Creating an xSignal in Altium Designer

An xSignal is a designer-defined signal path between two nodes; they can be two nodes within the same net or they can be two nodes in different nets.

xSignals are defined using the following methods:

  1. Use the xSignals Multi-Chip Wizard. This will be the most common approach to creating xSignals and is described below.

Alternatively, the following methods are used by selecting objects of interest first, then choosing the appropriate command:

  1. Create a single xSignal based on selected pads. Select the required start pad and end pad (these pads can be in different nets if there is a series termination component). Pads can be directly selected in the design space, or the PCB panel can be used in Nets mode to locate and select the pads (as shown in the image below). Once the pads are selected, either right-click on a selected pad in the design space then run the xSignals » Create xSignal from Selected Pins command, or right-click on one of the selected pads in the PCB panel and run the Create xSignal command. The new xSignal will be listed in the xSignals mode of the PCB panel.

    When you are defining an xSignal based on selected pins (footprint pads), select only the start pad and the end pad before running the Create command.

    The name of the new xSignal will be a combination of the two net names, separated by a hyphen. The xSignal name can be edited in the xSignals mode of the PCB panel.

    The new xSignal can be added to an xSignal class, right-click in the xSignal Classes region of the panel to create a new class and add members to it.

  2. Select the source component, then right-click on the selected component and choose the xSignal » Create xSignals between Components command from the context menu. The Create xSignals Between Components dialog will open, with the chosen source component selected. The dialog is described below.
  3. Select one or more series components in the design space then right-click on one of the selected components and choose the xSignal » Create xSignals from Connected Nets command from the context menu. The Create xSignals From Connected Nets dialog will open. The chosen source component, and the nets connected to that component, will be selected. The dialog is described below.
  4. There may also be situations where you wish to create an xSignal within an existing xSignal, in this situation the xSignal mode of the PCB panel can be used. Ensure that the Select option is enabled at the top of the panel, locate the current xSignal, select the required pads in the xSignal Primitives section of the panel, then right-click on one of the selected pads in the design space and use the method described in step 2 of this list to complete the process.

Select the two pads in the Nets mode of the panel, right-click on one of the selected pads then choose Create xSignal. Note that the pads are in different nets.
Select the two pads in the Nets mode of the panel, right-click on one of the selected pads then choose Create xSignal. Note that the pads are in different nets.

If the start and end pads are in the same net, an xSignal will take a name in the form <NetName>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net. If the start and end pads are in different nets, an xSignal will take a name in the form <StartNet>_<EndNet>_PPn, where n is the next available integer used to distinguish multiple xSignals defined for that net combination.
Note that xSignals can also be created using the Constraint Managerlearn more.

xSignals Multi-Chip Wizard

The xSignals Multi-Chip Wizard is used to create xSignals between a single source component and multiple target components. The Wizard uses a component-oriented approach to identifying potential xSignals – you select a single source component, the nets of interest and the target components and the Wizard then analyzes all potential paths from the source component to the designation components, passing through series passive components and along any branches. As the designer, you then can choose the xSignals you would like to have generated and you can also create Matched Length design rules if required. The Wizard also can be used to automatically create xSignals and xSignal classes for a number of different common interface and memory circuits.

 In this Wizard, an output pin is referred to as the Source, and the target input pin is referred to as the Destination.

The Wizard is also a multiple-run tool – from the overall master group of xSignals that you initially create on the xSignal Routes page, you can select a sub-set of these, define classes and rules, then return to the master group, choose another sub-set, define classes and rules for them, and so on.

One of the great strengths of the Wizard is the ease of working between the Wizard and the PCB editor. Click on an xSignal on any page of the Wizard and the pads and any routing are visually highlighted on the PCB.

