Issue link: https://resources.pcb.cadence.com/i/1532919
f Differential Pair ɢ Referenced Intra-DP Spacing CSet - diff pair trace to diff pair trace spacing ɢ Min Line Spacing - the thinnest diff pair trace can be ɢ Primary Gap - the edge-to-edge distance between the + and - diff pair traces during regular routing ɢ Neck Gap - the edge-to-edge distance between the + and - diff pair traces during Neck Mode routing ɢ (+)Tolerance - added trace width on any trace, whether in neck mode or not ɢ (-)Tolerance - the subtracted/minimal gap spacing width, whether in Neck mode or not. Note that the narrowest gap (during neck mode) minus the Tolerance must be equal to or greater than the Min Line Spacing rule/constraint, else you get an error f Vias - vias that are allowed on the differential pair traces f BB Via Stagger - the allowed parameters for blind and buried vias for the diff pair traces ɢ Min - the closest distance between two blind/buried vias ɢ Max - the furthest distance between two blind/buried vias f Pad-Pad Connect - Basically for allowing via in pad connections - typical for tight spacing conditions and via in pad technology f Etch f Ts - T-points - this allows you to make a T-junction between another trace and one of the traces of your diff pair Creating a Diff Pair Before continuing with this example, let's create a differential pair. 1. To create a differential pair: a. Go to the Physical > Net > All Layers worksheet b. Select the two nets you want to pair c. Right-click and choose Create > Differential Pair d. The Create Differential Pair window will appear e. Name the pair and click Create f. You can also remove a differential pair you might have made by mistake by clicking the Clear button g. Once you have created all your differential pairs, click Close 2. At this point, you can create a net class or group within the Physical > Net > All Layers worksheet (follow the instructions in Part 1 on how to create Net classes and groups). 11 www.cadence.com OrCAD X Constraint Management Guide