Parent article: The Routing
A differential signaling system is one where a signal is transmitted down a pair of tightly coupled carriers, one of these carrying the signal, the other carrying an equal but opposite image of the signal. Differential signaling was developed to cater for situations where the logic reference ground of the signal source could not be well connected to the logic reference ground of the load. Differential signaling is inherently immune to common mode electrical noise, the most common interference artifact present in an electronic product. Another major advantage of differential signaling is that it minimizes electromagnetic interference (EMI) generated from the signal pair.
Differential pair PCB routing is a design technique employed to create a balanced transmission system able to carry differential (equal and opposite) signals across a printed circuit board. Typically this differential routing will interface to an external differential transmission system, such as a connector and cable.
It is important to note that while the coupling ratio achieved in a twisted pair differential cable may be better than 99%, the coupling achieved in differential pair routing will typically be less than 50%. Current expert opinion is that the PCB routing task is not to try and ensure a specific differential impedance is achieved, rather the objective is to maintain the properties required to ensure the differential signal arrives in good condition at the target component as it travels from the external cabling.
According to Lee Ritchey, a noted industry high-speed PCB design expert, successful differential signaling does not require working to a specific differential impedance. What it does require is:
Differential pairs are defined on the schematic by placing a Differential Pair directive (Place » Directive) on each of the nets in the pair. Note that the net pair must be named with net label suffixes of _N and _P. Placing a Differential Pair directive on each pair net applies a parameter to the net, which has a parameter Name of
DifferentialPair and a Value of
Differential pair definitions are transferred to the PCB during design synchronization.
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 (the software detects nets whose Net Label hotspot is within the blanket boundary). The blanket is then tagged by a single Differential Pair directive, 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
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 this net class,
If you have placed Differential Pair directives on nets in the schematic, the default project options settings will result in the differential pairs members being created on the PCB. The following options in the Options for PCB Project dialog are used to configure this:
Differential pair definitions are viewed and managed in the PCB panel, set to Differential Pairs Editor. The image below shows the pairs that belong to the class
V_RX0 is highlighted, the nets in this pair are
V_RX0_P. The - and + displayed next to each member net name is a system flag, indicating if it is the positive or negative member of the pair.
Differential pairs can be defined on the schematic, and they can also be defined in the PCB Editor. To create a differential pair object in the PCB editor, click the Add button when the PCB panel is set to Differential Pairs Editor mode. From the resulting Differential Pair dialog, select existing nets for both the positive and negative nets, give the pair a name and click OK. Note that any two nets can be chosen as the differential pair members when they are defined in the PCB editor.
Often there is more than one differential pair that needs to be targeted by design rules. In this situation you can define classes of differential pairs, clustering them into logical groups. Classes are defined in the Object Class Explorer dialog (Design » Classes).
If your differential pairs have series components in the signal path, you might find it worthwhile creating xSignals. An xSignal is a designer-defined signal path between 2 nodes - they can be 2 nodes within the same net, or they can be 2 nodes in different nets. Using an xSignal, you can define the signal path so that it includes the net on either side of a series component, as well as the series component. Route length calculations for xSignals includes the length of the path through the series component, as shown by the thin line that is displayed when an xSignal is selected in the xSignals mode of the PCB panel.
To interactively route a differential pair, create and configure the following two design rules in the PCB Rules and Constraints Editor dialog (Design » Rules):
InDifferentialPairClass('All Differential Pairs'). Note that the Gap setting is used during placement, but not during design rule checking. During design rule checking, the distance between the nets in a pair is tested by the applicable Electrical Clearance design rule.
The scope of the design rule defines the set of objects to which you want the rule to apply. Since a differential pair is an object, you can use queries like the following examples:
Click the Rule Wizard button in the Differential Pairs Editor (PCB panel) to walk you through the process of setting the required design rules. Note that the scope used for the created rules will depend on what was selected when the Rule Wizard button was clicked - if one pair was selected the rules will target the nets in that pair, but if a differential pair class was selected then the rules will target the nets and all pairs in that class.
Differential pairs are routed as a pair - that is, you route two nets simultaneously. To route a differential pair, select Interactive Differential Pair Routing from the Route menu. You will be prompted to select one of the nets in the pair, click on either to start routing. The animation below shows a differential pair being routed.
