Altium Designer Documentation

Interactively Routing with Controlled Impedances on a PCB in Altium Designer

Created: May 11, 2022 | Updated: July 26, 2022

Parent page: High Speed Design

With increasing device switching speeds, controlled impedance routing has become a hot topic for the digital designer. This article introduces how you can use the Signal Integrity analysis engine to match component impedances and the controlled impedance routing capabilities in the PCB editor.

There is a saying in engineering circles - there are only two kinds of electronics engineers working in digital design: those who have had signal integrity problems, and those who will. Not so many years ago the term signal integrity was one for the specialist and you only had to deal with it on high-speed designs. However, the device switching speeds in those high-speed designs are no longer anything special, in fact, they are rapidly becoming the norm. As improving integrated circuit technology drives the size of the transistor down, the speeds at which they can switch goes up. And it is this switching speed that affects the integrity of digital signals.

Thankfully many potential signal integrity issues can be avoided by following good design principles and implementing the design as a controlled impedance board. Achieving this does require specific design tool capabilities - you need analysis tools that can detect nets with potential ringing and reflection issues, and board design tools that allow you to achieve the correct routing impedances. The PCB editor in Altium Designer has these capabilities.

This article will help you understand what causes signal integrity issues and if your board is likely to suffer from them. It will also discuss the two design approaches you must employ to minimizing potential SI issues ­- matching component impedances, and controlled impedance routing.

Controlled Impedance Routing: configuring the routing widths and clearances, as well as the material properties and dimensions, to deliver the required routing impedance(s).

When the Routing Becomes Part of the Circuit

As device switching speeds increase, so too do the demands on the printed circuit board designer and the fabricator. As the length of the signal switching edge becomes shorter than the length of the PCB trace that carries it, the trace has to be treated as part of the circuit. That trace has an impedance, which is referred to as the characteristic impedance (Zo).

The best way to manage the impact of these additional circuit elements is to design the trace routing so that the characteristic impedance is consistent over the length - a technique called controlled impedance routing.

The impedance of the trace routing is defined by the:

  • Cross-sectional area of the trace - determined from the width, the height (copper thickness), and the slope of the trace edges created during the etching process.
  • Distance from the trace to the reference plane(s) - the return path of the signal energy is as important as the signal's path, this return path follows the signal path in the adjacent reference plane(s).
  • Properties of the surrounding materials - the energy in the signal is not contained within the copper of the trace, due to the skin effect it also travels down the dielectric material that surrounds the trace. The permittivity of the dielectric material gives a measure of how much the dielectric impacts on the flow of that energy.

The Simbeor impedance calculator calculates the width(s) required to achieve the specified impedance. The Simbeor impedance calculator calculates the width(s) required to achieve the specified impedance.
The Simbeor impedance calculator calculates the width(s) required to achieve the specified impedance.

Do I Need Controlled Impedance Routing?

Do I need to bother with controlled impedance routing, you ask?

In an ideal situation, all of the energy that comes out of a component output pin would be coupled into the connected track on the PCB, flow through the PCB routing to the load input pin at the other end, and be absorbed by that load. If all the energy is not absorbed by the load then the leftover energy can be reflected back into the PCB routing, flowing to the source output pin. This reflected energy can interact with the original signal, adding to and subtracting from it (depending on the polarity of the energy), resulting in ringing. If the ringing is large enough, it will affect the integrity of the signal, resulting in unpredictable, erroneous circuit behavior.

So how do you know if this might occur? If the source pin is able to complete its edge transition before the signal reaches the load pin, the conditions exist for your design to be impacted by reflected energy. A common rule of thumb that is used to determine if SI issues are likely is the "1/3 rise time" rule. This rule states that if the trace is more than 1/3 of a rise time long, reflections (ringing) can occur. If the source pin has a 1 nSec rise time, a route longer than .33 nSec (which is approximately 2 inches in FR4) must be considered to be a transmission line, a candidate for signal integrity issues. If your devices have this sort of rise time and you know you will have routing of this sort of length, then you might end up with signal integrity issues on the PCB.

The speed at which the electrical energy can travel along the route is known as the propagation velocity, where:

Vp = speed of light / √ dielectric constant

Using:

Time = 1/3 * rise time
eR = 4 (approximation for FR4)
C = 11.811 in/nSec (speed of light, in inches per nanosecond)

√ is the square root symbol

To find the length of route above which the integrity of the signal could become a problem:

LR = Time * Vp
LR = Time * C / eR
LR = .33 * 11.811 / 2
LR = 1.95 in

How Do I Control the Impedances?

How do you avoid the situation where there is energy being reflected back and forth between the source and the load? You avoid it by matching the impedances. Impedance matching ensures that all the energy is coupled from the source into the routing, and then from the routing into the load. Routing the board with regard to the impedance is referred to as controlled impedance routing or another way of saying it is that a board where impedances have been managed is called a controlled impedance PCB.

