High Speed Design

Now reading version 18.1. For the latest, read: High Speed Design for version 24


Understanding the Challenge

This article does not attempt to provide a complete discussion of high speed design, for that there are a number of highly experienced and scholarly designers and engineers that have written excellent reference papers and books on the subject. Refer to the References section for links to these authors, and the papers used during research for this article. The purpose of this article is to introduce the key elements of high speed design, and then discuss how each of those elements is tackled in Altium Designer.

So exactly what makes a PCB design a high speed design? Sure it’s about things happening quickly, but it’s not just about the clock rate used on the board. A design is a high speed design when it includes devices with fast edges, devices that switch state so quickly that the transition is complete before the signal can travel along the route and reach the target pin. In this situation the signal can be reflected back to the source pin, degrading or destroying the original signal data. A signal with a fast edge can also radiate from the route and couple into adjacent routes, or radiate further and become electromagnetic interference (EMI), resulting in the product failing to meet mandatory emission standards.

When a signal has fast edges, it changes the way that the energy travels through the routing. In a circuit where edge rates change slowly, you can think of the energy flowing through the routing like water through a pipe – yes some energy is lost due to friction as the water is pushed through the pipe – but basically most of it arrives at the other end. For a DC or low switching frequency circuit you can work out the resistance of the route and make sure that the amount of energy lost along the way does not affect the circuit performance.

It's not so simple in a high speed design, because as well as the energy flowing as electrons though the routing copper, in a fast-switching signal some of that energy also travels as electromagnetic energy around the routing copper. Now you are no longer designing copper pathways for electrons, you're designing a series of transmission lines embedded in a printed circuit board.

How Long is too Long?

As the switching speed of the edge increases, the energy traveling through a route behaves differently. It no longer travels like water inside a pipe, instead, most of the energy is concentrated at the very surface of the route (known as the skin effect), with a portion of the energy actually traveling as electromagnetic radiation. Not traveling through the actual conductor, this electromagnetic energy travels through the material surrounding the route. Like dragging your foot through water, when energy travels in this way the signal actually slows down. Now it is the properties of the material around the route that dictate how quickly the signal travels, and how much its arrival will be delayed.

So when does this become a problem, the time it takes for the signal to propagate down the route to the target pin? Like a wave hitting a wall, when the signal arrives at the target input pin some of the energy in the signal is reflected back towards the source pin. If this reflected energy arrives back at the source pin while the original signal edge is still transitioning, then the original signal will be strong enough to swamp the reflection as it completes its transition - your signal will be OK. But if the edge transition is completed before the reflected energy arrives back, then like an echo in the canyon, that reflected energy will interact with the original signal and change it, perhaps so much that you cannot work out what was actually shouted into the canyon.

To summarize, when the travel time along this round-trip length is equal to or longer than the rise time of the signal, the integrity of that signal is in doubt - your design is now a high speed design! The length of that route is referred to as the critical length - routes shorter than this should not experience signal integrity issues, whereas routes longer than this might.

To analyze your design, a common rule of thumb that is often used is the 1/3 rise time rule, which states that if the route is more than 1/3 of a rise time long, reflections can occur. For example, if the source pin has a 1 nSec rise time, then a route longer than .33 nSec - which is approximately 2 inches in FR4 - must be considered to be a transmission line and therefore a candidate for signal integrity issues.

The 1/3 Rise Time Rule:

The speed at which electrical energy can travel along a route is known as the propagation velocity and can be defined as:

Vp= C / √εR


Vp = Propagation Velocity

C = Speed of Light (11.80285 in/nSec or 299.792458 mm/ns)

εR = Dielectric Constant

Assuming the Dielectric Constant εR of FR4 is 4, the Velocity of a Signal in FR4 is given as:

Vp(FR4) = (299.792458 / √4) mm/ns

              =149.89 mm/ns (approx 6 inches/ns)

Applying the 1/3 Rise Time Rule of Thumb, transmission line effects will begin when:

LR ≥ (TR / 3) × (C / √εR)


LR = Length of a route (in mm)

TR = Signal Rise Time (in ns).

For FR4, the route length at which transmission line effects need to be considered can be calculated as:

LR ≥ TR × 49.965 mm

If TR = 1nS

LR ≈ 50mm (2 inches)

If TR = 100pS

LR ≈ 5mm (0.2 inches)!! On a board with signals switching at these speeds, most routes will be transmission lines.

Matching the Impedances

Since it is not possible to ensure that all routes are shorter than the critical length, how do you ensure that the information encoded in your signals is received correctly, and not swamped by reflections? You do that by minimizing the amount of energy that is reflected back - ideally you want all of the energy that arrives at the target input pin to pass through into that component and none to be reflected back. Just how do you get that to happen?

To prevent reflections, you need to think of and design the route as if it is a transmission line. Why? because a transmission line has the special behavior that when it is terminated by an impedance the same as its own impedance, no energy is reflected. Now you have a method of handling those routes that are longer than the critical length - route them as a transmission line. This means you route them so they have a specific impedance, and then terminate them with the same impedance.

The impedance of the routing is defined by the dimensions of the routing (the width and height of the pipe), and the properties and dimensions of the surrounding materials, which will be the surrounding air or dielectric layers. To function as a transmission line, the layer that is adjacent to the signal layer must be a plane layer. By carefully arranging the layers in the layer stack and calculating the dimensions and properties, a specific impedance can be achieved for the routing. This approach to routing is referred to as controlled impedance routing, where the target impedance is kept constant, and the material dimensions and properties are selected and adjusted to achieve that.