At this stage, the Wizard does not support the automatic addition of T-junction identifiers, often referred to as tie-points or branch-points. If your design includes branched routing, it is suggested that you:

  1. Tune the length from the source component to the passive component (such as a series termination resistor), if there are any.
  2. Tune the length in each branch, from the T-Junction to the destination component.
  3. If required, tune the remaining length between the passive component (or from the source if there are no passives) to the T-junction.
If you need to tune the lengths of just the branches, create a user-defined branch point by placing a single-layer, single-pad component within the routing at the T-junction. Refer to the Defining the Branch Point in a Balanced T Pattern section below for more information.

To access the xSignals Multi-Chip Wizard, select the Design » xSignals » Run xSignals Wizard command from the main menus or right-click in the PCB layout and then select xSignals » Run xSignals Wizard. The opening page of the Wizard will be shown.

The opening page of the xSignals Multi-Chip Wizard
The opening page of the xSignals Multi-Chip Wizard

xSignals Multi-Chip Wizard Modes

On the second page of the Wizard, you will be asked to select either Custom Multi-Component Interconnect, On-Board DDR3 / DDR4, or USB 3.0. The Custom Multi-Component Interconnect mode is used to define multiple xSignals between a chosen source component and multiple target components, while the On-Board DDR3 / DDR4 mode is used to create xSignals for your DDR3 or DDR4 memory. The USB 3.0 mode creates the xSignals, xSignal Classes, and Matched Length rules for each USB 3.0 channel. Select the appropriate mode for your needs.

Create xSignals Between Components Dialog

If you have a large number of xSignals to define, it is more efficient to use the Create xSignals Between Components dialog. Accessed via the Design » xSignals » Create xSignals command, the dialog presents Source and Destination components, and allows you to create one or many xSignals in a single operation.

Use the dialog to quickly identify and create multiple xSignals and add them to the required xSignal class.
Use the dialog to quickly identify and create multiple xSignals and add them to the required xSignal class.

The approach is to:

  1. Select a single Source Component.
  2. Select one or more required Destination Components.
  3. Select the Source Net(s) of interest. All nets currently connecting to the chosen source component will be listed. For nets associated with a specific class, choose that class form the Net Class drop-down.
  4. Click the Analyze button. The software attempts to identify potential xSignals that exist between the chosen source and destination components for the selected nets. All possible xSignals that include the chosen nets and run between the chosen source and destination components will be listed in the xSignals field. Note that the analysis algorithm follows the current topology of the chosen nets and this will influence the proposed xSignals.
The software can also search through series components, if required, by selecting the appropriate option in the Analyze drop-down: Search for direct connections, Through 1 series component, Through 2 series components, or Multipath coupled nets.
  1. After analysis has been performed, potential xSignals will be listed in the lower region of the dialog, and all will be enabled for creation. Carefully check through the list of proposed xSignals, and enable only those that are required. Use commands available on the right-click context menu to toggle multiple entries.
  2. Select the required class at the bottom of the dialog, or type in a name to create a new class. If no class is chosen, the xSignals are still created and you can add them to any xSignal class in the Object Class Explorer dialog (Design » Classes). Using classes can greatly simplify the creation and configuration of design rules.
  3. Click OK to create the xSignals.

The dialog will close and you will be returned to the design space. The new xSignals will be listed in the xSignals mode of the PCB panel.

Use the filters above each list to quickly locate the components or nets of interest; wildcards are supported.

Create xSignals From Connected Nets Dialog

If you are creating xSignals that include series termination components, a good approach is to use the Create xSignals from connected nets command. The command is available whenever a component is selected either via Design » xSignals sub-menu from the main menus or the right-click xSignals sub-menu.

This command is designed to build xSignals outward from a selected series termination component, such as a resistor or capacitor. It supports both one or more discrete components, and one or more multi-instance pack-style components, such as resistor networks. After running this command, the Create xSignals From Connected Nets dialog will open.

Use the dialog to create xSignals that span across a selected series component. In this example, two possible xSignals were proposed, only one is going to be created.
Use the dialog to create xSignals that span across a selected series component. In this example, two possible xSignals were proposed, only one is going to be created.

