How to put an area of net names into the same class

Here is a quick way to put an area of net names into the same class for net spacing rules and physical rules using Constraint Manager for Capture.

The Legacy (Slow) Way

But first I want to show you the slow way one needed to set constraints and classes. Let’s say you have a schematic design and want to define the spacing for specific nets before PCB layout. In earlier versions of OrCAD, this could take at least 10 minutes to set your desired properties. You used to have to:

  1. Look up a list properties in PCB Editor with specific strings, like NET_PHYSICAL_TYPE and NET_SPACING_TYPE (at least 2 – 10 minutes)
  2. Select the nets manually in Capture (2 – 5 minutes)
  3. Use Ctrl+E to edit the properties for those nets (assuming you found all of them),
  4. Create a new property field for each property you want to add
  5. Enter the string that matches the exact net spacing property in PCB Editor’s Constraint Manager tool (copied from step 1)
  6. Finish and save the design, then
  7. Cross your fingers and hope your changes translate correctly when you net list into PCB Editor

As you can obviously tell, this is a long process just to add some properties. While you can still use the above method, Cadence has created a much better way.

The Fast Way (Using Constraint Manager within Capture)

OrCAD Capture now has Constraint Manager embedded into it. This means you can drive your PCB design rules directly from the schematic phase. Here’s the quick way to put net names into the same class for spacing and physical rules in your PCB design.

Have your design open in Capture (go to File – Open – Demo Designs – High Speed FPGA Board Demo and click Open)

High_Speed_FPGA_Board_Demo

Then you can drill down into the Power Supply block and open its circuit

In earlier versions of OrCAD, you needed to open PCB Editor to access Constraint Manager. That is no longer needed though, because we can open Constraint Manager directly from Capture!

Open Constraint Manager (CM) from Capture

So go to Capture menu Tools option, then select Constraint Manager (CM). You may get a prompt with a high-level overview of CM’s features so click OK. Then you would choose the first option (to open CM from Capture).

Then CM will open. Go to the Spacing – Net – All Layers section where you can see all the nets in your design.

Normally you can select any net by name, but what if you don’t know all the net names?

Select Your Desired Nets

You can instead, visually select all the nets you want and they will be highlighted in CM. So select some nets in Capture on your schematic

select desired nets from your schematic

Notice that the nets you chose graphically are auto-select in CM as well. And really who’s going to remember net name “N9903369”?

Nets selected in Capture get highlighted in constraint manager

How to put an area of net names into the same class

Okay with your nets selected, right click any highlighted net name in CM, then choose Create – Class…

Create a new net class

In the Create Net Class window, you can name the new class whatever you like (POWER_20MIL for example). Be sure to check mark “Create for both physical and spacing”. This sets the spacing and physical to be the same value.

Set the physical and spacing in a net class to 20 mils for power

Click OK. Notice that CM even prompts you to let you know if a net is already a member of another class. It also asks for your confirmation on whether it is okay to move it to your new class.

New Class window prompts you to re-classify nets for PCB

Then if you say OK, CM will commit your changes. This ability to move forward is powerful, because the design change is not a show-stopper, saving you some time.

Constraint Manager sets net class with physical and spacing rules

See the changes have been committed!

Continue Working on Your Design

With Constraint Manager as part of Capture, your PCB has the rules you need to pass Design for Manufacture. Now that’s true integration!

Learn More…

If you would like to learn more about OrCAD, you can go through the Help section. There, you can find all of Cadence’s documentation. You can also bookmark the website as we are the latest resource or OrCAD information. You can also come back to this blog and find new solutions common obstacles using OrCAD, PSpice or Allegro.

If you want full step-by-step video tutorials to build your own PCBs, enroll in a monthly membership and start your lessons today!

Free Info-graphic

Download our info-graphic on the high-level phases every PCB design goes through from start to finish.

Processing…
Success! You're on the list and will receive your download.