A controlled impedance PCB cannot be achieved through routing alone though. There are two pieces to this puzzle - matching the impedance of the output pin to the near-end routing, and matching the impedance of far-end routing to the target input pin. Achieving this matching often requires the addition of termination components. Terminations can be added close to the source pin, or close to the target pin. A good approach to working out if a high speed net needs terminating is to analyze the design with a signal integrity simulator. Unlike a circuit simulator, which models and simulates the behavior and interaction of the components, a signal integrity simulator models the behavior and interaction of the routing. Components are only modeled in terms of the I/O characteristics of their pins.

The signal integrity analysis tool needs to:

  • Identify nets that could have unacceptable levels of reflections (ringing)
  • Predict the potential levels of signal reflection and crosstalk as waveforms
  • Allow what-if analysis of potential termination components and help select suitable termination components

Suggested layer stackups for 4, 6, 8, 10 and 12 layer boards.
A series of overlaid waveforms that represent the behavior of a net being swept over a range of possible termination values. Left is unterminated, the right is with a theoretical 40Ω series terminator.

Where does the Return Energy Flow?

But wait, there’s more (or is that Moore?). Electrical energy only flows when there is a closed loop, so the energy flowing out along the signal route must also have a return path. This return path is typically provided by the ground routing, which has to provide a return path for all of the signals in the design. There’s an interesting phenomena that occurs with signals with fast switching edges, the returning energy of a signal wants to flow back along the same twisting and turning path that the signal route took across the board - why, because this is the path of least impedance for that signal. Even though it could flow the shortest distance from the target component back to the source component, it does not.

When a high speed signal crosses a split in a plane a loop is created, causing that signal to create EMI.
When a high speed signal crosses a split in a plane a loop is created, causing that signal to create EMI.

So as well as thinking about the routing path for the signal, you also have to ensure there is an unbroken path for the return current, immediately under the signal route. If the return energy has to deviate from below the signal path to get around an obstacle, like a hole in the plane (a blowout), then a loop is created. The loop is the gap between the two paths as you look down into the board, and the area of this loop is proportional to the amount of energy that will now be radiated by this signal. If there is a blowout in the plane that is unavoidable, consider rerouting the signal trace to suit the return path, as reducing the loop area is generally considered more important than minimizing the route length.

An important point to keep in mind, the return path is through the closest power plane, which might not be a ground plane. If the return path is through a power plane instead of a ground plane, then the return energy will ultimately get to ground through the decoupling capacitors that are closest to the source and target pins. If you are relying on a power plane to provide the return path, carefully consider the location of the decoupling capacitors near these pins to minimize the size of any loop created.

Differential Pairs

Modern signaling technologies, such as differential pairs, help reduce the need for a high-quality return plane by routing the signal path and the return path together as a pair, insuring that they are closely coupled in both separation and overall length.  As well as the strong coupling and the reduced reliance on a high-quality reference ground, differential pairs offer another big advantage - excellent immunity to noise.

The electromagnetic energy that is traveling around the route as part of each signal does not all couple into the target input pin, some of it escapes and interferes with adjacent signals. This escaped energy becomes what is called electromagnetic interference (EMI), and when it couples into a neighboring signal it creates what is called crosstalk. Differential pairs are good at coping with crosstalk, because the radiated energy couples into both the outgoing signal and the return signal, creating what is called common mode noise (the noise is common to both signal paths). If there was only a single signal, then this crosstalk would add to that signal, and distort it. But the differential pair input pins are designed to look at the difference between the pins in the pair, and so are able to reject the common mode noise.

These two qualities - the ability to closely match the lengths of the signal and its return path, and the ability to withstand the effects of crosstalk - make differential pairs the preferred solution for high-speed signaling, which can support data rates beyond 10 Gb/s on a PCB.

Differential pairs provide strong immunity to noise and reduce the reliance on a high-quality return path via a plane. This reduced reliance on a ground plane is directly related to the degree that the pair lengths are matched and remain consistently coupled - as the length matching or the coupling declines, then the reliance of the signals on the plane increases. Most experts agree that matching the length is the critical requirement for differential pairs.

What about Vias?

If carefully controlling the impedance and insuring there is a high quality return path are the first two edges of the high-speed design triangle, vias are the third edge of that triangle. At low frequencies, a via has little impact on the signal quality and can be used without consideration of its impact on circuit performance. However, if your design is functioning as a high speed design, then the vias can impact on the circuit performance and the signal quality.

Vias appear as both capacitive and inductive discontinuities, so their presence affects the impedance of the signal route. As well as affecting the impedance, unused via barrel length presents as a stub which can create reflections.

Quantitative studies have shown that their impact can be reduced by addressing each of the following areas:

  • Reducing the size of the annular ring where the signal route connects to the via.
  • Removing unused annular rings on layers that the via is not connected to.
  • Increasing the clearance from the via barrel to adjacent plane layers.
  • Placing stitching vias adjacent to signal vias to provide a path for the signal return current to be able to switch plane layers.
  • Careful placement of decoupling capacitors adjacent to the via when a different voltage plane will be used to carry the signal return.
  • Removal of via stubs (the extra, unused via length that projects beyond the layer that the signal route uses to access the via). This is done through:
    • via design and careful layer assignments to suit the fabrication process,
    • controlled depth drilling (backdrilling) to remove the unused section of the via barrel.

