In OrCAD PCB Designer how do I get the trace width of a signal
The information displayed by OrCAD depends on your current "Application Mode" ("general", "etch", "placement", etc) and the options you have selected in the "Find" dialog.

This is difficult to explain; let me show you some screenshots. Let's assume you are in "general edit" mode.




Starting with everything in the "Find" dialog selected (notice the red rectangles):



In this case, when you highlight a trace, the entire net becomes highlighted. Your "Show Element" window describes the entire net, and the mouse-hover text is net-specific. It is possible for this net to have many different trace widths, so OrCAD doesn't show that information.





But you don't want to know about the entire net, so uncheck "Nets" in the "Find" dialog (again, see the red rectangles). Now OrCAD won't select nets. Its next priority would be to select a "Connect Line":



Now, the connect line (or "CLine") is highlighted. You can't see it in my screenshots, but the selection includes the entire trace from one connection point to another. The selection stops when the trace hits a via, another component pad, etc. As before, the Connect Line may have varying trace widths, so the information isn't displayed.





Finally, uncheck "CLines" in the "Find" dialog. This causes OrCAD to ignore entire CLines, and so it will start selecting individual segments ("CLine Segs):



Now selecting a trace only highlights that one line segment. This is what you are looking for. The information displayed is for that one segment of copper, and the width is available.




This example starts with all options selected, and then successively removes them. It is actually easier to simply click "All Off", and then check only the "Cline Segs" box. But I wanted to demonstrate how OrCAD prioritizes the "Find" dialog options.