Netlist Manager

The Netlist Manager dialog.

Summary

This dialog allows the designer to effectively manage the netlist for the board. Nets can be added, edited, or deleted as required, and the pins (or rather pads) of the components in those nets, can be edited with respect to their properties also. 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.

Access

The dialog is accessed from the PCB Editor, by using the Design » Netlist » Edit Nets command, from the main menus.

Options/Controls

• Nets In Board - this region of the dialog presents all of the nets defined for the board, by their name. Use the mask field above the list to quickly filter the latter's content.

• Edit - click this button to access the Edit Net dialog, from where you can view and modify, the properties of the currently selected net (or focused net, where multiple nets are currently selected in the list. The focused net is presented with a dotted border).
• Add - click this button to add a new net for the board. The Edit Net dialog will appear in which to define the properties of the net. The initial, default name for the new net will be NewNet, change this as required.
• Delete - click this button to delete the currently selected net(s) from the board. A confirmation dialog will appear, simply click Yes to effect the removal.

• Pins In Focused Net - this region of the dialog presents all of the pins (component pads) associated/belonging to, the currently selected/focused net. For each entry in the list, the identifier for the pin is shown in the format <ComponentDesignator>-<PinDesignator>. Use the mask field above the list to quickly filter the latter's content.

• Edit - click this button to access the Pad dialog, from where you can view, and modify, the properties of the currently selected pin (pad).
• Menu - click this button to access a menu offering the following commands:
  • Add Net - use this command to add a new net for the board. The Edit Net dialog will appear in which to define the properties of the net
  • Delete Net - use this command to delete the currently selected net(s) from the board. A confirmation dialog will appear, simply click Yes to effect the removal.
  • Update Free Primitives From Component Pads - use this command to resynchronize the net name of the routing primitives to the net name on the pads they connect to. After launching the command, a confirmation dialog appears asking whether you wish to update free primitive nets with the component-pad nets. After clicking Yes, starting from each pad, the connected copper is selected and the net name of each primitive set to match that of the pad.

• Clear All Nets - use this command 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. 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 will be removed. Any routed track will remain routed, but will have a No Net assignment. Any unrouted logical connections will be removed.
• Export Netlist From PCB - use this command to export to file, the internal PCB netlist for the current document. After launching the command, a confirmation dialog will appear asking if you wish to export the netlist from the PCB. After clicking Yes, a netlist (Exported <PCBDocumentName>.Net) is created in the same folder as the PCB design document.
• Create Netlist From Connected Copper - use this command to create a netlist file, based on the connectivity created by the routing in the current design. After launching the command, a confirmation dialog will appear asking if you wish 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.