There are two distinct elements to achieving impedance matching: the first is matching the components; the second is routing the board to give the required impedance.

Impedance Matching the Components

You cannot achieve a controlled impedance PCB with routing alone. First, you must check, and if necessary, match the impedances of the components.

Ideally, you want to detect nets that could have potential signal integrity issues during the design capture phase so that any additional termination components can be included before the board design process starts. Since output pins are low impedance and input pins are high impedance, it is likely that you will need to add termination components to the design to achieve impedance matching.

You can perform a signal integrity analysis on your design at the schematic capture stage. When you run the Tools » Signal Integrity command the Errors or Warnings dialog will often appear, indicating that not all components have signal integrity models assigned. The Signal Integrity analysis engine will automatically select default models based on the component designators, click Continue to use the defaults or Model Assignments to examine and change the models. You can access the Signal Integrity Model Assignments dialog at any time, via the Model Assignments button in the Signal Integrity panel.

The Signal Integrity analysis engine will use defaults for the required impedance and average track length. It will also use default values for the signal stimulus (the properties of the theoretical signal that is injected). These defaults can be configured once the Signal Integrity panel has opened, via the panel's Menu button » Setup Options command. This command opens the SI Setup Options dialog (show image), where the Supply Nets can also be configured. If the project includes a PCB, it will be checked for layer stack settings, as well as Supply Nets and Signal Stimulus design rules. Note that the Signal Integrity analysis engine requires power planes for the reference planes, it is not able to use a signal layer covered by a polygon.

The Signal Integrity analysis engine installs as a System Extension. If it is installed it will appear on the Installed list of the Extensions & Updates view, as shown below. If it is not currently installed, click the Configure button to install it.

Extensions add functionality to the design environment, they are managed in the Extensions & Updates view

Learn more about Extending Altium Designer

Analyzing the Design

When the Tools » Signal Integrity command is run the design is analyzed, any potential problem nets are identified in the Signal Integrity panel, as shown below.

The Signal Integrity analysis engine presents its screening results in the Signal Integrity panel Testing the design for potential signal integrity issues during design capture.

From the panel, you can perform a reflection analysis on a selected net (or nets). On the left is the analysis results for all nets in the design, select a net and click the Button to add the selected net(s) to the analysis region of the Signal Integrity panel button (or double-click a net name) to transfer that net to the Net field on the right of the panel, where you can perform a detailed analysis of that net, including:

  • Examining the pins in that net, where you can single-click to cross probe to that pin on the schematic, or double-click to check and configure the model assigned to that pin.
  • Enable one or more theoretical termination options for that net.
  • Perform a Reflection Analysis on the net, producing a set of waveforms showing the behavior at each pin in the net.

The panel allows you to experiment with possible termination configurations and values. Note that the Termination region of the Signal Integrity panel shown in the image above has the Serial Res option enabled. The section of the panel below that shows a series termination resistor. This is where you define the minimum and maximum theoretical series termination resistance values that will be used for the reflection analysis (disable the Suggest checkbox to enter your own values).

Exploring the Results

When the Reflection Waveforms button is clicked an accurate reflection analysis is performed on that net, with the results being presented in a new waveform window (*.SDF).

The waveform window will include:

  • A Chart for each net being analyzed, click the tabs at the bottom of the window to switch between Charts.
  • Each Chart will include a Plot for each pin in that net, showing signal behavior at that pin.

The images below show two graphs of the results at the input pin of the net selected in the previous panel image. The first graph is the input pin in the net without termination; the second graph shows six sweeps, one for the original unterminated net, then five sweeps with the theoretical series termination resistance included at the source pin.

Five passes of the reflection analysis were performed (Sweep Steps option value = 5), with the theoretical termination resistor stepping from Min = 20 ohms to Max = 60 ohms. The five passes (first pass at 20 ohms, last pass at 60 ohms) are listed on the right-hand side of the graph. Clicking on each label highlights that result and displays the theoretical termination resistance value at the bottom right. For this net, a series termination resistance of 40 ohms would produce the graph selected in the image on the right.

Graphical results of a reflection analysis performed on a net with ringing Reflection analysis results when the net includes a theoretical series termination resistor, with its value being sweptThe graph on the left shows the reflection analysis of a net with potential signal integrity issues; the graph on the right is the same net with a theoretical series termination resistor of approximately 40 ohms added.

To hide a floating panel, press F4 when the panel is active (the caption bar is colored). Press F4 to restore the display of the panel.

What Determines the Routing Impedance?

The second part of achieving a controlled impedance PCB is to route the board so that the tracks are a defined impedance. There are a number of factors that influence the impedance of your signal routing, including the dimensions of the routes and the properties of the materials used to fabricate the PCB.

The PCB editor includes the Simbeor® electromagnetic Signal Integrity engine from Simberian. Simbeor's model accuracy is validated through the use of advanced algorithms for 3D full wave analysis, benchmarking, and experimental validation. The Simbeor engine supports all modern board structures and materials.

