Defining Design Requirements Using the Constraint Manager in Altium Designer

The Constraint Manager is a document-based, spreadsheet-like user interface that allows you to view, create, and manage the design constraints used for your PCB designs.

Some of the advantages of using the Constraint Manager, especially for complex designs with many nets, classes, etc., are:

• Availability at the project level that makes the access to the design constraint management similar from both schematic capture and PCB design domains.
• A shift from query-based rule scoping to an applied object type matching simplifies constraint rule creation.
• Use of constraint sets to expedite the process of defining the constraints.
• Rule priority is automatic based on the natural hierarchy of design objects.
• Using a document-based presentation interface rather than a dialog means that the schematic and PCB editor and its associated functions remain active and accessible.

Accessing the Constraint Manager

The Constraint Manager is accessed by selecting the Design » Constraint Manager command from the main menus of the schematic or PCB editor.

Access the Constraint Manager from the schematic editor

Access the Constraint Manager from the PCB editor

Constraint Types

Using the buttons at the top left of the Constraint Manager, you can switch between its views to define different constraint types.

Working with the Clearance Matrix

By default, the clearance matrix in the Clearances view of the Constraint Manager includes a single All Net Classes to All Net Classes entry with which you can define a default clearance value between any nets in the design. Use the Add control at the top left of the matrix (or right-click any cell in the clearance matrix and use the Add command from the context menu) to show a pop-up with a list of currently defined net and differential pair classes. Select one or more required classes (multiple class entries can be selected using the Shift+Click or Ctrl+Click technique) and click the Add button. A row and a column for each selected class will be added to the matrix.

Click a cell where the row and column of two classes intersect to select it and show the detailed clearance settings at the lower part of the Constraint Manager, where you can define specific clearance values between different objects and on different layers.

❯ ❮ Javascript ID: CM_Clearances_AD24_3

Click a cell in the clearance matrix to access settings for the corresponding class pair that is denoted in the lower part. Use the Clearance field in the lower part to enter the required value that will be applied to all object pairings and all layers for this class pair. Alternatively, double-click a cell in the matrix in the upper part to directly enter the required value. Enter the required clearance values for specific object pairs in the table. Note that the cell in the clearance matrix shows the range of minimum and maximum values defined in the table. Multi-editing within a selected row/column is supported in the detailed clearance settings. Click the header of a row or column to select it, type the required value, and press Enter or click to apply this value to all cells of the row/column. Note that if you change a track-to-primitive value, that same clearance will be applied to text-to-primitive. Using the tabs below the table, you can also define clearance values by layers. Use the Add control to add a tab for a specific layer. Note that when the Constraint Manager is accessed from the schematic editor, only the Top and Bottom layers can be added as specific layers. When the Constraint Manager is accessed from the PCB editor, any signal layer currently present in the PCB design can be added. To quickly define values for the inner and outer layers, you can also enter two values delimited by a slash (e.g., 5/6) in a cell in the clearance matrix at the top. The first value will be applied to the inner layers, and the second value will be applied to the outer layers.

Notes on working with the Clearances view:

• Entering a value into a cell in the clearance matrix or into the Clearance field will automatically apply that value to all of the fields in the grid region in the lower part of the Constraint Manager when a cell in the clearance matrix is selected. You only need to edit in the grid region when you need to define a clearance based on the object type.

• In the detailed clearance settings at the lower part of the Constraint Manager, you can also enable the Creepage constraint for the selected classes and define the creepage value – show image. This constraint tests the creepage distance between the targeted signals across the board surface through unplated holes, cutouts, and around the board edge. 

• To reset the clearance value for a specific object pair (for example, a Track to Track pair) to its default (i.e. to the value defined for the All Net Classes to All Net Classes entry), select its cell in the bottom table and press the Delete key or right-click the cell and select the Reset to Default command from the context menu.

• To reset the clearance value for all object pairs of a specific entry in the clearance matrix (for example, a net class and another net class entry) to their defaults, right-click the corresponding cell in the clearance matrix and select the Remove Rule command from the context menu.

• To remove a class from the clearance matrix, right-click any cell in the row for this class in the clearance matrix and select the Remove Scope command from the context menu.

Working with Physical and Electrical Constraints

When in the Physical or Electrical view of the Constraint Manager, click a cell in the grid area to show the settings of the corresponding rule(s) at the lower part of the Constraint Manager, where you can define their constraint values.

❯ ❮ Javascript ID: CM_PhysicalElectrical_AD24_3

Notes on working with the Physical or Electrical views:

• The Constraint Manager defines the priorities of the rules in these views automatically: the priority is ordered from All (lowest) to object class to object (highest).