Another approach to minimizing the impact of vias in a high speed design is to use microvias. A microvia is a small via, IPC standards (IPC/JPCA-2315 and IPC-2226) define microvias as blind or buried vias with a diameter equal to or less than 6 mil (0.15 mm). 6 mil is at the limit for mechanical drilling so microvias are typically laser-drilled. There are also hybrid laser modified + controlled depth mechanical hole drilling techniques used, as outlined in this paper, which offer advantages in fabrication.

Microvias offer a number of advantages:

  • Reduced parasitics (in the order of one-tenth of a drilled thruhole via), resulting in lower inductance.
  • Smaller geometries, which result in a smaller annular ring.
  • Reduced size of blowout on plane layers that they pass through.
  • Removal or reduction of stub length. Because they are constructed as part of the layer stacking process during fabrication, they can connect between specific start and end layers. While they cannot span any pair of layers, careful selection of the signal layers used for high speed signals can ensure that those layers have access to a microvia start/stop layer.

Using a controlled depth drilling process, often referred to as backdrilling, unused via barrels can be removed.

Suitable via design is an important ingredient in the high speed board design process. The possible layer-to-layer via connection possibilities are dictated by the board fabrication process, making it essential to choose the fabrication and drilling process at the same time as the via style and the layer stackup are being defined.


Because some of the energy in a high-speed signal travels through the material that surrounds the route, it is inevitable that some of that energy will couple into adjacent routes. Referred to as crosstalk, this energy will degrade the quality of that signal. In signal integrity language, the signal that is radiating the energy is referred to as the aggressor net, and the signal that is receiving the crosstalk energy is referred to as the victim net. So how do you reduce the amount of energy that escapes from the aggressor, and how do you reduce how much of that energy is coupled into the victim? The basic approach is to: reduce the amount of energy escaping from the aggressor route through impedance matching and correct design of the signal return path; and to keep potential victim nets away from aggressors.

Clock signals and other periodic signals are the prime source of crosstalk in a design. An often-used rule of thumb is to ensure that potential aggressors, such as clocks, are separated from potential victims by 3 times the width of the routing (center to center). This is known as the 3-W rule. Or in edge-to-edge terms, the separation must be no less that twice the routing width. This is a large clearance, so you will need to be selective about the nets that it is applied to. High-threat aggressors, such as clocks, are one group. The other main group to consider are the more sensitive potential victims, such as differential pairs; this group also benefits from a pair-to-other-signal separation of 3-W.

  Predicted ringing on an unterminated aggressor route (green waveform), and the resultant crosstalk in the adjacent victim route (blue waveform). Note that each graph has a different voltage scale.
Predicted ringing on an unterminated aggressor route (green waveform), and the resultant crosstalk in the adjacent victim route (blue waveform). Note that each graph has a different voltage scale.

Dancing in Time

And last but not least, there is the time it takes for the signal to arrive at its destination input pin. Generally a signal does not exist in isolation, it is working in harmony with a multitude of other signals, a simple example would be the 8 bits in a byte of data. Not only must the entire byte arrive within the time allowed, the bits within the byte must all arrive together too.  The time it takes for a signal to travel from output to input is referred to as the flight time, and any difference between the arrival times of the bits is referred to as the signal skew.

The key factors that influence both the flight time and the skew are:

  • The length of the signal routes - how far the signals have to travel
  • The materials that the signals are traveling through - this affects how fast the signals travel

Managing these, requires consideration of:

  • Component placement - good component placement is a key element of a successful high speed design. Use the Manhattan length to guide the initial placement of different components that need similar route lengths, for example DDR3 memory devices configured in T-branch topology. 
  • Material selection - the material that the PCB is fabricated from is a critical factor in a high-speed design. FR4 has served the PCB industry well for decades, but its use becomes a limiting factor in high speed designs as the inconsistent dielectric constant of FR4 creates skew. Material is discussed more in the following section.
  • Overall route length - as well as influencing the flight time, overall lengths are also important when routing sets of related nets. For example, DDR timing requirements specify that the clock route be longer than the address and control routes. These requirements are managed by Length design rules.
  • Matched route lengths - skew is managed by matching route lengths. It is the longest route in a set of signals that determines the route length for each net in that set. Lengths are matched by defining Matched Length design rules, and then lengthening each shorter route to match the specified length.

Differential pairs, lengths are matched within the pairs, and also between the pairs (image courtesy FEDEVEL Open Source, www.fedevel.com).
Differential pairs, lengths are matched within the pairs, and also between the pairs (image courtesy FEDEVEL Open Source, www.fedevel.com).

The Board

All of this happens on the printed circuit board. Since they were first created in the 1940s, the humble PCB has undergone tremendous levels of refinement in fabrication technology and materials. This has lead to enormous reductions in the size of the features, such as the routing and vias. Tracks are no longer fabricated at 20 mil wide, now they can be as small as 2 mil wide. And a small via is no longer 30/18 mil (land/hole), it is 12/6 mil. A new name was created to describe designs using features this small - High Density Interconnect (HDI) techniques. While it costs more to create the smaller features used on HDI boards, their smaller size means the finished design can use fewer layers, have shorter routes and improved signal integrity - which can ultimately result in a board that might not cost any more to make (but can be much harder to test and repair).

