Tutorials, news, snippets, and other various musings about the electrical engineering industry.
How to Perform Signal Integrity Analysis on Nets in OrCAD PCB Designer Professional
Starting in 16.5 and continuing to the present version (16.6), you can perform signal integrity (SI) analysis from your OrCAD PCB board file using only your OrCAD PCB Professional license (no special SI licenses needed!)
First you need to set up some SI parameters for your board, specifically for the nets that you want to analyze. To invoke this setup routine, in OrCAD PCB Editor, go to Setup > SI Design Setup. This will present you with a dialog allowing you to choose what you'd like to configure.
Normally, unless you know you’d only like to look at a single category, it’s not a bad idea to leave everything checked.
The first dialog that you will encounter after hitting Next is important as it allows you to pick the nets that you’d like to set up for SI analysis. Pick the nets you are interested in analyzing instead of leaving everything selected so that you won’t have to set up every component and net in the design.
Use the wildcard search to find your specific net(s) in case your overall list of nets is long making scrolling difficult. You can use the question mark (?) for a single wild card character and the asterisk (*) for an any length wildcard in the Xnet Filter.
After clicking Next through a few library configuration screens, you can set up power and ground given the suggestions that the tool gives you based on the net names and pin types that the nets are connected to.
Just before models are assigned to components, the setup tool wants to know what types of components it is managing. In the Setup Component Classes screen, you need to define what types of components you’re dealing with, where:
- IC is an active device (usually U?)
- IO is a connector (usually J?)
- Discrete is a passive device (usually R?, C?, L?)
Now that the components are assigned to their correct class, you can assign some model to them. All the discrete devices are taken care of easily by choosing the “Create Default Models For All Discretes” button.
The remaining devices can be chosen and assigned an existing model (if you have downloaded one from the internet) or a new model can be created for it.
Once your models are defined and attached to the component, you can hit Next to finish out the Setup Wizard.
- If you’d like to set default library paths or add new libraries, you can go directly to that function in the PCB tool by choosing Analyze > Model Browser.
- If you’d like to change model assignments on the parts in your design, you can get there directly by going to Analyze > Model Assignment.
- If you’d like to change any other defaults choose Analyze > Preferences.
Now that the models are all hooked up, we can go and do some SI analysis on our net; to do this, go to Tools > Topology Extract. In this window, you only need to select the net that you’d like to take a look at and if you want to extract the real physical traces or not.
You can select the net by scrolling through the list, using the filter to shorten the list or you can simply click on the net in the board itself behind the dialog box. Ticking off “Include Routed Interconnect” will also include accurate models of the physical traces and vias from your board instead of ignoring them.
Once that’s all selected, choose the View button to bring an SI representation of the net over to the SigXplorer tool.
The SigXplorer tool which is using your OrCAD PCB Designer Professional license will open with a copy of your net’s topology. Select the driving pin and right mouse button (RMB) on it and apply a stimulus to it.
After a Stimulus is applied, you can simulate by choosing Analyze > Simulate or by hitting the
button to see the results in SigWave.
That’s all it takes to run a simulation on a net from OrCAD PCB Editor using the OrCAD PCB Professional license that many people already have.