Altium Designer 文档
...
对话框参考
Dialogs((M to R))_AD
PCB_Dlg-NetlistManagerNetlist Manager_AD
Created: 九月 28, 2017 | Updated: 二月 21, 2018
| Applies to versions: 18.0, 18.1, 19.0, 19.1, 20.0, 20.1, 20.2 and 21
您正在阅读的是 20. 版本。关于最新版本，请前往 PCB_Dlg-NetlistManager((Netlist Manager))_AD 阅读 22 版本
The Netlist Manager dialog
Summary
The Netlist Manager dialog provides controls to effectively manage the netlist for the board. Nets can be added, edited or deleted as required, and the pins (or 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.
Access
The dialog is accessed from the PCB editor by clicking Design » Netlist » Edit Nets from the main menus.
Options/Controls
- Nets In Board - this region of the dialog presents all of the nets defined for the board by name. Use the mask field above the list to quickly filter the content.
- Edit - click to access the Edit Net dialog in which you can view and modify the properties of the currently selected net (or focused net, when multiple nets are currently selected in the list. The focused net is presented with a dotted border).
- Add - click to add a new net for the board. The Edit Net dialog opens in which you can define the properties of the net. The initial, default name for the new net is NewNet; change as required.
- Delete - click to delete the currently selected net(s) from the board. A confirmation dialog will appear; click Yes to continue with the removal.
- Pins In Focused Net - this region 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 content.
- Edit - click to access the Pad dialog in which you can view and modify the properties of the currently selected pin (pad).
- Menu - click to access a menu offering the following commands:
- Add Net - use to add a new net for the board. The Edit Net dialog opens in which you can define the properties of the net
- Delete Net - use to delete the currently selected net(s) from the board. A confirmation dialog will appear; click Yes to continue with the removal.
- Update Free Primitives From Component Pads - use to resynchronize the net name of the routing primitives to the net name to which the pads they connect. 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 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 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 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 which automatically opens as the active document in the main design window.