The Materials

A large part of the challenge with high-speed design is managing the medium that the signals travel through. Traditional FR4 has provided a cheap and effective board substrate material for decades, but the non-homogenous structure of fiberglass weave embedded in resin becomes a limiting factor for high speed designs. The resin has a different dielectric constant (≈3) from the fiberglass weave (≈6), and as the fiberglass is a woven structure with gaps in the weave, the signal sees a changing dielectric constant as it travels across the board. Because of this, there is a range of FR4 materials available, better materials have a tighter weave structure that give a more consistent dielectric constant. The dielectric constant of FR4 also changes with temperature, by as much as ± 20%.

There are superior materials available for PCB fabrication, such as Teflon or ceramic, but these come at a price. The material that the board is fabricated from must be considered and chosen early in the PCB design process, in consultation with the fabricator. To help balance material selection against material cost, many PCB fabricators allow a mix of materials, so that the expensive materials are only used for the layers that carry the high speed signals.

The Layers

Like many aspects of printed circuit board design, working out the best number of layers is as much art as it is maths. Fanout and escape routing of dense BGAs will strongly influence the number of routing layers, performing a test fanout and escape route to check the densest BGA in the design can help verify there are enough signal layers. Another approach, recommended by Barry Olney of In-Circuit Design, is to run a test autoroute on the board. He suggests that if it completes at least 85% of the routes, then the board should be hand routable using the current layer stackup.

Adding and assigning layers is done in pairs. Generally, you will either have a pair of plane layers for each pair of signals layers, or a pair of plane layers for every two pairs of signal layers. So a 4 layer board will be 2 plane and 2 signal, a 6 layer board will be 2 plane and 4 signal, an eight layer board will be 4 plane and 4 signal, and a 10 layer board will be 4 plane and 6 signal. Note that this is only a guideline, the overriding objective is to ensure that every high-speed signal layer is adjacent to a plane layer.

Not all signals are high speed signals, and not all layers can be configured as high speed routing layers, so the standard practice is to assign and route the high speed signals on specific layer pairs. Each signal layer pair should have one layer in the pair assigned for vertical routing and the other assigned for horizontal routing, and these should be followed as best as possible to reduce crosstalk between the adjacent layers. The high speed pair can be positioned on either side of a plane layer, or between 2 plane layers. 

The thickness of the dielectric between the high speed signal layers and the reference plane layer will be set to suit the required characteristic impedance, typically this will be less than 10 mil (0.25 mm). To achieve the overall board thickness required for mechanical reasons, adjust the thickness of a dielectric layer(s) that is not adjacent to a high speed signal layer, for example the center core layer.

The HDI Handbook includes a packaging technology map (page 53), which can be used to indicate if a design can be implemented using traditional mechanical drilling, or if it is likely to need to use a High Density Interconnect (HDI) structure. IPC standards IPC/JPCA-2315 and IPC-2226 include formulae which can be used to calculate component and wiring densities, providing you with valuable information to use when discussing the number of layers and the layer stackups with your fabricator.

Possible Layer Stackups

The table below shows possible layer stackups and layer assignments. The arrangement of high speed pairs and general purpose pairs can be changed, for example if your 6 layer / thruhole only design can have the high-speed signals routed on the top layer, then this is a good option if it means the high speed signals do not need to use vias. Keep each high speed layer adjacent to a plane layer, and the surrounding dielectric thicknesses the same for the high speed layers.

4-layer 6-layer 8-layer 10-layer 12-layer
        Signal HS-H
      Signal HS-H GND
    Signal HS-H GND Signal HS-V
  Signal H GND Signal HS-V Signal H
Signal V GND Signal HS-V Signal H GND
GND Signal HS-V GND GND Signal V
Signal H POWER Signal H Signal V POWER
  Signal V GND Signal HS-H Signal V
    Signal V GND Signal HS-H
      Signal HS-V GND
        Signal HS-V

Suggested layer stackups for 4, 6, 8, 10 and 12 layer boards.

Define the layer stackup early, and play close attention to the start/stop layers available for vias.

High Speed Design in Altium Designer

This section provides information on how to tackle each of these challenges in Altium Designer.

To summarize, the process of routing a board with high speed signals requires you to manage:

  1. Termination components that may be required
  2. The definition of the signals that need high-speed design rules applied to them
  3. The mechanical dimensions of the routes - for controlled impedance routing
  4. The properties and dimensions of the board materials
  5. The quantity and arrangement of the layers in the layer stack
  6. The return path of each high speed signal
  7. The impact of vias
  8. The configuration and routing of differential pairs
  9. Configuring and controlling the route lengths

Pre- and Post-layout Signal Integrity Analysis

Early in the design process, it is important to identify signals that might require impedance matching, so that additional termination components can be included before the component placement process is complete. Since output pins are typically low impedance and input pins are typically high impedance, termination components may need to be added to the design to achieve impedance matching.

Altium Designer includes a signal integrity simulator that can be accessed during both the design capture and board layout phases of the design process, allowing both pre- and post-layout signal integrity analysis to be performed (Tools » Signal Integrity). The signal integrity simulator models the behavior of the routed board by using the calculated characteristic impedance of the traces combined with I/O buffer macro-model information, as input for the simulations. The simulator is based on a Fast Reflection and Crosstalk Simulator, which produces very accurate simulations using industry-proven algorithms.

