nets have been cleared from the design using the Netlist Manager dialog. You will see that the Nets In Board listing is empty.

Applied Parameters: Action=ConfigurePhysicalNets

Summary

This command is used to run the Configure Physical Nets dialog. This dialog allows you to examine and confirm that the objects that are physically connected have the correct net assigned in that physical net.

Access

This command is accessed from the PCB Editor by choosing the Design » Netlist » Configure Physical Nets command from the main menus.

Use

After launching the command, the Configure Physical Nets dialog will open. The software analyzes the design, checking that all pads and the objects that physically connect them together (tracks, arcs, fills, etc.,) have the same net name assigned. When all net objects are correct, the net is shown in green. If any objects are detected as touching but have a different net assigned, they are flagged in red. A common example of when this can occur is if a component footprint has extra copper objects within the footprint. When this footprint is loaded during synchronization, the pads have the assigned net name applied to each pad but not the extra copper.

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.

The Action region of the dialog provides controls for specifying the action needed to be taken to resolve issues with the connected copper. By default, actions will be set automatically but can be adjusted as required. Once the actions are set, click the Execute button to update the net assignments.

Tips

1. A physical net means connected copper in this instance.

Applied Parameters: Action=CreateNetlistFromConnectedCopper

Summary

This command is used to create a netlist file based on the connectivity created by the routing in the current design.

Access

This command is accessed from the PCB Editor by choosing the Design » Netlist » Create Netlist From Connected Copper command from the main menus.

Use

After launching the command, a confirmation dialog will open asking if you want to generate a netlist from the copper on the PCB. After clicking Yes, a netlist (Generated <PCBDocumentName>.Net) is created in the same folder as the PCB design document and automatically opened as the active document in the main design window.

Each net in the netlist gets its name from one of the pads to which the routed copper connects.

Tips

1. The netlist will be added to the Projects panel as a free document under the Source Documents sub-folder.

Applied Parameters: Action=CleanUpNets

Summary

This command is used to clean all routed nets for undesired duplicate (stacked) track segments.

Access

This command is accessed from the PCB Editor by choosing the Design » Netlist » Clean All Nets command from the main menus.

Use

After launching the command, a confirmation dilaog opens asking if you want to clean-up nets. Click Yes to analyze all nets and resolve all instances of stacked track segments with the redundant segments being removed.

Tips

1. The Autorouter initiates this command automatically after it has finished routing.
2. The command will only work on stacked track segments that are identical in their properties (i.e. same layer, same width, etc.,).

Applied Parameters: Action=CleanUpSingleNets

Summary

This command is used to clean individually routed nets for undesired duplicate (stacked) track segments.

Access

This command is accessed from the PCB Editor by choosing the Design » Netlist » Clean Single Nets command from the main menus.

Use

After launching the command, the cursor will change to a cross-hair and you will be prompted to choose an electrical object (pad, track, etc.,). Position the cursor over an electrical object that is attached to the net you want to clean then click or press Enter. The net will be analyzed and cleaned with any redundant segments being removed.

Continue cleaning additional routed nets in the design or right-click or press Esc to exit.

Tips

1. The command will only work on stacked track segments that are identical in their properties (i.e. same layer, same width, etc.,).