Issue link: https://resources.pcb.cadence.com/i/1533024
The pin pairs are the way to choose the first and last pins where there are intermediate pins that would separate those two pins into different nets. The example I use is the series element that is inserted in a controlled length line breaking it into two nets that are considered one link in terms of length matching. Figure 5. Adding a pin pair is invoked with a right mouse click on a net in the same column as Figure 3. Instead of Analyze, it's Create > Pin Pair and it pulls up this window where the pins of a net are listed twice for selection as potential the start and end points. Your selection is based on the terminal locations of the net, usually first and last stop. Let's say you have a diff-pair where one net has a shunt element at the connector where the other net does not. Then, you would Include the endpoints that would allow phase matching without including the stub. Using Two Match Groups Rather Than XNets Take a bus where all of the data lines have a series resistor in the path between A and B. If you don't have the high-speed option and you still want to bridge across the component to find a total length of two nets, it is still possible to automate that to some extent. The easiest way to do that is to make sure both sides are independently matched. Try strategically placing the series elements so that one side of the connections lends themselves to a natural length matching. If all of them end up routing to a length of say three millimeters, then all you have to do is make a match group out of the nets on the other side of the resistors or whatever is breaking the chains. In terms of maximum length, you still have to account for the 3 mm used for the fan-out to the resistors. When two nets are used for a connection where the maximum length is provided as a single value, I like to enforce that with the old school Total Etch Length. This is the one electrical property I used before learning about Relative Propagation Delay. In the example above the short lines of the workaround x-net group would be given a Total Etch Length of 3mm on one leg and the rest of the allowable length on the other side of the resistors as they go longer. The issue is that you are sharing the length tolerance between the two sides so try to really nail those 3 mm segments. 5 www.cadence.com Controlling Trace Length for Digital Circuits Using OrCAD X and Allegro X Tools