Because both design capture and board design use an integrated component system that links schematic symbols to relevant PCB footprints, SPICE simulation models and signal integrity macro-models, signal integrity analysis can be run at the schematic capture stage prior to the creation of the board design. When no board design is present, the tool allows you to set up the physical characteristics of the design, such as the desired characteristic trace impedance, from within the signal integrity simulator. At this pre-layout stage of the design process the signal integrity simulator cannot determine the actual length of particular connections, so it uses a user-definable average connection length to make its transmission line calculations. By carefully choosing this default length to reflect the dimensions of the intended board, you can gain a fairly accurate picture of the likely signal integrity performance of the design.

Nets with potential reflection problems can be identified and any additional termination components added to the schematic before proceeding to board layout. The values of these components can then be further tuned once the post-layout signal integrity analysis has been performed.

The Signal Integrity analysis engine helps identify nets with potential reflection issues, note that measurements can be taken directly from the waveforms.
The Signal Integrity analysis engine helps identify nets with potential reflection issues, note that measurements can be taken directly from the waveforms.

Defining the High Speed Signals

Main articles: Defining High Speed Signal Paths with xSignals, xSignal Wizard

High speed design is the art of managing the flow of energy from one point on a circuit board to another point. As the designer, you need to be able to focus your attention, and apply the design constraints, onto a signal that travels from this point on the board, to that point on the board. This signal you are focusing on is not necessarily a single PCB net though - the signal might be one branch of A0 in a design that you intend to route in a T-branch topology, with the other branch of A0 being another signal you need to focus your attention on as well, and be able to compare the route lengths of these two signals. Or the signal might include a series termination component in its path (which the PCB editor sees as 1 component and 2 PCB nets), and if that signal is in a differential pair, then its length needs to be compared to the length of the other signal in that pair.

You manage this requirement using a feature known as xSignals, where an xSignal is essentially a user-defined signal path. You select the source pad and the target pad, then right-click on either to define that signal path as an xSignal. As well as interactively defining an xSignal by its start and end pads, you can also run an intelligent xSignals Wizard, whose heuristics will help you to quickly set up a large number of xSignals between the chosen components.
These xSignals can then be used to target design rules to your high speed signals. The software understands the structure of these xSignals, for example calculating the overall length that includes multiple nets connected through a termination component.

The PCB panel includes an xSignal mode, use this to examine and manage the xSignals. The panel also provides feedback on the signal length, highlighting xSignals that are close to meeting (yellow) or failing to meet (red) the applicable design constraints. The panel includes the Signal Length, which is an accurate point-to-point length. Traditional length inconsistencies, such as tracks within pads and stacked track segments are resolved, and accurate via span distances are used to calculate the Signal Length.

Use the xSignals panel to manage and investigate your xSignals. Note the thin line, this is the signal path the software uses.
(Image courtesy FEDEVEL Open Source, www.fedevel.com)

The delay caused by the length of the pin within the device package is also supported, to learn more read about Pin Package Delay.

Read more about xSignals.

Defining the Properties of the Routing

Main articles: Routing Width Design Rule, Controlled Impedance Routing

Traditionally, board designers would define the widths and thickness of the routing by entering a dimension for the width, and selecting a thickness of copper for that layer. This was generally sufficient, you only needed to ensure that the current could be carried and the required voltage clearances were maintained. This approach is not sufficient for the high speed signals in your design, the objective of controlled impedance routing is to adjust the properties of the materials to deliver the required impedance.

This is achieved in Altium Designer by enabling the Characteristic Impedance Driven Width option in the Routing Width design rule. To translate that impedance into a width setting, the software applies an industry-standard equation. The equation includes the permittivity of the material that surrounds the route as well as the width and thickness of the copper, so the routing width required to deliver that impedance can change from layer to layer. You may also need to be ready to adjust the layer thicknesses to arrive at suitable settings that achieve your required impedance.

The routing width can be calculated to deliver a specified impedance.
The routing width can be calculated to deliver a specified impedance.

Altium Designer does not support controlled differential impedance routing, refer to the Specifying the Impedance section for more information on how to manage these.

Practical and cost-effective minimum starting values for high speed signal routing and via sizes are:

  • 4/4 mil (0.1/0.1 mm) routing/clearance
  • 20/8 mil (0.5/0.2 mm) via land/hole

The routing width and clearance is then adjusted as required to deliver the required impedance. The impedance algorithm needs information about the dielectric material, including its permittivity and its thickness, as well as the thickness of the copper layers. This information is defined in the Layer Stack Manager, which is discussed below.  

There is a great deal of debate about corners in high speed signal routes. While it is agreed that the electrons will not fly off when they hit a 90 degree corner, a traditional 90 degree corner is wider across the corner diagonal, which does change the impedance of the route. Rounded or 45 degree corners are preferred - both are standard features of Altium Designer's interactive router (link) - and if needed 90 degree corners can be mitered, using the Convert Selected Tracks to Chamfered Path command.

Specifying the Impedance

So how do you know what target impedance to select? This is normally driven by the characteristic source impedance of the logic family or technology being used. For example, ECL logic has a 50Ω characteristic impedance, and TTL has a source impedance range of 70 to 100Ω. 50 to 60Ω is a common target impedance used in many designs, and for differential pairs, 90Ω or 100Ω differential impedance is common. Remember, the lower the impedance the greater the current drain, the higher the impedance the more chance there will be EMI emitted, and the more susceptible that signal will be to crosstalk.

A 100Ω differential pair can also be viewed as two, 50Ω single-ended routes that have the same length. This is not exactly correct due to the coupling that occurs between the pair, which becomes stronger as they become closer, reducing the differential impedance of the pair. To maintain 100Ω differential impedance the width of each route can be reduced, which slightly increases the characteristic impedance of each route in the pair by a few ohms.

