Defining Differential Pairs in Your Schematics
Parent page: Creating Circuit Connectivity in Your Schematics
A differential pair on the schematic can be defined using Differential Pair directives. The two nets in the pair must each be identified by a common Net Label with the suffixes _N and _P, and a directive must be attached to each.
Place a directive of this type by choosing the Place » Directives » Differential Pair command from the main menus. This command is used to place a Parameter Set object onto the active document, preconfigured as a differential pair directive (Label = DIFFPAIR). Each pair of directives (one for the positive net, one for the negative) of this type will yield a single differential pair object when transferred to the PCB.
Place directives on the schematic to define differential pairs. In this example, two differential pairs named V_RX1 and V_TX1 will be generated in the PCB.
On the PCB side, each resulting differential pair object will be added to the default Differential Pair class: <All Differential Pairs>. You can rename differential pair objects on the PCB side only.
If there are a large number of pairs to be defined, an alternate approach is to also place a Blanket directive. This allows you to apply directives to multiple nets that are under the blanket (Altium Designer detects nets whose Net Label hotspot is within the blanket boundary). A single Differential Pair directive is placed to touch the edge of the blanket, as shown in the image below.
The image also shows that as well as directing that the contained nets be defined as differential pair members (via the presence of the Differential Pair directive), the directive also instructs all contained nets to become members of the Net Class RocketIO, the pairs to become members of the Differential Pair Class ROCKET_IO_LINES, and also to create a Differential Pair Routing rule. Because there is a Net Class specified in the same Differential Pair directive, in the PCB editor this rule will be scoped to target the RocketIO Net Class when you transfer the design to the PCB editor.
A Blanket can be used to configure multiple nets as differential pair members, create a Diff Pair Class and Net Class of these nets, and apply a Differential Pair Routing design rule to this Net Class.