Routing Differential Pairs in PCB Schematics with Altium Designer

Created: December 21, 2018
Updated: August 5, 2020

Blue IC in tweezers

Working with routing tools in your PCB design software can be a huge time saver. When you have a simple board with a small number of components, it’s fine to route by hand, but routing components like connectors or FPGAs with a large number of connections can take a huge amount of time. Automated routing, pin swapping, and part swapping tools make it easy to route all of these connections quickly while still working within standard PCB design rules.

If you’re working with a high speed device, you’ll need to route differential pairs between components if you want to reduce crosstalk and eliminate mode electronic noise in these sensitive signal lines. When you’re working with a large number of components with tight spacing requirements, using an auto router of differential pairs can be a huge time saver. All of these features need to operate within your PCB design rules.

Working in a PCB design software package that unifies your routing, layout, and simulation tools in the same rules-driven design engine ensures that your designs will meet the basic rules that ensure PCB functionality. That way, you know technical details like managing impedance and trace lengths are handled in the background. You’ll also be able to define custom design rules that are critical for your application. Other design software packages claim to unify these features, but they still separate these features into different programs or force you to use a third party program to finish basic design tasks.

Defining Differential Pairs in Your Schematic

When you need to use differential pairs in your device, you’ll need to define which nets will use differential signalling to interface with your components. Simply placing a net is not enough, a net needs to be specifically called out as being part of a differential signal. The schematic and layout editor in Altium Designer® include net definitions functions, and you can define differential pairs within a signal net. First, you’ll need to select some components that will communicate with each other, place them in your schematic, and define which ports will use differential signalling.

Here, we have three objectives:

  1. Define differential pairs in the schematic;
  2. Setup impedance and routing rules for our differential pairs;
  3. Start differential pair routing in the PCB layout.

To get started, we’ll look at the schematic below and define the differential pairs we need to use create our differential signal. This schematic contains a Microchip LAN9514I-JZX USB/Ethernet Controller, an edge connector, and a few shielded USB connectors. These component can be found in the Manufacturer Part Search panel within Altium Designer. For brevity, we’ll only look at “Part A” from this pin list, labeled with the designator “U1A” on the schematic. Some of the outputs will be connected to the board edge connector, and other nets will be routed to USB connectors.

A simple schematic for differential pair routing in Altium Designer

USB/Ethernet controller and some connections in Altium Designer

Note that, in this schematic, I've defined the USB outputs as differential pairs with a special directive symbol. you can specify which connections are differential pairs by clicking on the “Place” menu. Highlight the “Directives” option and select “Differential Pair”. You’ll be able to place the directive symbol on the connections you want to function as differential pairs. Simply select all nets that will be part of a differential pair.

Next, each half of a differential pair is defined as positive or negative using its net name. The positive end must be named using “_P” at the end of the net label, and the negative end must be named using “_N”. I've done this for the USB1-USB3 lines in the above schematic. We can do the same for the RX lines in the lower left portion of U1A. Note that these would normally be connected to a magnetics and Bob Smith termination circuit before being routed to an RJ45 connector, but we'll just use the simple situation above to illustrate differential pair routing.

Which Classes to Define?

Routing your differential pairs successfully requires setting up Differential Pair Classes and Net Classes. The goal here is to group multiple pairs together so that the same design rules can be applied to all pairs in the group. This group is a Differential Pair Class, and you'll apply geometry requirements and length matching requirements in the Design Rules editor.

Since we need to define a Differential Pair Class, we’ll add this to each directive. I’ve defined classes USB1 o USB 3 for each of the connections shown in the schematic. If you double click on the directive symbol, you’ll be able to define classes and design rules for a connection in a differential pair. You can also right-click on the directive symbol and click on “Properties”. This will bring up a dialog that allows you to specify a label, classes, and rules for a differential pair. Here, we will add the “Diff. Pair Net Class” to each pair and assign a class name for this net. This is shown below for USB1_P.

Defining differential pair design rules and constraints in Altium Designer

Defining a differential pair net class

You'll also need to add design rules to this directive. This can be done within the dialog shown above to apply a design rule to an individual net. If you want to do something like length tuning for a differential pair, or for a group of differential pairs, it's better to do this in the PCB Editor. If you create a rule from the above dialog, a new design rule will be created that only applies to this net. Since we want to apply length matching to individual USB1 to USB3 connections, we can just define the Differential Pair Classes shown above and wait until the schematic is captured to set a design rule for these nets.