The Simberian site also includes an extensive library of application notes and papers published by Simberian's principal developer, Yuriy Shlepnev, as well as papers written in collaboration with other leading industry and academic researchers.

The Simbeor SFS

Impedances are calculated by the Simbeor SFS, a quasi-Static Field Solver. Simbeor SFS is an advanced quasi-static 2D field solver based on Method of Moments, which has been validated by convergence, comparisons, and measurements. The solver meshes dielectric and conductor boundaries and solves corresponding equations to build frequency-dependent RLGC matrices for the Telegraph equations.

Simbeor SFS is not a full-wave solver as this is not needed to evaluate the impedance, delay, or attenuation in PCB interconnects, because of the quasi-TEM nature of the waves propagating there. Such waves can be accurately simulated with RLGC parameters extracted with a quasi-static 2D field solver.

A unique property of the Simbeor SFS solver is that it supports conductor roughness models. Note that it does not support a multi-layered conductor model (plating), and the roughness is common for all conductors. The solver is quasi-static because the solution does not include the high-frequency dispersion that takes place in microstrip lines (higher concentration of fields in a dielectric with higher dielectric constant at high frequencies).

Learn more about Simberian electromagnetic signal integrity technology

Supported PCB Structures

Impedances can be calculated for the following PCB structures:

  • Microstrip
  • Symmetrical Stripline
  • Asymmetrical Stripline
  • Single and differential coplanar structures
  • Multiple adjacent dielectric layers, with different dielectric properties.

Configuring the PCB for Controlled Impedance Routing

Controlled Impedance routing is all about configuring the dimensions of the routes and the properties of the board materials to deliver a specific impedance. This is done in the PCB editor's Layer Stack Manager. To open the Layer Stack Manager select Design » Layer Stack Manager from the main menus. The Layer Stack Manager opens in a document editor, in the same way as a schematic sheet, the PCB, and other document types do.

The trace width required to deliver a specific impedance is calculated as part of the impedance profile, configured in the Impedance tab of the Layer Stack Manager.

Based on:

  • The values of the Target Impedance, Target Tolerance and Roughness that you configure in the Impedance tab, and
  • the materials settings defined in the Stackup tab, including:
    • the thickness of the signal layer,
    • the thickness of the surrounding dielectric layers (the distances from the reference plane(s)), and 
    • the properties of the dielectric material (permittivity Dk, and dissipation factor Df).

When these are correctly configured, the impedance calculator has sufficient information to calculate the:

  • Trace Width
  • Calculated Impedance (Z)
  • Impedance Deviation (Z Deviation)
  • Propagation Delay (Tp)
  • Inductance per unit length (p.u.l.)
  • Capacitance per unit length (p.u.l.)

To improve calculation speeds, impedance profiles are calculated in separate threads (when available).

The calculated values are displayed in the Transmission Line section of the Properties panel, when the Impedance tab is selected in the Layer Stack Manager, as shown below.

A 50Ω  impedance profile defined for single nets routed on the top layer, hover the cursor over the image to display the settings for the same profile for layer L3 (image courtesy FEDEVEL Open Source, www.fedevel.com).A 50Ω impedance profile defined for single nets routed on the top layer, hover the cursor over the image to display the settings for the same profile for layer L3 (image courtesy FEDEVEL Open Source, www.fedevel.com).

Configuring the Layer Stackup

Main article: Defining the Layer Stack

The copper and dielectric fabrication layers are configured on the Stackup tab of the Layer Stack Manager.

  • Layers are added, removed, and configured in this tab. For a rigid-flex design, layers are also enabled and disabled in this tab.
  • The properties of the currently selected layer can be edited directly in the grid, or in the Properties panel. Click the Panels button, click to show or hide a workspace panel button at the bottom of the design space to enable the panel.
  • Right-click in the layer grid or use the Edit » Add Layer commands to add a layer. Adding a copper layer will also add a dielectric layer when an existing adjacent layer is also a copper layer.
  • If the Stack Symmetry option is enabled in the Board section of the Properties panel, layers are added in matching pairs, centered around the mid-dielectric layer.
  • The layer Material can either be typed into the selected Material cell; or selected in the Select Material dialog; click the ellipsis button (Ellipsis button, click to select a suitable material from the Select Material dialog) to open it.
  • A surface finish can be added to a copper layer. Use the Add Layer sub-menu to add a Surface Finish layer to the currently selected copper layer, then click the ellipsis button for the new surface finish layer to select the finish type.
  • The selected layer can be moved up or down within the layers of the same type using either the right-click or Edit menus.
  • The Board region of the Properties panel includes options to enforce Stack Symmetry and Library Compliance. More on these below.
  • The Board region of the Properties panel displays a summary of the currently selected stack (or substack for a multi-stack rigid/flex design).