As you route the differential pair the standard conflict resolution modes are available, including Walkaround, Push, Hug and Push, and Ignore obstacles.
The PCB editor includes powerful tools for improving the quality of existing routing. These tools are known as Glossing and Retracing, both are available on the Route menu.
To learn more about Gloss and Retrace, read the Post-Route Glossing and Retracing page.
The animation in the previous section, Routing a Differential Pair, includes a simple demonstration of glossing.
Selection is a core activity in all areas of the design process, including working with existing routing. Whether you're about to gloss or you want to delete some routing, the routes need to be selected first.
In the PCB editor, selection can either be objects that are Within the selection rectangle, or Touching the selection rectangle. This is controlled by the direction you move the mouse as you draw the selection rectangle:
|Select Within - click and drag a blue rectangle from Left to Right to select all visible, unlocked objects that are completely within the selection rectangle.|
|Select Touching - click and drag a green rectangle from Right to Left to select all visible, unlocked objects that touch the selection rectangle.|
A common situation is needing to select many objects that are touching, for example, the track segments in a routed net, or the connection lines in an unrouted net. It is relatively easy to select a set of track segments that run parallel to each other using the Select Touching technique just described, but interactively selecting entire routes can be difficult.
This can easily be achieved though by selecting one or more track segments and then extending the selection to include touching track segments. This is done using the Tab key, as demonstrated in the video below.
During routing, there will be many instances where you need to change some of the existing routing, for example, you might not be happy with the pad exits and wish to re-shape them (as shown in the animation below). While you can change the existing routing using a drafting type approach of clicking and dragging track segments, it is often easier to simply re-route.
To do this, select the Place » Interactive Differential Pair Routing command, then click anywhere on the existing routing. Proceed to route the new path, coming back to meet the existing routing where required. This will create a loop with the old path and the new path, when you right-click or press Esc to terminate the route, the redundant segments are automatically removed, including any redundant vias. Differential pair routing is slightly different from single net routing, during single net routing the last segment is hollow, (the look-ahead segment), this segment is not placed when you click. Differential pair routing does not include look-ahead segments, so when you click you will place all visible segments. Position the cursor to ensure that there are no redundant segments.
If you are adjusting differential pairs by manually dragging track segments, you can either push one pair member with the other or drag each independently.
To learn more, refer to the Modifying the Routing article.
Have you ever been stuck during routing, wondering why the route won't fit through that gap? This frustration is even more likely during differential pair routing. Altium Designer V16 introduced a feature to help with this, called dynamic display of clearance boundaries. When enabled, the no-go clearance area defined by the existing objects + the applicable clearance rule is displayed as shaded polygons, within a local viewing circle, as shown in the animation below. Press Ctrl+W to toggle the feature on and off.
The display area can be restricted to a circle around the current cursor location, or it can be the entire screen. This is controlled by the Reduce Display clearance area option, in the PCB Editor - Interactive Routing page of the Preferences dialog.
Differential pairs are often used in high-speed design due to their inherent immunity to noise, and the fact that they simplify the challenge of providing a high-quality return path for the signals. However, like single-sided signals, their lengths must be managed to ensure the signal timing requirements are met.
During differential pair routing, the length of each of the two nets in the pair is displayed on the Status bar, and also in the Heads-up display (Shift+H to toggle on/off). The length values displayed in the PCB panel are updated when you drop out of routing a pair.
Length and Matched Length design rules can be defined to ensure that the flight time and skew timing requirements are met. As well as being used during a design rule check (DRC), these rules are also used during interactive length tuning.
The Matched Length design rule detects the longest pair targeted by the rule scope, and uses the Average Length value of that pair as the reference to compare the other targeted pairs, requiring their lengths to be within + or - the Tolerance defined in the rule. The Average Length value is shown in the Differential Pairs Editor in the PCB panel.
It is likely that you will have matched length requirements between the pairs, and also within each pair.
To manage this you create suitable Matched Length design rules:
The length of pairs, and the nets within each pair, are tuned using the two length tuning commands. To tune the lengths:
Manually, enter the value in the Target Length field
From a user-selected routed diff pair
From the applicable Length and Matched Length design rules.
Differential pair length tuning accordions are created from multiple short track and arc segments. These can be manually selected and deleted, however, it is usually more efficient to simply re-route over the top of them, the loop removal feature will then remove the redundant track/arc segments.
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.