• To remove custom constraint values defined by a specific rule (effectively, reset values for this rule to its defaults), right-click the corresponding cell in the grid and select the Remove rule command from the context menu.

• To remove custom constraint values by all rules for an object, right-click any cell in the row for this object in the grid and select the Remove rules from scope command from the context menu.

• All nodes, except those predefined (e.g., All Nets), are collapsed in the Physical and Electrical views by default. You can use the Expand All and Collapse All right-click menu commands to control the grid nodes.

• When a value is entered in the Physical view's top grid for a single net or xNet (Min Width or Preferred Width), differential pair (Min Width, Preferred Width, or Preferred Diff Pair Gap) or net/xNet/diff pair class, this value will be propagated to corresponding width (Min Width/Preferred Width/Max Width) or gap (Min Gap/Preferred Gap/Max Gap) fields in the constraint regions below. Note that an entered value will be propagated to other fields only if the object does not have the specific rule defined.

Configuring Constraint Values per Layer

When accessing the Constraint Manager from the schematic, you can configure the Width and Differential Pairs Routing constraints for layers in a chosen layer stack.

Using the drop-down at the top of the Constraint Manager, select an entry for a specific PCB document of the design project. If the selected PCB contains multiple layer stacks, you can choose the required stack for which constraints need to be configured using tabs in the lower part of the Constraint Manager when the corresponding rule is selected. Also, you can use a chosen Impedance Profile (where defined as part of the selected PCB’s layer stack).

Defining Differential Pairs

Differential pairs are created from the Physical view or from the Diff Pairs tab of the Electrical view of the Constraint Manager. For the Constraint Manager to create differential pairs from nets, the nets to be paired must have a consistent naming scheme (i.e. they have a common root followed by a consistent positive/negative suffix, for example, TX0_P and TX0_N).

Right-click anywhere in the grid area of the Physical view or the Diff Pairs tab of the Electrical view and select the Differential Pairs » Create Differential Pairs From Nets command from the context menu to open the Create Differential Pairs From Nets dialog to define differential pair creation options. The filters at the top of the dialog enable you to quickly target these nets in terms of the net class to which they belong and the particular differentiating factor that has been used to distinguish the positive and negative nets in an intended pairing, for example, _P and _N. You can also define a prefix to be added to the differential pair objects created and determine to which differential pair class they will be added.

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

When all options are set as required, click the Execute button – the differential pair objects will be created and shown in the Physical view of the Constraint Manager, with constituent nets listed under their entries.

The Diff Pairs tab of the Electrical view can also be used for explicitly managing differential pairs. A hierarchical list of the differential pairs in the design is shown on this tab. Select a cell for a differential pair or differential pair class to present constraints for it in the lower part of the Constraint Manager.

Defining xNets

A path from a source component to a destination component passing through one or more series components can be defined as an xNet.

Comma-separated lists of prefixes for designators of components that can be used as source or destination components (Sources/Destinations) and series components (Discretes) can be defined in the xNets Creation region of the Options tab of the Project Options dialog.

The xNets Creation region of the Options tab of the Project Options dialog

An example path that can be defined as an xNet in the Constraint Manager (according to the xNet creation settings shown above)

In the Physical or Electrical view of the Constraint Manager (when it is accessed from either a schematic or PCB), right-click a net to be included in a new xNet and select the xNets » Create xNets From Selected Nets command from the context menu. A new xNet will be created and shown in the Physical or Electrical views of the Constraint Manager, with constituent nets listed under its entry.

Defining xSignals

From the Constraint Manager, you can also define xSignals – user-defined signal paths between two nodes in the PCB. When in the Electrical view of the Constraint Manager, select the cell in the Topology column for a net or xNet, choose Custom from the drop-down in the lower part of the Constraint Manager, and then use the provided controls to define the custom topology and select corresponding xSignals.

An example of defining xSignals for an xNet shown below is described and demonstrated thereafter.

An example of xNet for which xSignals should be created.

A custom topology can be defined using the topology graph in the lower part of the Constraint Manager. Use the right-click menu in the graph area to add and remove nodes and change their type from Source to Destination and back and Click, Hold&Drag the nodes to define the tolopogy.

The list of proposed xSignals (named using the <SourceNetName> (<SourcePinDesignator> → <DestinationPinDesignator>) scheme) appear at the right of the grid area. The list is divided into two groups: xSignals going from a source to a destination (S-T) and xSignals going from one destination to another (T-T). Use checkboxes for groups or individual xSignals to select/deselect xSignals to be created. Selected xSignals will appear on the xSignals tab of the Electrical view.