Layer Stack Considerations

A fundamental requirement for controlling the impedance is to include a signal return path below each signal path. The Simbeor SI engine supports both plane layers, and signal layers covered by a polygon. These return-path layers should be distributed through the board stackup. Ideally, they are arranged so that there is at least one return-path layer adjacent to each signal layer that is carrying controlled impedance routing. The adjacent return-path layer provides the signal return path, and for reasons that will not be covered here, does so regardless of the DC voltage distributed by that plane.

The return path current flowing through the plane will attempt to follow the same physical path as the route on the signal layer, so it is important to avoid introducing discontinuities, such as a split or cutout in the return-path layer underneath any critical signal routing.

As well as selecting a suitable order for signal and plane layers, you also need to define the material properties of each layer, including:

  • Copper thickness
  • Dielectric thickness
  • Dielectric constant

These values, and the routing width, all contribute to the final impedance. Achieving the required impedance then becomes a process of tuning all these values. Keep in mind that possible copper and dielectric thickness values may also be limited, determined by the materials available from your PCB fabricator.

Learn more about possible layer stackups

Defining the Impedance Profiles

The Simbeor engine is built into the PCB editor's Layer Stack Manager (Design » Layer Stack Manager). To configure the layer stack for controlled impedance routing, switch to the Layer Stack Manager's Impedance tab where you can add and configure an impedance profile.

Impedance profiles are added and configured in the Impedance tab of the Layer Stack ManagerA 50Ω impedance profile defined for individual nets routed on the top layer, hover the cursor over the image to display the settings for the same profile for layer L3.

Notes on creating and configuring an Impedance Profile:

  1. In the Layer Stack Manager switch to the Impedance tab, as shown above.
  2. Click the Add Impedance Profile button, appears when there are no impedance profiles defined button (or the Plus button, click to add an additional impedance profile button if there is a profile already defined), to add a new profile.
  3. Define the required impedance Type, Target Impedance, and Target Tolerance in the Properties panel. The Description is optional, it will be displayed wherever the Impedance Profile name is displayed.
  4. The grid of layers is divided into 2 regions; the layers in the stackup are displayed on the left, then for each signal layer in the stackup, there is a layer displayed in the Impedance Profile region on the right. Use the layer checkbox in the Profile region to enable impedance calculation for that layer. Using the image above as an example and referring to the layer number shown in the left-most column, layers L1, L3, L10 and L12 have their layer checkbox ticked, enabling them for impedance calculations.
  5. When you click on an enabled layer in the Profile region, all layers in the layer stack will fade except those being used to calculate the impedance for that selected signal layer (as shown in the image above). Edit that layer's reference layer(s) in the Top Ref and Bottom Ref columns in the Impedance Profile region. Note that reference layer(s) can have a layer Type of either Plane or Signal. For example, in the image above, layer L10 in the stackup is enabled for impedance calculations, with the Top Ref set to 9-L9, which is a Plane layer, and the Bottom Ref set to 11-L11, which is a Signal layer. The software assumes that if a signal layer is being used as a reference plane, it contains a continuous plane of copper connected to a power or ground net.
  6. Enable the Impedance Profile checkbox for each other layer that will carry routing at this impedance, and configure the reference plane(s). Hover the cursor over the image above to display the S50 Impedance Profile for layer L3.
  7. If the calculated routing trace width is a value that cannot be ordered, you can tune the width and gap settings.

Tuning the Width and Gap Settings

From the target impedance and target tolerance, the software calculates the Trace Width. It is not uncommon that the calculated trace width will be a value that cannot be ordered, for example 0.0683mm. The fabricator will advise what material thicknesses are available and what precision they can achieve for trace widths. Then it becomes a process of starting at the desired values, then testing the impact on the calculated impedance values when the dimensions are adjusted to what is available.

To support this process of testing and tuning the settings, the impedance calculators support forward and reverse impedance calculations. The default mode is forward (enter the impedance, the software calculates the width). The  icon indicates the calculated variable.

A Target Impedance of 50Ω  gives a forward calculated width (W1) of 94.6µm, the image on the right shows the reverse calculation when the width (W1) is set to 95µm.  A Target Impedance of 50Ω  gives a forward calculated width (W1) of 94.6µm, the image on the right shows the reverse calculation when the width (W1) is set to 95µm. A Target Impedance of 50Ω gives a forward calculated width (W1) of 94.6µm, the image on the right shows the reverse calculation when the width (W1) is set to 95µm.

To reverse the calculation and explore different trace widths for the selected layer, type in the new Width (W1) value and press Enter on the keyboard. The calculated values will update to reflect the impact of changing to that width. Click the  button to return the calculator to forward calculation mode. Entering a new value into Width (W2) will change the Etch value.

To explore the differential pair transmission line results, nominate the calculated variable - either the Trace Width or Trace Gap - by clicking the appropriate button. Edit the other variable to change the Target Impedance, or alternatively change the Target Impedance to explore the impact on the other variable.

Press Enter on the keyboard to apply a value typed in to a field in the panel.