Routing Differential Pairs in Your Layout

Define an Impedance Profile

Before you capture your schematic and start routing, you need to create a new PcbDoc that includes an impedance profile for your differential pairs. For this simple example, I've created a 4-layer PCB with a single-ended impedance profile (50 Ohm, named S50) and a differential pair impedance profile (90 Ohm, named D90). The differential pair impedance profile will be used for the USB lines as these need to have defined differential impedance. You can do this through the Layer Stack Manager within the PCB Editor. My stackup and impedance profile are shown below:

Impedance profile in differential pair routing

Defining an impedance profile for differential pair routing

Defining Design Rules: Single Pairs

At this point, we can capture the schematic as a layout and route the differential pairs we defined. I’ve defined differential pairs for the rest of the connections between the FPGA and the connector. First, add a new PCB to your project and capture your schematic. You can do this by opening your empty PCB and clicking the “Design” menu, followed by “Import Changes From…”. Note that a Room will be created by default unless you uncheck the option in the Engineering Change Order dialog.

Before routing, we need to define design rules for the differential pair nets in our schematic. This is done by opening the Design -> Rules dialog in the PCB Editor. Here, we need to define the following rules for these nets to comply with the USB specification:

  1. Length tolerance: 2 mil (found in the High Speed -> Matched Lengths entry)
  2. Differential pair routing constraints: defined by impedance profile (found in the Routing -> Differential Pair Routing entry)

When you define the design rules for these pairs, you can create a rule for each net and select the impedance profile you want to use. This is shown below.

Defining differential pair rules in Altium Designer

Defining design rules for individual nets

Defining Design Rules: Multiple Pairs

Since we're working with multiple differential pairs that all need the same design rules, a better option is to create a single design rule that applies to our Differential Pair Class. To check and create classes, open the Design -> Classes dialog in the PCB Editor. Go down to the Differential Pair Classes entry, right-click, and create a new class. As long as you defined your differential pairs correctly in the schematic, you can now add these pairs to your new class. This is shown in the image below.

Classes in differential pair routing

Defining a class for a group of USB differential pairs

Now, you can go to the design rules editor and select the net class you just created for the length tolerance and routing constraints, just as was done for individual nets. Under the "Where The Object Matches" entry in the design rule window, select the Differential Pair Class you defined in the above window. The design rule will now apply to all nets in the class. This includes the impedance profile you defined in the Layer Stack Manager as long as you select the option in the design rule window.

Capture and Route

Now it's time to import changes from the schematic and start your layout. We've done a lot of work on the front-end to get to this point, but this will ensure that all lines in the layout have consistent impedance, spacing, and length matching rules as the pairs are routed. Once you've arranged the components the way you want, simply select the Interactive Differential Pair Routing option at the top of the PCB Editor window.

The image below shows the component we want to work with in mid-route. When you use the interactive router, you only need to click on one end of the net, and both traces will be routed in tandem as you move across the board.

Mid differential pair routing in a PCB layout.


If you ever need to route around an obstacle, such as another component, the router will automatically place traces around the obstacle. To illustrate, a resistor has been placed in the routing path as shown below. As the traces approach the component, they'll be automatically placed around the component with the tightest possible clearance. You can then click on the far side of the component to set your routing around the component, and you can continue routing towards the destination. Your design rules for the maximum uncoupled length and obstacle avoidance will be followed here as you move around the component.

Differential pair routing around an obstacle.


For more complicated components, such as BGA with high ball count, you'll need to use a fanout strategy to create connections for your traces, or you'll need to use some creative layout options to ensure all your connections are routeable. For a high ball count BGA, you might also need to use pin and differential pair swapping to clean up any overlapping nets before you start routing. This will help eliminate excessive use of vias on the differential lines.

Next Steps: Length Tuning and Signal Integrity

The image below shows two routed differential pairs. This is a quick and easy process thanks to the interactive routing tools in Altium Designer. At this point, you can apply length tuning to each pair, or across multiple pairs. Take a look at this article to see how to apply length tuning to differential pairs.

Finished differential pair routing

Finished differential pair routing in Altium Designer

You could also use the xSignals package to examine signal integrity for these nets, or for a group of nets. Examining a group of nets requires defining an xSignals class from the Design -> Classes dialog, just as was done for creating a Differential Pair Class. This allows you toe examine the rising and falling edges of signals, and any overshoot/undershoot. Other high speed design rules can be applied to this layout inthe same way as was done for length tolerance and differential impedance. The design rules shown here are the key to quick and easy differential pair routing.

Altium Designer unifies information in your design with your routing tools, ensuring that your next device will function as intended. The integrated environment in Altium Designer allows all your tools to communicate using the same rules-driven design engine. The best schematic, CAD, simulation, and routing tools are exactly what you need to create the best PCBs.

Talk to an Altium Designer expert today if you want to learn more about Altium Designer.

Related Resources

Related Technical Documentation

Back to Home
Thank you, you are now subscribed to updates.