When entering shematic data in DxDesigner, I would like to hilite an entire net
to ensure that all legs of a net are connected. How do I hilite an entire net ?
A couple of methods.
1. If the net is all one segment, simply selecting a net branch, and then RMB, right mouse button, select net.
2. If the nets segments are separate, and connected with labeling, then use the command line interface and enter sname, and then the labeled name. The dropdown selection will work if the net is labeled. Then change the zoom level (Edit Fit Selected or capital Z on the keyboard) to refresh the screen and highlight the nets. Depending on your settings, rolling the mouse wheel can also change the zoom level.
3. If you have cross probing to another tool, select the net in the other tool and the net will highlight. Cross probing has several settings, to adjust how for opening new pages, setup, settings, cross probing, will adjust the settings.
4. Setup settings, Navigator, allow viewing of nets and buses. and select the net using the Navigator pane and then Fit Selected.
5. Use the Find Replace Dialog, select More, search for the name of the net, look within the board level and details select net, names only.
6. For another tool dialog, File Export CCZ (or PDF) and use the free VisECAD schematic viewer. The VisECAD tool is really cool and will show exactly which nets are connected to what pins even tracing down through the hierarchy. It is available here http://www.mentor.com/products/pcb-system-design/fabrication-assembly-test/visecad/visecad-evaluation
Retrieving data ...