Etch Factor

The signal traces on a PCB are fabricated by etching away unwanted copper. Because the etchant starts etching away the copper at the surface, this copper spends more time in contact with the etchant. The result is the finished edges of the trace will have a slope, reducing the cross-sectional area of the finished trace, as shown in the image below.

The area of trace-edge copper lost (on both edges) during etching = X * Y

The amount of slope is referred to as the Etch Factor, where:

Etch Factor = Y/X

If Y = X, then the Etch Factor = 1

Referring to the image shown in the Properties panel:

Hover the cursor over the ? to show the formula.Hover the cursor over the ? to show the formula.

The standard definition for Etch Factor is to specify it as the ratio of  trace thickness / amount of over-etching. This gives the following formula:

Etch Factor = T/[0.5(W1-W2)]

The downside of this approach is that to specify no over-etching (meaning the trace edges are vertical), you would have to enter a value of inf (infinite) for the etch factor. To simplify specifying the amount of etch, the formula has been inverted so a value of 0 (zero) can be entered to indicate there is no over-etching.

Etch = [0.5(W1-W2)]/T

  • To exclude the Etch Factor from the calculations (specify there is no slope created along the trace edge), set the value to 0 (zero). The inverse value is used for the Etch Factor to simplify configuring for no etch.
  • Consult the board fabricator for information about the Etch Factor created by their processes.

Copper orientation

Another fabrication detail that contributes to the etch factor is the orientation of the copper. PCB traces are formed by etching away unwanted copper from a continuous sheet of copper laminated onto a dielectric substrate. The copper orientation defines the direction the copper projects away from that substrate. You can also think of it as the direction the copper is etched from, either above or below.

Click the Trace Inverted checkbox to toggle the Copper Orientation from Above to Below.  Click the Trace Inverted checkbox to toggle the Copper Orientation from Above to Below.Click the Trace Inverted checkbox to toggle the Copper Orientation from Above to Below.

The Copper Orientation can be edited in the Properties panel: in the Transmission line section (Impedance tab active), or in the Layer section (Stackup tab active). It can also be edited in the Layer Stack Manager grid, if the Copper Orientation column is currently being displayed in the Grid.

Copper layers also include an Orientation option. This field defines on which side of that copper layer the components are mounted on. Configure this when a rigid-flex design has an internal/flex layer with components mounted on it, or when the design uses embedded components, to indicate the direction the component is oriented relative to that copper layer.

Learn more about Defining and Configuring the Rigid-Flex Substacks

Learn more about Embedded Components

Conductor Surface Roughness

The surface of each of the copper layers in a printed circuit board has a degree of roughness. During PCB fabrication the surface of copper layers are treated to increase the roughness, to improve the adhesion between the copper and dielectric layers. This surface roughness becomes a significant contributor to conductor impedance at switching speeds above 10 GB/s. Through extensive research and analysis, industry experts have concluded that the surface roughness can be modeled by a roughness correction coefficient, derived from Surface Roughness and Roughness Factor values.

Roughness settings are available in the Layer Stack Manager mode of the Properties panel. These parameters are used only for conductive layers.

Surface roughness is included in the calculation of the characteristic impedance.Surface roughness is included in the calculation of the characteristic impedance.

Roughness:

  • Model Type - preferred model for calculating the impact of surface roughness (refer to the articles below for more information on the various models). Applies to all copper layers in the substack.
  • Surface Roughness - value of the surface roughness (available from your fabricator). Enter a value ​between 0 to 10µm, default is 0.1µm
  • Roughness Factor - characterizes the expected maximal increase in conductor losses due to the roughness effect. Enter a value between 1 to 100, default is 2.

Further reading

Support for Coplanar Transmission Line Structures

The impedance calculator in the Layer Stack Manager supports single and differential coplanar structures. Create a new impedance profile, then select Single-Coplanar or Differential-Coplanar from the Impedance Profile Type drop-down list.

Working with coplanar structures:

  • As with the standard single and differential impedances, values for each variable are automatically calculated based on the user-defined Target Impedance and Target Tolerance, and the physical properties of the board layers. These automatically calculated values can be adjusted by entering new values into the edit boxes of the Layer Stack Manager mode of the Properties panel.
  • To target the signal nets you want to be routed with a coplanar structure, configure a Routing Width (or Differential Pairs Routing) design rule with the Use Impedance Profile option enabled, and the required Coplanar Impedance Profile selected.
  • Coplanar structures require a reference plane on both sides of the signal route; this can be created by a polygon you place, or if stitching vias are added, by the Add Shielding to Net command (more info below). If you are placing a polygon, the separation between this polygon and the signal route is defined by the Clearance (S) value determined by Simbeor impedance calculator (displayed in the Properties panel, shown in the images above and below). Configure a Clearance design rule to control the clearance between the reference polygon and the signal route (show image).
  • It is common practice to include a via fence along each side of the signal trace when the coplanar structure is grounded, use the Tools » Via Stitching/Shielding » Add Shielding to Net command in the PCB editor to do this. As well as placing vias, by enabling the Add shielding copper option this command can also place a polygon around the signal routing to cover the via fence, as shown in the image on the right, below.
    Learn more about Via Shielding

The impedance calculator determines the signal properties and clearances (first image), use that clearance in the via shielding Distance setting.  The impedance calculator determines the signal properties and clearances (first image), use that clearance in the via shielding Distance setting.The impedance calculator determines the signal properties and clearances (first image), use that clearance in the via shielding Distance setting.