An example of creating xSignals using the topology graph

Alternatively, a custom topology can be defined using the table. Add the required pins and serial components using the Pin column, select their roles (Source, Destination, or Discrete) using the Role column, and define the desired order using the Order column.

An example of creating xSignals using the table user interface

For a created xSignal class (refer to the Defining Classes section below for details), the Tolerance constraint can be defined, and an xSignal within this class can be selected as Matching Length. When the Constraint Manager is accessed from the PCB side, the Actual Value and Margin columns are also available.

In the PCB document, the defined xSignals can be browsed from the PCB panel in its xSignals mode. Also, corresponding From-Tos will be created and can be browsed from the PCB panel in its From-To Editor mode.

❯ ❮ Javascript ID: CM_xSignals_PCB_AD23_11

In the PCB document, the generated xSignals can be browsed from the PCB panel in its xSignals mode. From-Tos will also be generated, and they can be browsed from the PCB panel in its From-To Editor mode.

Defining Classes

The Constraint Manager allows you to define classes of nets, differential pairs, xNets, and xSignals.

• To add objects in the Physical or Electrical view of the Constraint Manager to an existing class, select multiple object entries using the Ctrl+Click, Shift+Click, or Click, Hold&Drag technique, then right-click the selection and choose the required class from the Classes » Add Selected to Class sub-menu of the context menu.

  

  When there are more than 30 classes, the Classes » Add Selected to Class » Existing Class command is presented instead of the list of classes. Use this command to access a dialog where you can select an existing class to which the selected object(s) are to be added.

  

• To add a new class of objects listed in the Physical or Electrical view of the Constraint Manager, select them, then right-click the selection and choose the Classes » Add Selected to Class » New Class command from the context menu to open the Add Class dialog. Define the class Name (which must be unique and not empty) and the set of class members. The objects selected prior to accessing the dialog will be already in the Member list. If required, further configure the set of class members by moving object entries between Non-Members and Member lists using the arrow buttons.

  

• Alternatively, right-click in the grid area and select the Classes » Add Class command in the Clearances or Electrical view or a command from the (to add a net class) or the Classes » Add Class sub-menu to access the Add Class dialog. When accessing the dialog this way, the Member lists will initially be empty.

• To remove objects from a class to which they are currently added, select them, then right-click the selection and choose the Classes » Remove Selected from Class command from the context menu.

• To edit a class, right-click its entry and select the Classes » Edit Class command from the context menu to access the Edit Class dialog, where you can edit the name and members of the class.

•  

   

   

   

   

  To remove an existing class, right-click its entry and select the Classes » Remove Class command from the context menu.

Alternatively, you can use the Object Class Explorer dialog to add, edit, and remove classes. Right-click in the grid area and select the Classes » Class Explorer command from the context menu to open the dialog.

The folder-tree pane on the left side of the dialog lists supported object class types and existing object classes of each type.

• Click on the root Object Classes folder to access a summary listing in the main editing region of the dialog of all specific classes that have been defined across all object class types.
• Click on a child object class type folder to access a summary listing of all specific classes that have been defined for that type.
• Click on the entry for a specific class (or double-click on its entry in a summary list) to access controls for managing the object membership of that class.

To add a new user-defined class from the Object Class Explorer dialog, right-click within the category of class you want to create and choose Add Class from the context menu. To rename or delete a user-defined class, right-click its name and choose Rename Class or Delete Class, respectively.

Constraint Sets

To expedite the process of defining constraints for objects, the Constraint Manager provides the ability to save a set of constraints as a Constraint Set and then apply this Constraint Set to objects.

To save the set of constraints currently defined for an object as a Constraint Set, right-click a cell for this object and select the Save as Constraint Set command from the context menu. In the New Constraint Set pop-up, enter the desired name of the Constraint Set (which must be unique and not empty) and click Create.

A newly created Constraint Set will be applied to the object from which the Constraint Set has been created. To apply a Constraint Set to another object, right-click its cell and select the required Constraint Set from the Select Constraint Set sub-menu of the context menu. The cells to which a Constraint Set is applied are distinguished with a symbol in their top-left corner (e.g., ), and, in the Physical or Electrical views, the name of the applied Constraint Set will be reflected in the Constraint Set column.

To edit the values of an existing Constraint Set, select an object to which this Constraint Set is applied and click the  button. Change the constraint values as required and then click the Save button in the pop-up that appears to save the changes. The changes will be applied to all objects to which that Constraint Set is currently selected.

Currently defined Constraint Sets are listed in the Constraint Sets region of the Properties panel. Click the entry of a Constraint Set to show its constraint values. A Constraint Set selected in the Properties panel can be removed by clicking the  button at the bottom of the Constraint Sets region. Objects to which the removed Constraint Set has been selected will keep the constraint values applied by this Constraint Set before its removal.

Importing Directives from Schematics

You can import net and diff pair classes, differential pairs, and constraints from parameter set and differential pair design directives, placed and defined on your schematic source documents, into the Constraint Manager. To perform this,  click the  button when the Constraint Manager is accessed from the schematic side. The Refresh Constraint Manager dialog will display a summary of the import from the schematic to the Constraint Manager that will be completed by clicking the  button in the dialog.

Modifying Directives Imported from Read-only Documents

Directives that have been imported from read-only documents (for example, device sheets and managed sheets) cannot be modified if the Make Device Sheets In Projects Read-Only option is enabled (checked) on the Data Management - Device Sheets page of the Preferences dialog.

When the option is disabled (unchecked), the directives can be modified. After directives have been imported (with the option enabled), the rule is highlighted in blue in the Constraint Manager.

Importing and Exporting Constraints and Constraint Sets

You can import and export constraints and constraint sets between designs. To access, right-click in the Clearances, Physical or Electrical view of the Constraint Manager, then select Import or Export.

Importing Constraints and Constraint Sets

After selecting Import, the standard File Explorer dialog opens in which you can select the desired constraint/constraint set  (*.CstrDot ) to import into your design. The Constraints for Export dialog opens in which you can select the constraints/constraint sets to import into the currect design. The selected constraints/constraint sets will be applied to corresponding objects in the target design.

 

Exporting Constraints and Constraint Sets

After selecting one or more cells in the Clearances view or one or more lines in the Physical or Electrical view and then choosing Export, the Constraints to Import dialog opens with constraints and constraint sets for all objects that have been selected prior to choosing the command listed in the grid. Select the constraints/constraint sets you want to export using checkboxes (constraints related to the current view will be selected in the dialog by default). After clicking OK, the standard File Explorer dialog opens in which you can name and save the constraints/constraint sets. The file will be exported with the extension *.CstrDot  and can then be imported into another design.

Working with All Rules on the PCB Side

Cross-Probing

The Constraint Manager includes a cross-probe feature that will show the associated objects by visually highlighting them in the corresponding document. To cross probe to any object, right-click on its entry, then choose the Cross Probe option from the context menu or select Cross Probe from an advanced rule's  menu.

❯ ❮ Javascript ID: CM_CrossProbe_AD24_1

Set the Cross Probe View Settings in the Properties panel to configure cross-probing settings.

Use the schematic/PCB editor Clear Filter option (right-click in the design space and select Clear Filter, shortcut: Shift+C) to reset cross-probe highlighting.

Refer to the Cross-Probing & Selecting page to learn more about cross-probing in Altium Designer.

Cross Selecting

The cross selecting feature facilitates dynamic, bi-directional object selection. When cross select mode is enabled (using the Cross Select Mode command from the Tools main menu of the Constraint Manager, the schematic or PCB editor), objects selected in the Constraint Manager are also selected in the schematic and PCB documents, and vice versa.

Refer to the Cross-Probing & Selecting page to learn more about cross selecting in Altium Designer.

Transferring Constraints between Schematic and PCB

Changes applied in the Constraint Manager are transferred between the schematic and PCB designs using the Engineering Change Order (ECO) process. Select a command to update the constraints on the other side:

• To transfer changes from the schematic to the PCB – select the Design » Update PCB Document <PCBDocumentName> command from the main menus of the schematic editor.

• To transfer changes (made in the Clearances, Physical, and/or Electrical views of the Constraint Manager) from the PCB to the schematic – select the Design » Update Schematics in <PCBProjectName> command from the main menus of the PCB editor.

Use the subsequential Engineering Change Order dialog to explore, validate, and execute the changes.

Refer to the Keeping the Schematics & PCB Synchronized page to learn more.

Migrating from Design Rules to the Constraint Manager

If a PCB project uses the old rules management system (i.e., PCB Rules and Constraints Editor dialog), you can perform a one-time, one-way migration to the Constraint Manager.

Use the Design » Migrate Project to Constraint Manager Flow command from the main menus in the PCB and schematic editors. The Migration Required dialog opens to warn that the migration will take place and it cannot be undone after the  button is clicked.

Both PCB design rules and schematic directives will be transferred into applicable corresponding constraints within the Constraint Manager. Once the migration has successfully concluded, the Constraint Manager will be opened (in the context of which editor was active when you performed the migration).