Altium Designer does not include a differential impedance calculator, to calculate differential impedance you will need to use a 3rd party stackup designer / impedance calculator, such as the ones available from In-Circuit Design or Polar Instruments. A strength of these tools is that they include dielectric constants for a large range of standard materials, which speeds up the selection and calculation process. The In-Circuit Design stackup planner also supports direct import/export to an Altium-format board stackup file, which can then be loaded into Altium Designer's Layer Stack Manager, bringing detailed material information into your design. If you like the idea of working directly with a low-level impedance calculator, you can explore the Arbitrary Transmission Line Calculator (ATLC), available under the GNU General Public License.

Defining the Properties of the Board

Main article: Layer Stack Management

The materials used for the layers in your board, their dimensions, and the number of and order that the layers are arranged, are all defined in the Layer Stack Manager. Here you configure the various layers that are needed to fabricate the final board: including the copper signal and plane layers, the dielectric layers that separate the copper, the cover layers, and the component overlay.

The dimensions and properties of the copper and dielectric layers are factors in the impedance calculations, which can also be examined and edited through the Layer Stack Manager.  

All fabricated layers are defined in the Layer Stack Manager. The information in this dialog is included in a placed Layer Stack Table.
All fabricated layers are defined in the Layer Stack Manager. The information in this dialog is included in a placed Layer Stack Table.

Detailed information about the material properties that is entered in the Layer Stack Manager is included in the Layer Stack Table, use this to pass information to the fabricator.

You can also Save and Load layer stackups in the Layer Stack Manager, use this feature to quickly load your preferred stackup into future designs.

Blind and Buried Vias

Many high speed designs use blind and buried vias. A blind or buried via will be used automatically in a layer swap during interactive or autorouting, if the drill pairs have been defined in the Drill Pair Manager. Click the Drill Pairs button in the Layer Stack Manager to configure them.

Configure the start and stop layer for valid layer pairs.
Configure the start and stop layer for valid layer pairs.

Managing the Return Path for High Speed Signals

A good quality return path is essential for each high speed signal in the design. Whenever the return path deviates and does not flow under the signal route a loop is created and this loop results in EMI being generated, with the amount being directly related to the area of the loop.

A good quality return path is one where:

  • There are no breaks, splits or blowouts (holes in the plane created by a via or thruhole pin) under the signal route, in the plane providing the return path (the plane closest to the signal of interest).
  • The width of the return path is ideally 3x the width of the signal routing, or 3x the distance from the route to the plane, whichever is smaller. While the greatest current density is directly below the signal route, it actually spreads out into the plane on either side of the route too, with approximately 95% flowing within 3x the route width. Breaks in the plane within this region have the effect of increasing the impedance of the return path, and any deviation in the return path will create a loop. In terms of signal integrity, this increased return path impedance impacts the quality of the signal as much as increasing the impedance of the signal path.
  • The area of the loop has been minimized. Generally it is more important to reduce the loop area than minimize the routed signal length, if the return path encounters a blowout, consider re-routing the signal to suit an available return path. 
  • When a power plane is providing the return path, the return energy will ultimately get to ground through a decoupling capacitor. Carefully consider the location of the decoupling capacitors near the source pin of the signal, to minimize the size of any loop created.

There is general agreement that a ground plane should not be split unless there is a specific requirement for it, and you understand how to define and manage it. Instead, the components should be arranged to keep noisy components separate from quiet components, and to also cluster components by the supply rail that they use.

Other points to keep in mind about power and ground planes include:

  • If the design requires a ground plane to be partially split, then signals that traverse those areas should be routed across the bridge (the zone without a split below it).
  • If you are attempting to minimize circuit noise, it is better to use additional ground planes than to split a plane, and where possible, include plane layers for both the supply and ground rails of each regulated power supply. 
  • If the design includes multiple rails with each distributed on its own plane, ensure that each power plane only references its own ground plane - do not let allow a power plane overlap (reference) a different rail's ground plane. This creates capacitive coupling, allowing noise to travel from one supply to another.
  • If the adjacent plane is a power plane which must be split into different voltage areas, then you might need to decouple directly across the 2 voltages areas to provide a suitable return path.

To help with the task of visually checking the return paths, you can configure the display so you can more easily examine the return path under the critical route paths. To do  this:

  • In the in the View Options tab of the View Configurations dialog, set the Plane Drawing option to Solid Net Colored.
  • Switch to the signal layer and Ctrl+Click on the net of interest to highlight it (include Shift to highlight multiple nets).
  • Then make the plane layer the active layer and switch to single layer mode (Shift+S).

Your net(s) will stand out, and any splits or discontinuities that lie in the return path, such as split lines or blowouts created by though-holes, will be easy to see. 

These signals travel over split lines as they traverse different voltage areas on the plane. Note that each power net has been assigned a different color, to make each area easier to see.
These signals travel over split lines as they traverse different voltage areas on the plane. Note that each power net has been assigned a different color, to make each area easier to see.

While it is possible to create a plane layer by covering a signal layer with a polygon pour, Altium Designer's Signal Integrity analysis tool and impedance calculator do not consider such a signal layer as a solid plane. For this reason it is better to use plane layers.

You can ensure that signals are not inadvertently routed across a split in a plane by placing a keepout along the split, on the keepout layer.