Selecting the Layer Material

In a controlled impedance design, the selection of the materials used in the layer stackup is very important.

For example, the most common material used to fabricate PCBs is glass fiber (fiberglass) reinforced epoxy resin, with copper foil bonded onto each side. The tightness of the weave of the glass fiber fabric affects the value and consistency of the dielectric constant Dk (permittivity) and Loss Tangent Df. Surrounding the woven glass fabric is resin - the percentage of resin used is also important in the performance of the material.

There is a large range of glass fiber weaves available. To help ensure the predictability and performance of the glass fiber-based materials used in PCB fabrication, the IPC have a standard for weaves:

IPC standard IPC-4412B: Specification for Finished Fabric Woven from "E" Glass for Printed Boards

  • The weave numbers detailed in the standard are the Constructions values displayed in the Altium Material Library dialog.
  • If the layer structure is symetrical enable the Stack Symmetry option in the Board section of the Properties panel. Each time you add a layer, a partner layer is automatically added in the other half of the stackup. 

The Material Library

As the designer, you can either edit the material properties directly in the Layer Stack Manager, or select materials from the Altium Material Library.

The entire library can be viewed (and added to) in the Altium Material Library dialog (Tools » Material Library).

The materials are organized into usage categories, accessed through a tree structure on the left of the dialog. Below this level, each usage category is broken into functional categories, such as: Conductive layer material, Dielectric layer material and Surface Layer Material; in the PCB layer material category.

Adding, Saving and Loading Material

New material can be added to the library when a specific material category is selected in the tree. Materials defined in an external material library can be loaded (Load button), and user-defined material that has been added in the Altium Material Library dialog can also be saved to a user-library (Save button). Only user-defined material is saved.

Adding Custom Properties to Material

Custom properties can be added to material detailed in the library (default and user-defined material). To add a custom property, first select the correct node in the tree on the left to define the material(s) it is to be added to, then click the  button to open the Material Library Settings dialog.

The required value can then be added to the selected material in the Altium Material Library dialog, select the row and click the Edit button.

Dielectric Material Behavior

The Dk/Df of PCB dielectrics are frequency dependent - for composite dielectrics Dk decreases with frequency while Df increases slightly (due to the relaxation-type of atomic polarization in such dielectrics).

The dispersion over frequency can be described with a multi-pole Debye model - which requires multiple frequency points to build. For PCB dielectrics, a simpler pole-continuous model has been developed - called Djordjevic-Sarkar or the Wideband Debye model. The model is analytical, causal and can be built with measurement of Dk/Df at just one frequency point - a much simpler but still accurate approach (for more information refer to the Material World tutorial #2016_01 in the Simberian Technical Presentations Library).

The Layer Stack Manager's impedance calculator uses the Wideband Debye model, with a default frequency value of 1 GHz. If a different frequency is required, pick the Dk/Df values from one frequency point from 1 to 10 GHz from the laminate specs and then use the characteristic impedance value computed at 1 GHz.

  • All calculations use a default frequency of 1 GHz.
  • If Df is undefined, the default value of zero is used.

Properties Panel

When the Impedance tab of the Layer Stack document is active, the Properties panel allows you to configure the Impedance Profile requirements. The required Impedance Profile can then be selected in the Routing Width or Differential Pairs Routing design rules.

