Altium Designer Documentation

New Design Rules Editor

Modified by Susan Riege on Feb 2, 2021
All Contents
NOTE: This page is a work in progress and will continue to be updated.

This Altium Designer release offers a new alternative approach for viewing, creating and managing the design constraint rules used for your PCB layouts. Provided as a document-based user interface, the new Design Rules Editor coexists with the existing Rules and Constraints Editor, but takes a design-orientated rather than purely rule-orientated approach to PCB design constraints.

Some of the notable advantages of this new approach are:

  • Using a document-based presentation interface rather than a modal dialog means that the PCB Editor and its associated functions remain active and accessible. This is a similar approach to the application of a Bill of Materials (BoM) or Layer Stack Manager (LSM) document along with its associated Properties panel mode.
  • A shift from query-based rule scoping to an applied object type matching simplifies constraint rule creation.
  • Rule priority is automatic, based on the natural hierarchy of design objects.
  • Interactive rule validation checking for detecting common syntax, assignment and scoping errors.
  • The design constraint rules are available to both the Rules and Constraints Editor and the new document-based Rules Editor. Rules created in the new system are backward compatible with the old system.

New Rules Editor Interface

To access the new Rules Editor document interface, open the existing Rules and Constraints Editor dialog (Design » Rules) and then click the dialog's Switch to Document View button (on the left in the lower margin).

The new Rules Editor is opened as an interactive Rules document that is arranged into six selectable rule sections of increasing priority – Nets, Diff Pairs , xSignals, Polygons, Components and Advanced. In this arrangement the first five sections (Nets to Components) represent a design object view of the rules, while the Advanced view section applies to more complex rules (typically using queries) that cannot be expressed as the simpler design object -orientated rules. Click the Switch to Dialog View button to return to the Rules and Constraints Editor dialog view.

Constraint Rule Types

In the new Rules Editor, existing rules that feature more complex query expressions in their matching scope are considered as Advanced Rules (or Custom Rules) while other simpler rules are re-expressed as the object-type Basic Rules – rules based on the type of design objects being checked. See below for an overview of the design-orientated object (Basic) rules.

Most rules in the Advanced (query-based) format can be converted to the simpler Basic rules by dragging and dropping the rule on to the Basic Rules listing, or by selecting the Move Custom Rule to Basic option from the advanced rule's right-click menu options. When converted, the advanced rule's query-based scope will be interpreted to the basic rule's object type qualification.

Rule Priorities

In general, the priority of Rules is dealt with automatically by the system. This is indicated by the arrangement of the rules view buttons in the interface, which are positioned by rule priority from left to right – Nets having the lowest priority.

  • Advanced (or Custom Created) rules take precedence over the sequence of Basic object rules, and can be manually reordered within the Advanced view by dragging their entries up or down.
  • Conversely, Basic rules are automatically prioritized by the system based on the design object type, as indicated by the object sections (Nets to Components) in the document interface.
  • Within each of the (Basic) object rule sections the priority is ordered from All (lowest) to Object Class to Object (highest), and by inference, rules with an All scope that have been converted to Basic rules will have the lowest priority.
  • To set an explicit priority for a Basic rule, right-click on the rule and select the Move Basic Rule to Advanced option, and then manually set its priority position in the Advanced view. This applies to rules other than those with an All scope -- for example in the Nets view, a rule with a Net Class or Net scope specified can be converted (moved) to be an Advanced rule.

New Custom Constraint Rule

Creating a new Rule in the manager's default Advanced mode (as indicated and selected by the button) is similar to constructing a Rule in the existing Rules and Constraints Editor. To do so, select Add Custom Rule from the view's right-click context menu (or the lower button), add a query-based matching scope if required (), and enter the constraint parameters in the column grid or the lower graphical representation.

To simplify the repeated process of creating advanced/custom type rules, the Rules Editor allows you to store query-based object matching scopes in a Scopes Library (via the menu). The library is presented through the Properties panel, where custom scopes can be imported, managed and exported for reuse in other custom constraint rules. The use of a library-based scope in a rule is indicated by an icon in the rule's Object Match column entry.

  • Once a library-based scope has been applied to a rule, you can use the Object Match (scope) field's menu to remove the scope entry (Clear Scope) or revert the scope back to its query-based format (Detach Scope).
  • Also note that the Scopes Library itself may be exported as a custom scope XML file, which can then be used to populate the Scope Library of another Altium Designer installation.
  • Drag and drop a rule to a different position in the listing to change its priority. Custom Rules adopt the highest priority. Note that the priority order of Basic (object) rule entries is automatically determined by their inherent hierarchy – see above for more information.
  • Select File » Save to PCB to save the constraints document file to the PCB project.

Scope Cross Probe

The new Rules Editor includes a cross-probe feature that will show a constraint rule's object scope by visually highlighting the net and connections in the corresponding PCB layout. To cross probe to any rule in the manager's grid listing, right click on its entry and choose the Cross Probe option from the context menu, or select the Cross Probe option from an advanced rule's menu.

Set the Cross Probe View Settings – the Zoom and Select options – in the Properties panel, and use the PCB editor Clear Filter option to reset cross probe highlighting.

Design Object Constraint Modes

To take a simpler design-object orientation approach to constraint rule creation, select a suitable object mode button at the top of the rules grid to change from the default Advanced mode. Conceptually, these modes present a more integrated rule interface that focuses on constraining (limiting) how design objects can be applied, rather than the creation of breakable design rules. The positional sequence of the design object buttons relates to increasing object complexity (and rule priority), from basic Nets (and classes) to unified Components and on to the Advanced mode.

When in Advanced mode (), the rules are grouped by type, such as the basic Via and Width constraint rules shown in the below image(s). Further rule specificity would be created by adding a further rule and/or including a query language element.

Conversely, the object-orientated views (Nets to Components) organize the rules by design objects (eg: Nets) or classes (eg: Net Class), and as a result provide a direct overview of how the rules apply to the design. To see an overview of rules that apply to an object type, select an object or class in the left column to see all associated rules, or select All to see all rules associated with the object type. The below example shows the overview of rules associated with Nets ().

When using the design object orientated approach say with the Nets object type selected as shown below, the basic Via and Width rules are integrated in one composite entry. The grid layout also offers provision for more constraints to be added by (Net) object and class.

Adding further, more specific constraints in this example requires only that a Net or Net Class is selected, and then suitable values entered in the grid cells that correspond to the desired type of constraint rule. As shown below, a larger Via size has been permitted for Power nets (defined by its class), and an increased maximum track width is assigned to the 5V supply rail net. In effect, four rules are encompassed in the one simple grid view – a width constraint for the 5V net, a width constraint for all other nets, a Via size constraint for the Power nets, and a Via size constraint for all other net classes.

Use the button to add a variation of the currently selected constraint rule, such as in the example shown below, where an additional 5V net rule sets a preferred width for the Bottom layer.

Note that the availability of rule types within the grid entries is set by the available columns, which is in turn specified by those enabled in the Properties panel Rule Visibility listing. For example, enabling the Clearance entry in the Rule Visibility list will add the Clearance column to the Nets object type, as shown below. Adding an applicable clearance rule then involves just entering a net or class scope and suitable distance parameters.

Rule Validation

The validity of all active rules can be checked in the Rules/Constraints Checks section of the Properties panel by clicking the section's button. This action detects rules for likely errors such as duplicated rules, rules of the same scope with different values, rules with overlapping class members (such as nets), and rules with unresolved scopes. Each violation type entry can be expanded to show its violating rule(s), which when selected will open the specific rule entry.

Rule Violations

Enabled design constraint rules are applied to the current board design through a range of mechanisms, such as live Online Design Rule Checking, the batch Design Rule Checker or selectively run from the PCB Rules and Violations panel. Violations of those constraint Rules – where the specified and scoped limits are exceeded – are indicated through board graphics, panel entries and reports, and also by alert icons in the Rules Editor itself. And as a bonus, violations can be inspected, analyzed and corrected while the Rules Editor is open, thanks to its design document (rather than dialog) format.

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

联系我们

联系原厂或当地办公室

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
You are reporting an issue with the following selected text
and/or image within the active document:
Altium Designer 免费试用
Altium Designer Free Trial
我们开始吧!首先,您或者您的公司已经在使用Altium Designer了吗?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

既然您在使用Altium Designer,为何仍需要试用?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,实际上您无需下载一个试用版本。

点击下方按钮下载最新版本的Altium Designer安装包

下载Altium Designer 安装包

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

填写下方表格,获取Altium Designer最新报价。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

如果您是Altium维保期内客户,您不需要下载试用版本。

如果您不是Altium维保客户,请填写下方表格免费试用。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

您为何想要试用Altium Designer?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

那您来对地方了!请填写下方表格申请试用吧。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好棒!创作是一件超酷的事情,我们可以为您提供完美的设计软件。

Upverter是一个社区导向的交流平台,专为您这样的创客量身定做。

点击这里看看吧!

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。