Managing the Impact of Vias

As mentioned in the overview section of this article, vias affect the impedance of the signal routing. Quantitative studies have been performed to understand their impact, such as the Altera Application Note AN529 Via Optimization Techniques for High-Speed Channel Designs. Summarizing this study and other references, the following guidelines are given to help minimize the impact of vias:

  • Reduce the size of the via annular ring where the signal route connects to the via, the App Note suggests a via diameter/holesize of 20/10 mil (0.5/0.25 mm) for mechanically drilled vias.
  • Remove unused annular rings (also known as NFPs, or Non Functioning Pads) on layers that the via is not connected to. Use the Tools » Remove Unused Pad Shapes command to do this.
  • Increase the clearance from the via barrel to adjacent plane layers. This is controlled by the Power Plane Clearance design rule, the App Note suggests 40 to 50 mil (1.0 to 1.25 mm). Note that this increases the size of blow outs in those plane layers.
  • Place stitching vias adjacent to signal vias whenever the signal route has a layer change that results in the return path switching to another layer. If the new reference plane layer is the same voltage as the original reference plane then those planes should be tied together with a via, within 35 mil (0.9 mm) of the signal via (center to center).
  • Careful placement of decoupling capacitors adjacent to the signal via, when the layer change results in a different voltage plane being used to carry the signal return. This capacitor decouples directly between the 2 planes, regardless of the voltages they carry. Note that this solution can result in noise being coupled from one plane to the other, so this should only be done as a last resort to reduce the return path loop area.
  • Remove via stubs (extra via length beyond the layer that the signal route accesses the via). This is done by using suitable blind and buried vias, or by via backdrilling during fabrication.

The design of the vias is an key ingredient in the high speed board design process. The possible layer-to-layer via connection options are dictated by the fabrication process chosen to achieve the layer stackup, which means you must choose the fabrication and drilling process as the via style and the layer stackup are being defined.

The PCB editor supports backdrilling (also referred to as Controlled Depth Drilling). The feature supports backdrilling from both sides of the board, and backdrilled sites can be easily examined in the PCB panel, with the board displayed in 3D mode.

Read more about Controlled Depth Drilling.

Configuring and Routing Differential Pairs

Main article: Differential Pair Routing

The definition of differential pairs can be done during schematic capture, or they can be defined once the design has been transferred to board layout. A core requirement of defining a pair on the schematic is to include an _P or _N at the end of the Net name for each of the relevant nets. Differential pairs are identified on the schematic by placing a Differential Pair directive on each net, or by placing one on a Blanket directive, where the Blanket directive overlays a set of enclosed differential-style Net Labels, as shown in the image below.

Differential Pairs defined for a set of nets on the schematic, by including them within a Blanket directive.
Differential Pairs defined for a set of nets on the schematic, by including them within a Blanket directive.

In the PCB editor, differential pairs can be defined in the Differential Pair Editor mode of the PCB panel. To simplify the process of defining design rules that apply to the differential pairs, they can either be assigned to Net Classes or to Differential Pair Classes, both of which are defined in the Object Class Explorer.

The width and clearance properties of the differential pair are defined by the Differential Pair Routing design rule. Currently Altium Designer does not support defining the differential pair routing widths based on a differential pair impedance, you will need to calculate these using an external impedance calculator, such as the ICD Stackup Planner from In-Circuit Design, and enter the width values in for each layer in the design rule.

To route a differential pair, you use the Interactive Differential Pair routing command. Click on either the _P or _N pad to commence routing, then use the Spacebar to cycle through the available exit routing shapes. The routing behavior is the same as single net routing, press Shift+F1 for a list of interactive routing shortcuts. As you approach the target pads, press Ctrl+Click to complete the routing up to the pads.

Differential Pair rules of thumb:

  • Length matching is critical for differential pairs to be effective, keep the lengths matched to within 25 mil (0.635 mm). Another rule of thumb that is used is to match the lengths to be within 20% of the signal rise time. Differential pairs work because the return energy flows back through the other member of the pair, the more that the lengths do not match, the greater the amount of energy that returns through the nearest plane layer instead.
  • Discontinuities in the coupling, such as when the pair members route around either side of an obstacle, increases the impedance. It can be better to route the entire pair with looser coupling (for example 2 x signal route width) to reduce the amount that the impedance changes due to coupling discontinuities.
  • Keep aggressor routes away, especially on surface layers, aim for a clearance of 3 x the signal route width for potential aggressor nets.
  • As a general rule, aim for a pair-to-other signal clearance of 2 x signal route width.
  • Keep same-layer ground polygons away by at least 3 x signal route width.
  • Reflections introduced by vias and coupling discontinuities are managed through controlled impedance routing, doing this requires a continuous reference plane below the signal path.
  • Reduce the signal layer-to-plane separation to improve immunity to crosstalk.

Controlling and Tuning the Route Lengths

Main articles: Length design rule, Matched Length design rule, Length Tuning

A key requirement of managing high speed signals on a board is to control and tune their route lengths.

  • The absolute and relative route lengths can be monitored by the Length and Matched Length design rules.
  • The current lengths of a set of nets, and their compliance with applicable design rules, can be checked in the PCB panel in Nets mode (as shown below).
  • If there is a Length rule and/or a Matched Length rule defined, then you can monitor the length during interactive routing or length tuning by displaying the Length Tuning Gauge (Shift+G).
  • The delay caused by the length of the pin within the device package is supported, to learn more read about Pin Package Delay.

  • Nets that include serial components in their path are managed by defining xSignals.