  • Impedance Profile
    • Description – enter a meaningful description. This field is optional and will be displayed wherever the Impedance Profile name is displayed.
    • Type – use the drop-down to choose the impedance type. Choices are Single, Differential, Single-Coplanar, and Differential-Coplanar.
When working with coplanar structured impedances and the standard single/differential impedances, values for each variable are automatically calculated based on the user-defined Target Impedance and Target Tolerance, and the physical properties of the board layers. These automatically calculated values can be adjusted by entering new values into the edit boxes of the Layer Stack Manager mode of the Properties panel.
  • Target Impedance – enter the impedance you want to achieve.
  • Target Tolerance – enter the tolerance you want to achieve. You should consult with the fabricator to find a realistic value for tolerance that the fabricator can deliver.
  • Transmission Line
    • Trace inverted – enable this option to invert the trace, as demonstrated in the Properties panel. This option is the same as the Copper Orientation option displayed when the Stackup tab is active and defines the direction that the copper is laminated onto the core. The copper orientation defines the direction the copper projects away from that substrate. You can also think of it as the direction the copper is etched from, either above or below.
    • Etch – the Etch Factor is = T/[(W1-W2)/2], which reduces the total cross-section area of the trace by the thickness of the copper squared. Consult the board fabricator for information about the Etch created by their processes.
To exclude the Etch from the calculations (i.e. assume there is no slope created along the trace edge), set the value to 0.
  • Width (W1) / (W2) – W1 is the width of the trace you route, W2 is the width of the upper surface of that trace once it has been etched, with the Etch factor applied. There is a forward/reverse calculation feature available for trace width. The default is for the width to be calculated based on the Target Impedance you entered (forward calculation). That width may be a value that the fabricator may not be able to deliver, such as 5.978, and they will want a more sensible value, such as 6.0. You can enter 6.0 into the Width field and press Enter on the keyboard to recalculate the calculated values (Impedance, Deviation, etc.). The button turns gray (becomes inactive) and you are now in reverse calculation mode. If you click the button to make it active, you are again in forward mode and the Width (W1) will revert to the calculated value. This feature lets you explore realistic fabricate-able width options. Manually entering a value for W2 will update the etch factor to suit.
  • Impedance – the software calculates the impedance based on the properties of the materials used to make the board (copper, core and prepreg), and the cross-sectional area of the trace (determined by the width, thickness and etch factor of the trace).
  • Deviation – this is a measure of the difference between what you wanted (target impedance) and what you got (calculated impedance). The software calculates the impedance deviation (what you will actually get based on the material and dimensions entered) based on the properties of the materials used to make the board (copper, core and prepreg), and the cross-sectional area of the trace (determined by the width, thickness and etch factor of the trace).
  • Delay – this is the amount of time it takes for the signal to travel from the sender to the receiver.
  • Inductance – the impedance calculator uses the Impedance value to calculate the inductance per unit length.
  • Capacitance – the impedance calculator uses the Impedance value to calculate the capacitance per unit length.
  • Board
    • Stack Symmetry – enable to add layers in matching pairs, centered around the mid-dielectric layer. When enabled, the layer stack is immediately checked for symmetry around the central dielectric layer. If any pair of layers that are equidistant from the central dielectric reference layer are not identical, the Stack is not symmetric dialog opens.
    • Library Compliance – when enabled, for each layer that has been selected from the Material Library, the current layer properties are checked against the values of that material definition in the library.
When Stack Symmetry is enabled:
– An edit action applied to a layer property is automatically applied to the symmetrical partner layer.
– Adding layers will automatically add matching symmetrical partner layers.
  • Substack – this information is for the currently selected substack (layers, dielectric, thicknesses, etc.,). As you switch from one substack to another, this information will update accordingly (for the currently selected substack).
The Substack region will only be available if the Rigid/Flex option is enabled in the Features drop-down.
  • Stack Name – enter a meaningful substack name. This field is useful when the X/Y stackup region is being assigned a layer substack.
  • Is Flex – enable if the substack is flex.
  • Layers – the total number of layers.
  • Dielectrics – the total number of dielectrics.
  • Conductive Thickness – the thickness of conductive layer(s). Copper signal layers are referred to as conductive layers.
  • Dielectric Thickness – the thickness of dielectric layer(s).
  • Total Thickness – the total thickness of the board.
  • Other
  • Roughness – shows roughness of conductive layers.
    • Model Type – preferred model for calculating the impact of surface roughness (refer to the articles below for more information on the various models). Applies to all copper layers in the stack (should it be the substack?).
    • Surface Roughness – value of the surface roughness (available from your fabricator). Enter a value ​between 0 to 10µm, default is 0.1µm
    • Roughness Factor – characterizes the expected maximal increase in conductor losses due to the roughness effect. Enter a value between 1 to 100, default is 2.

Configuring the Design Rules

The routing impedance is determined by the width and height of the route, and the properties of the surrounding dielectric materials. Based on the material properties defined in the Layer Stack Manager, the required routing widths are calculated when each impedance profile is created. Depending on the material properties, the width may change as the routing layer is changed. This requirement changes widths as you change routing layers is automatically managed by the applicable routing design rule configured in the PCB Rules and Constraints Editor (Design » Rules).

For most board designs, there will be a specific set of nets to be routed with a controlled impedance. A common approach is to create a net class or differential pair class that includes these nets, then create a routing rule that targets this class, as shown in the images below.

Normally you manually define the Min, Max, and Preferred Widths, either in the upper constraint settings to apply them to all layers; or individually for each layer in the layer grid. For controlled impedance routing you enable the Use Impedance Profile option instead, then select the required Impedance Profile from the dropdown. When this is done, the Constraints region of the rule will change. The first thing you will notice is that the available layers region will no longer show all signal layers on the board, it will now only show the layers enabled in the selected Impedance Profile. The Preferred Width values (and diff pair gap) will update to reflect the widths (and gaps) calculated for each layer. These Preferred values cannot be edited but the Min and Max values can; set these to suitable smaller/larger values. The nets can then be interactively routed, in the usual way.