The approach is to:

  1. Select a single Source Component.
  2. Select the Source Net(s) of interest. All nets currently connecting to the chosen source component will be listed. For nets associated with a specific class, choose that class form the Net Class drop-down.
  3. Click the Analyze button. The software attempts to identify potential xSignals that exist for the chosen source components and for its selected nets. All possible xSignals will be listed in the xSignals field.
  4. After analysis has been performed, potential xSignals will be listed in the lower region of the dialog, and all will be enabled for creation. Carefully check through the list of proposed xSignals, and enable only those that are required. Use commands available on the right-click context menu to toggle multiple entries.
  5. Select the required class at the bottom of the dialog, or type in a name to create a new class. If no class is chosen, the xSignals are still created and you can add them to any xSignal class in the Object Class Explorer dialog (Design » Classes). Using classes can greatly simplify the creation and configuration of design rules.
  6. Click OK to create the xSignals.

The dialog will close and you will be returned to the design space. The new xSignals will be listed in the xSignals mode of the PCB panel.

Use the filters above each list to quickly locate the components or nets of interest; wildcards are supported.

The Role of the Net Topology

When you define an xSignal, it is between two nodes or pads. However, when you select that xSignal in the xSignals mode of the PCB panel, it will actually follow the path of the connection lines that runs between those two pads, indicating that this is the path that the software assumes the xSignal will be routed. The reason it does this is because it is obeying the topology defined for that net. Net topology is defined by the applicable Routing Topology design rule; the default topology is Shortest.

The simple animation shows a CPU connected to four DDR3 memory chips, which is going to be routed using a fly-by routing strategy. The DRAM_A2 xSignal class contains four xSignals. First, the class is selected, then each xSignal is selected in turn. You can see how the xSignal path follows the topology of the net, which is currently set to the default - Shortest.

Because the net topology is currently set to Shortest, the xSignals are not following the required path from the processor to the memory chips.
Because the net topology is currently set to Shortest, the xSignals are not following the required path from the processor to the memory chips.

If you plan on using the Create xSignals Between Components dialog, you will need to configure the topology of the net(s) to ensure the xSignal analysis algorithm understands the intended path of the routed xSignal.

xSignal Creation Commands

Apart from the Design » xSignals » Create xSignals command, there are other xSignal creation commands in the xSignals sub-menu when certain conditions are met.

Below is a summary of the commands and when they are available:

Command Description
Create xSignal from selected pins

Immediately creates a single xSignal. This command is available when there are two or more pads selected in the design space, and is the same command presented when you right-click on one of the selected pads.

Create xSignals between components

This command is available when components are selected in the design space. When it is run the Create xSignals Between Components dialog opens with the component(s) pre-selected. Ensure that the correct Source and Designation components are selected, then complete the Analysis/Creation process.

After launching the command, the Create xSignals Between Components dialog will open. Use the dialog to create your xSignals as follows:

  1. The chosen source component will appear selected in the Source Component region.
  2. Any other component(s) selected in the workspace will appear selected in the Destination Components region. If not, make your choice(s) now.
  3. By default, all nets associated with the pads of the source component will be selected (in the Source Component Nets region). Adjust this selection as required.
  4. Click the Analyze button - the software attempts to identify potential xSignals that exist between the chosen source and destination components, for the selected nets.

    Note that the analysis algorithm follows the current topology of the chosen nets.
    The software can also search through series components if required, by selecting the appropriate mode from the button's associated drop-down menu. Modes available are: Search for direct connections, Through 1 series component, Through 2 series components, and Multipath coupled nets.
  5. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
  6. You can optionally have the created xSignals associated to an xSignal class. Either choose an existing xSignal class or enter a name for a new class. You can leave the field blank if you wish; the xSignals can always be added as members to the required class at a later stage.
  7. Click OK to create the xSignals. The dialog will close and you will be returned to the design space, which presents a filtered view showing the newly created xSignals. If an xSignal class was specified, this will be created (if not existing) and the xSignals associated to it.
Create xSignals from connected nets

Use this command when there are one or more series termination components to create xSignals for. Select the termination component(s), then run the command to open the Create xSignals from Connected Nets dialog, ready to complete the process of creating a set of xSignals. Use the dialog to create your xSignals as follows:

  1. The chosen source component(s) will appear selected in the Source Component region.
  2. By default, all nets associated with the pads of the source component(s) will be selected (in the Source Component Nets region). Adjust this selection as required.
  3. Click the Analyze button - the software attempts to identify potential xSignals that exist for the selected nets emanating from the chosen component(s).