Design Rules

  • Managing the Overall Route Lengths - the overall route length of a net or set of nets can be monitored by a Length design rule. The Length design rule has a minimum and maximum allowed length, a signal length less than the allowed minimum is highlighted in yellow in the PCB panel, a signal length greater than the allowed maximum is highlighted in red (as shown in the image below).
  • Managing the Relative Route Lengths - the relative route lengths of a set of nets can be monitored by a Matched Length design rule. The Matched Length design rule has a tolerance and uses the longest route in the set of targeted nets as reference length. A signal whose length is less than the longest route by more than the tolerance, is highlighted in yellow. 

To understand how the settings of these two rules are resolved when both are present in a design, refer to the Length Tuning page.

Monitoring the Route Length

Current route lengths are displayed in the Nets mode of the PCB panel, and are updated as you route. The Routed length value will go yellow as you approach the target length, and turn red if you exceed it, as shown in the image below.

If there is a Length rule and/or a Matched Length rule defined, then you can monitor the length during interactive routing or length tuning by displaying the Length Tuning Gauge. While you are routing, use the Shift+G shortcut to toggle the Gauge on and off.

The Gauge shows the current Routed Length as a number, while the green slider shows the Estimated Length. At first glance at the Gauge it might seem confusing that the Routed Length has not even reached the rule minimum value, but the green slider is somewhere between the rule minimum and maximum - as it is in the image below. That is because the green slider represents the Estimated Length, where

Estimated Length = Routed Length + distance to target.

The Gauge displayed as a Length design rule is being obeyed during Interactive Routing - it shows the current Routed length as a number, the green slider shows the current Estimated Length.The Gauge displayed as a Length design rule is being obeyed during Interactive Routing - it shows the current Routed length as a number, the green slider shows the current Estimated Length.

Routed Length = sum of the lengths of the placed track segments.

Estimated Length = current Routed Length + distance from current location to target pad (length of the remaining connection line).

Signal Length = current Routed Length + Manhattan (X + Y) distance from current location to target pad.

Tuning the Route Lengths

Route lengths can be tuned after the routing is complete, using the Interactive Length Tuning command, or the Interactive Diff Pair Length Tuning command (Tools menu). These commands add accordion sections to the routing, in a choice of three shapes.

If there is an applicable Length rule and Matched Length rule, the length tuning tool considers both of these rules and works out the tightest set of constraints. So if the maximum length specified by the Length rule is shorter than the longest length targeted by the Match Length rule, then the Length rule wins and its length is used during tuning.

To see which rules are being applied or to change the accordion properties during length tuning, press Tab to open the Interactive Length Tuning mode of the Properties panel, as shown below. Note the Target Length, this is the Max Limit of the strictest applicable rule settings.

Press TAB during length tuning to open the panel in Interactive Length Tuning mode,
where you can select the target length mode and adjust the accordion parameters.

To tune the length of a net, run the command and then click anywhere along the net's length. Move the cursor so that it follows the path of the route, tuning accordion sections will be added as you do. Tuning sections will continue to be added until the the length requirements defined by the applicable design rule(s) have been satisfied. If the cursor moves outside the bounds of the tuning accordions, the accordion shapes will disappear - when the cursor is moved so that it is back within the bounds of the accordion shape, they will re-appear.

Length and Length matching rules can be applied to nets, or to xSignals. xSignals are ideal if the lengths being monitored or matched include series components or branched routing. The xSignals mode of the PCB panel displays the current routed length of each xSignal.

Impedance Calculator and Layer Stackup Planning Tools

Altium Designer includes an impedance calculator, which allows you to define the routing width based on the required impedance. To learn more, refer to the Controlled Impedance Routing article.

For more comprehensive stackup guides and calculators, including differential pair calculators, explore the following sites.

In Conclusion

While it is not possible to derive a universal set of rules that apply to every high speed design, it is possible to follow good design practices that will help you succeed with your high speed design. There are a number of industry experts that deliver practical and popular training courses on high speed design. Use the links below to learn more, and to research specialized training options.


The author gratefully acknowledges the work of the following industry experts, this article is an attempt to summarize their collective knowledge.

Douglas Brooks articles

  • Microstrip Propagation Times
  • Splitting Planes For Speed and Power
  • Skin Effect
  • Differential Trace Design Rules - Truth vs Fiction

Dr. Howard Johnson articles

  • Via Inductance
  • 10 Layer Stack

In-Circuit Design articles - Barry Olney

  • Differential Pair Routing
  • The Plain Truth About Plane Jumpers
  • Critical Placement
  • Stackup Planning (Parts 1, 2 & 3)
  • The Perfect Stackup

Lee W. Ritchey books and articles

Best Practice in Circuit Board Design - Tim Jarvis RadioCAD Limited

PCB Layout - Learn EMC website

Keith Armstrong articles, EMC Information Centre (free registration required)

The Electronic Packaging Handbook - Glenn R. Blackwell

The HDI Handbook - Happy Holden and others

Via Optimization Techniques for High-Speed Channel Designs - Altera Application Note AN529

High-Speed PCB Design Considerations - Lattice Semiconductor Application Note TN 1033 

Measuring a Signal's Flight Time - Chris Grachanen, EDN

The Future of HDI Via Structures, Power Delivery, and Thermal Management in Next Generation Printed Circuits - Tom Buck TTM Technologies

The Printed Circuits Handbook - Clyde Coombs and Happy Holden


If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.