  • When an Impedance Profile is applied all other signal layers are removed from the design rule constraint, as it is assumed that the targeted nets will only be routed on those layers.
  • The Preferred Width is locked to the values calculated in the Impedance Profile, the Min Width and Max Width values can still be user-defined.
  • If the dimensions are set to metric, the Min Width and Max Width settings may need to be made slightly smaller/larger to avoid false design rule violations caused by rounding errors.

Routing Width Design Rule

For single-sided nets, the routing width is defined by the Routing Width design rule.

When the Routing Width design rule is set to Use an Impedance Profile, the preferred width settings come from the profileWhen you choose to Use an Impedance Profile, the available layers and Preferred Widths are controlled by the selected profile.

Differential Pairs Routing Design Rule

The routing of differential pairs is controlled by the Differential Pair Routing design rule.

When the Diff Pair Routing design rule is set to Use an Impedance Profile the preferred width settings come from the profileFor a differential pair, the available layers, the Preferred Width and the Preferred Gap are controlled by the selected profile.

Learn more about Differential Pair Routing

Return Path Design Rule

Breaks or necks in the return path can be detected by the Return Path design rule. The Return Path design rule checks for a continuous signal return path on the designated reference layer(s) above or below the signal(s) targeted by the rule. The return path can be created from fills, regions, and polygon pours placed on the reference signal layer, or it can be a plane layer.

The return path layers are the reference layers defined in the Impedance Profile selected in the Return Path design rule. These layers are checked to ensure the specified Minimum Gap (width beyond the signal edge) exists along the signal's path. Add a new Return Path design rule in the High Speed rule category.

The return path layers are defined in the selected Impedance Profile, the path width (beyond the signal edge) is defined by the Minimum Gap.The return path layers are defined in the selected Impedance Profile, the path width (beyond the signal edge) is defined by the Minimum Gap.

The image below shows return path errors detected for the signal, NetX, with a Minimum Gap setting of 0.1mm. It can be easier to locate Return Path errors by configuring the DRC Violation Display Style to show Violation Details but not the Violation Overlay ( show image) in the Preferences dialog. Doing this highlights the exact locations where the rule has failed rather than the entire object(s) in violation. 

To avoid detecting small errors, such as the section highlighted in the diagonal track segment in the image above, configure the PCB.Rules.ReturnPathIgnoreArea setting in the Advanced Settings dialog. The default is to ignore areas < 10 sq mils.

Learn more about High Speed Design in Altium Designer

Routing Nets at the Required Impedance

As you route the board and change layers, the software will automatically adjust the track width to the size needed to achieve the specified impedance. This interactive controlled impedance routing greatly simplifies the task of designing a controlled impedance PCB.

Neither the Simbeor impedance calculator integrated into the Layer Stack Manager or the Signal Integrity Analysis engine include vias in their calculations. Learn more about Defining the Via Types.

Length Tuning the Routes

Two of the core challenges with routing a high-speed design are controlling the impedance of the routes, and matching the lengths of critical nets. Impedance-controlled routing ensures that the signal that leaves an output pin is correctly received by the target input pins. Matching the route lengths ensures that timing-critical signals arrive at their target pins at the same time. Tuning and matching route lengths is also an essential ingredient of differential pair routing.

Accordion patterns have been added into the routing to ensure that the differential pairs have matched lengths. Accordion patterns have been added into the routing to ensure that the differential pairs have matched lengths.

The Interactive Length Tuning and Interactive Diff Pair Length Tuning commands (Route menu) provide a dynamic means of optimizing and controlling net or differential pair lengths by allowing variable amplitude wave patterns (accordions) to be inserted, according to the available space, rules, and obstacles in your design.

Learn more about Length Tuning

Testing the Signal Integrity of the Routed Board

In the same way that you tested the nets during design capture using an assumed routing length and routing impedance, once the routing is complete, you should repeat this process on the board to check for potential impedance mismatches and reflection issues. Launch the Signal Integrity command from the PCB editor Tools menu. Since the PCB is part of the project, the material properties and dimensions defined in the Layer Stack Manager and the actual widths of the routes on the board will be used to calculate the impedances used for the signal integrity tests.

Achieving the Specified Impedances

Beyond the iterative dimension tuning process that you go through to achieve the correct impedances, there are other factors that influence the final impedance that will be achieved on your fabricated PCB. These include the consistency and stability of the dielectric material used in the PCB, and also the consistency and quality of the etching process. If you require a controlled impedance PCB, you should discuss this with your PCB fabricator. Some fabricators can advise on track geometries if you supply them with your preferred stackup. Many will also be able to include an impedance test coupon on each panel that they fabricate - this can be used to measure the real impedances achieved on the board.

Additional Reading and Resources

This article gives an introduction to the topic of signal integrity and controlled impedance PCB design. Use the following links to learn more, where you can access resources developed by recognized industry experts.

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

お問合せ

お近くの営業所にお問合せください。

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: