Design Rule Wizard

Now reading version 17.1. For the latest, read: Design Rule Wizard for version 21

The front page of the Design Rule Wizard.
The front page of the Design Rule Wizard.


The Design Rule Wizard allows you to manually create, from scratch, new rules for the PCB.


The Design Rule Wizard can be opened from the PCB Editor by going to the main menu and selecting Design » Rule Wizard or by clicking the Rule Wizard button, to the lower-left of the PCB Rules and Constraints Editor dialog.


Choose the Rule Type

From the front page of the wizard, click the Next button to move to this page. The Choose the Rule Type page of the Design Rule Wizard allows designers to easily select the kind of rule they wish to create and give it a name and description. Rule type categories can easily be expanded or collapsed using the buttons.

When a design rule type has been chosen and given a name and description, click Next to continue.

Choose the Rule Scope

The third page of the Design Rule Wizard lets designers set the scope of the design rule to be created. Options include: Whole Board, 1 Net, A Few Nets, A Net on a Particular Layer, A Net on a Particular Component, and Advanced (Start With a Blank Query). The option chosen will determine how the next page of the wizard is presented. If the Whole Board board option is selected, the wizard will proceed directly to the Choose Rule Priority page. However, for all other options the wizard will first proceed to the Advanced Rule Scope page, which allows designers to refine the details of the objects the new rule will apply to.

When an object(s) has been chosen for the rule to apply to, click Next.

Advanced Rule Scope

If you chose the Whole Board option on the last page, this section doesn't apply and you can proceed to the next page, Choose Rule Priority. For all other options, the Advanced Rule Scope uses the Query Builder to refine details of the objects that the new rule will apply to.

The Query Builder will be structured to match the option chosen for the Rule Scope, with the exception of the Advanced option, which allows designers to build a query from scratch. The above screenshot is how the query will appear when the A Net on a Particular Layer option is selected for Rule Scope. To change a condition type/operator or value, simple click in the field. Designers can type the desired condition into the field, or select one from the dropdown.

When building a query from scratch, the query builder allows designers to create a query for targeting specific objects in the design document, by simple construction of a string of ANDed and/or ORed conditions.

The left-hand section of the query builder is where you specify the condition(s) that you require to target the set of objects needed. Initially the entry in the Condition Type/Operator column will be Add first condition. Clicking once on this entry will reveal a drop-down list of condition types. The condition types listed will only reflect those relevant to a board design.

Select the condition and click in the Condition Value column to access a drop-down list of possible values for that condition type. As you define a condition in the left-hand section of the query builder, a preview of the currently built query is shown in the right-hand section.

Continue to add further conditions to narrow down your target set of design objects as required. Conditions can be ANDed or ORed together. The default logical operator is AND, which is automatically inserted when you add another condition.

To change the logical operator between conditions, click on the AND or OR entry in the Condition Type/Operator column and select the required operator. The preview of the query will update accordingly.

Specifying Precedence

The  and  buttons at the top of the query builder allow you to essentially add and remove brackets around the presently selected condition (increasing and decreasing indent). This allows you to create precedence for certain logically ANDed or logically ORed conditions.

For example, consider the following built query:
InNet('GND') AND (OnLayer('Top Layer')

The first condition has been set to the condition type Belongs to Net, with value GND. Another condition has then been added, using the condition type Exists on Layer, with the value Top Layer.

Note that the outermost bracket pairing is added automatically by the Builder, and is not displayed while building the query expression.

At this stage, with the second condition selected in the dialog, the right arrow button has been clicked. Brackets have been automatically added around the second condition, and now the possibility to add a condition within that pair of brackets is available.

The third condition with condition type Object Kind is and value Track is then added within the brackets.

Use the Show Level drop-down at the top-left of the dialog to control the visual display of levels in your structured string of conditions. This essentially expands/collapses the display of brackets. Adding brackets effectively creates a new level. You can display levels 1-5, but for any further levels added use the Show All Levels option.

Alternatively, click on the expand or contract symbols (associated with a bracketed condition) to show the next level(s) or hide the current level (and all levels below) respectively. The  and  buttons at the top of the dialog can also be used to expand or collapse the currently selected condition.

Use the  and  buttons at the top of the query builder to move a selected condition in the query string being built. For a condition that has sub-levels (i.e. a bracketed condition), any condition in the level structure can be moved. When levels are expanded, a condition can be moved down or up through the levels. When levels are collapsed, a condition will be moved over the level structure.

To delete a condition, select it and either click the  button at the top of the dialog, or use the Delete key.

When the expression for the query has been defined as required, clicking OK will load the central region of the PCB Filter panel with the query, ready to apply the filter.

Additional buttons in this region of the panel provide access to previously used and favorite (stored) queries, as well as the ability to create design rules. The following drop-down sections look at these features in more detail.

When your desired query has been built, click Next to continue.

Choose the Rule Priority

Define the priority of the new rule. Use the Increase Priority and Decrease Priority buttons to move a rule up or down in the order. Where the rule stands in the priority is listed under the Priority column, with 1 being the highest priority.

This page of the wizard also allows designers to view the Name, Scope, and Attributes of the current rules on the PCB. As well, designers can see whether or not a rule is enabled. However, these categories for existing rules cannot be edited from the wizard. The new rule can be edited by clicking the Back button and returning to previous pages where those categories were determined.

When the priority order is as desired, click Next.

The New Rule is Complete

The final page of the Design Rule Wizard confirms that your new rule has been completed correctly. In the main area of the wizard, designers can view given information about the new rule that is being created. Additionally, you can elect to launch the main design rules dialog (the PCB Rules and Constraints Editor) after exiting the wizard. This option is enabled by default, but can be disabled by clicking the checkbox next to the option. The PCB Rules and Constraints Editor dialog allows designers to browse and manage the defined design rules for the current PCB document.

If any information is incorrect, click the Back button to return to previous pages and correct the misinformation. Otherwise, click Finish to exit the wizard and launch the PCB Rules and Constraints Editor (unless the design rules dialog option has been disabled).

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

The features available depend on your Altium product access level. If you don’t see a discussed feature in your software, contact Altium Sales to find out more.