Altium Designer Documentation

Managing Differential Pairs using the PCB Panel in Altium Designer

Modified by Jason Howie on Jul 13, 2021
All Contents

Parent Page: PCB Panels


The Differential Pairs Editor mode of the PCB panel.

Summary

The Differential Pairs Editor mode of the PCB panel can be used to create and edit differential pairs. Differential pairs can be added manually or through the Differential Pair Wizard, or created from nets.

The three segments of the Differential Pairs Editor mode of the PCB panel are:

  1. Differential pair classes.
  2. Individual member differential pairs within a class.
  3. The constituent nets (negative and positive) that form a differential pair.

Panel Access

When the PCB Editor is active, click the button at the bottom-right corner of the workspace and select  PCB from the context menu. Alternatively, you can access the panel through the View » Workspace Panels » PCB » PCB sub-menu.

Panels can be configured to be floating in the editor space or docked to sides of the screen. If the PCB panel is currently in a group of panels, use the PCB tab located at the bottom of the panels to bring it to the front.

Once the PCB panel has been opened, select the Differential Pairs Editor option from the dropdown menu at the top of the PCB panel to enter Differential Pairs Editor mode.

Using the Differential Pairs Editor

As you click on an entry in a list, a filter will be applied based on that entry, the visual result of which (in the design editor window) is determined by the highlighting methods enabled (Mask/Dim/Normal, Select, Zoom). In this way you can quickly highlight all differential pairs in a particular class, a particular differential pair, or a particular net that forms the negative or positive half of a differential pair. Multiple entries can be selected in each region, using standard Shift+Click and Ctrl+Click features.

Right-clicking on a differential pair class entry and selecting Properties (or double-clicking on the entry directly) will open the Edit Class dialog, where you can rename it or view/modify the differential pair membership of the class. For full control and editing of all classes, including Differential Pair Classes, open the Object Class Explorer dialog through the Design » Classes menu path.


The Object Class Explorer allows creating, viewing and modification for all classes, including Differential Pairs.

Right-clicking on a Differential Pair entry in the PCB panel and selecting Properties (or double-clicking on the entry directly) will provide access to the Differential Pair dialog, from where you can view/modify the properties for differential pair name and its constituent nets. See the following Managing Differential Pairs section for more on the Differential Pair dialog.

Right-clicking on a net entry in the PCB panel and selecting Properties (or double-clicking on the entry directly) will provide access to the Edit Net dialog, from where you can view/modify the properties of the net as required.

Back in the PCB panel, as you click on an entry in a list a filter will be applied based on that entry. The visual result (in the design editor window) of the cumulative filter is determined by the highlighting methods enabled (Mask/Dim/Normal, Select, Zoom).

In this way you can quickly highlight all differential pairs in a particular class, a particular differential pair, or a particular net that forms the negative or positive half of a differential pair. Multiple entries can be selected in each region, using standard Shift+Click and Ctrl+Click features.

Managing Differential Pairs

Use the Differential Pairs region of the panel to manage the differential pair objects in a design. For the particular differential pair class selected, all currently defined differential pair objects that belong to that class will be listed in this region.

Use the buttons at the bottom of this region to create new differential pair objects, or edit or delete existing ones. These three commands are also available from the right-click menu for the region. When adding a new differential pair, the Differential Pair dialog will open.

 

Use the dialog to define the pair object, in terms of a positive and negative net and a meaningful name. By default, the name will be set to NewDifferentialPair1 and the positive and negative nets will be set to the first and second available nets in the netlist for the design. Use the drop-down lists to select from the available nets.

Note that only available nets are listed for selection. Nets currently defined as part of existing differential pairs are not listed.

When editing an existing differential pair object, the Differential Pair dialog will again appear, with the currently chosen nets for the pair entered into the Positive Net and Negative Net dropdown fields respectively. Change one or both nets for the pair, or rename the pair, as required.

Creating Differential Pairs from Design Nets

Differential pair objects can be automatically created from the nets in your design using the Create Differential Pairs From Nets dialog. This dialog is accessed by clicking on the Create From Nets button at the bottom of the Nets region of the PCB panel.


Prospective differential pair objects are listed for creation in response to the filter entries at the top of the dialog.

The effectiveness of this automated method directly depends on the naming convention that has been used for the specific nets that will make up the differential pairs. Ideally, a naming convention will be used whereby a common root is followed by a consistent positive/negative indicator (P and N). For example, consider the receiver signal D_ETH_O.RX (see above), which is a differential signal in the design. The two nets that constitute this signal are ETH_O.RX_P and ETH_O.RX_N  - these represent the positive and negative sides of the signal, respectively.

The filters at the top of the dialog enable you to quickly target these nets in terms of the net class to which they belong and the particular differentiating factor that has been used to distinguish the positive and negative nets in an intended pairing - for example, _P and _N. You can also define a prefix to be added to the differential pair objects created, and also determine in which differential pair class they are to be added. In the above example, notice that the name for a differential pair object is created using the prefix specified and the root of the differential pair signal. The polarity indicators are discarded.

For each differential pair object, the dialog lists its constituent positive and negative nets. By default, all prospective differential pair objects are selected for creation, and individual ones can be excluded by clearing the associated Create check box. In the example above, only D_ETH_O.RX is checked for creation.

When all options are set as required, click the Execute button - the differential pair objects will be created and the PCB panel will update accordingly.

Filtering will be applied to show the created pairs in the workspace, as shown below.


Differential pair objects created from nets. In practice, differential pairs would normally be defined before the nets are routed.

Configuring Applicable Design Rules

A Differential Pair Routing rule needs to be configured before routing a differential pair in a design. A differential routing rule defines:

  • The preferred Gap between the network pair, and its permitted range.
  • The maximum Uncoupled Length (the pair is uncoupled when the gap is wider than the maximum Gap setting).
  • The preferred routing Width for each net.
  • The optional gap/width setting variations for each layer in the stack.
  • The scope (in terms of classes and objects) for the rule's application.

While rules can be created manually using the PCB Rules and Constraints Editor (Design » Rules), the PCB panel offers the convenience of the Differential Pair Rule Wizard. Use the Rule Wizard button (below the Nets region in the PCB panel) to access the Wizard and implement the rule properties as required.


The Differential Pair Rule Wizard guides you through the rule definition process.

Note that the scope of the rules will depend on the selection in the PCB panel prior to launching the wizard, as follows:

Differential Pair Class

If the All Differential Pairs class is selected, the scope will be All for each rule.

If a specific differential pair class is selected, the scope will be InDifferentialPairClass('ClassName') for each rule.

Differential Pair

If a single differential pair object is selected in the panel, the scopes will be:

  • Width - InDifferentialPair('PairName')
  • Matched Net Lengths and Differential Pairs Routing - IsDifferentialPair And (Name = 'PairName'))

If multiple differential pair objects are selected in the panel, there will be individual scope entries for each pair object, each separated by an Or operator. For example a routing Width rule targeting individually selected differential pair objects D_ETH_O.TX and D_ETH_O.RX will have a scope of:
InDifferentialPair('D_ETH_O.TX') Or InDifferentialPair('D_ETH_O.RX')

Note that the clearance from a net in a differential pair to any other electrical object that is not a part of the pair is monitored by the applicable Clearance rule.

To edit the configuration of an existing Differential Pairs Routing rule, including its scope etc, open the PCB Rules and Constraints Editor dialog (Design » Rules from the main menu) and navigate to Routing - Differential Pairs Routing.


For a differential pair the Gap settings can either be set for all layers using the controls beside the image of the pairs, or they can be set for each layer in the grid region below the image.

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.