    Note that the analysis algorithm follows the current topology of the chosen nets.
  4. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
  5. You can optionally have the created xSignals associated to an xSignal class. Either choose an existing xSignal class or enter a name for a new class. You can leave the field blank if you wish; the xSignals can always be added as members to the required class at a later stage.
  6. Click OK to create the xSignals. The dialog will close and you will be returned to the design space, which presents a filtered view showing the newly created xSignals. If an xSignal class was specified, this will be created (if not existing) and the xSignals associated to it.
Create xSignals

Opens the Create xSignals Between Components dialog. This command is always available. Use the dialog to create your xSignals as follows:

  1. Choose a source component in the Source Component region.
  2. Choose one or more destination components in the Destination Components region.
  3. All nets associated with the pads of the source component will be listed in the Source Component Nets region. Select the nets of interest.
  4. Click the Analyze button - the software attempts to identify potential xSignals that exist between the chosen source and destination components for the selected nets.

    Note that the analysis algorithm follows the current topology of the chosen nets.
    The software can also search through series components if required, by selecting the appropriate mode from the button's associated drop-down menu. Modes available are: Search for direct connections, Through 1 series component, Through 2 series components, and Multipath coupled nets.
  5. All identified xSignals are listed in the xSignals region of the dialog. By default, all are selected for creation - adjust this as required.
  6. You can optionally have the created xSignals associated to an xSignal class. Either choose an existing xSignal class or enter a name for a new class. You can leave the field blank if you wish; the xSignals can always be added as members to the required class at a later stage.
  7. Click OK to create the xSignals. The dialog will close and you will be returned to the design space, which presents a filtered view showing the newly created xSignals. If an xSignal class was specified, this will be created (if not existing) and the xSignals associated to it.

Defining the Branch Point in a Balanced T Pattern

One of the challenges of a Balanced T routing strategy is how to equalize the length of the trunks and the branches beyond the T points. The available nodes in the net are only at the pads, so it is not possible to define separate xSignals for the trunk, and from the branch point to the end of each branch. The branch points are indicated by the red dots in the image below.

One way to solve this problem is to add a single pin component to the net. Create a component with a single pad that is the size of the vias being used in the design. If the branch point component pad is single-layer, then it can also be used in combination with a blind or buried via, by placing it on the via's start or end layer, giving complete flexibility as to how the routing is created. If you only want to include the branch point component on the PCB, set the branch point component's Type to Mechanical to exclude it from the BOM, and prevent any synchronization issues with the schematic. If you plan on including the branch point component on the schematic, the component Type can be set to Standard (no BOM).

Balanced T routing can require matched lengths between intermediate branch points.
Balanced T routing can require matched lengths between intermediate branch points.

Because the branch point is a node in the net, you can now define xSignals for just the trunk, for each major branch, and for each minor branch, if needed. These can then be used to scope matched length design rules, giving the designer complete control over how finely the length matching is to be performed. 

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

Altium 제품에 접근할 수 있는 레벨에 따라 사용할 수 있는 기능이 달라집니다. 다양한 레벨의 Altium Designer Software Subscription에 포함된 기능과 Altium 365 플랫폼에서 제공하는 애플리케이션을 통해 제공되는 기능을 비교해보세요.

소프트웨어에서 논의된 기능을 찾을 수 없는 경우, Altium 영업팀에 문의하여 자세한 정보를 확인해주세요.

콘텐츠