Parent page: Specifying the Design Requirements
Altium Designer's PCB Editor uses the concept of Design Rules to define the requirements of a design. These rules collectively form an 'instruction set' for the PCB Editor to follow. They cover every aspect of the design - from routing widths, clearances, plane connection styles, routing via styles, and so on, and many of the rules can be monitored in real-time by the online Design Rule Checker (DRC).
Design rules target specific objects and are applied in a hierarchical fashion, for example, there is a clearance rule for the entire board, then perhaps a clearance rule for a class of nets, then perhaps another for one of the pads in a class. Using the rule priority and the scope, the PCB Editor can determine which rule applies to each object in the design.
With a well-defined set of design rules, you can successfully complete board designs with varying and often stringent design requirements. And as the PCB Editor is rules-driven, taking the time to set up the rules at the outset of the design will enable you to effectively get on with the job of designing, safe in the knowledge that the rules system is working hard to ensure that success.
The rules system built into Altium Designer's PCB Editor has several fundamental features that set it apart from most other design rule systems employed by other PCB editing environments:
Design rules are defined and managed from within the PCB Rules and Constraints Editor dialog. The dialog has two sections:
To add a new design rule from within the PCB Rules and Constraints Editor dialog, simply navigate to, and select the required rule type, within the left-hand tree, and either:
The new rule will be added to the folder-tree and will also appear in the summary list for that rule type.
To access the scope and constraint attributes for the rule, either click on the entry for the rule in the folder-tree pane, or double-click on its entry in a summary list. The main editing window of the dialog will change to give access to the controls for defining the scope and constraint attributes for that rule.
To fully define the new rule, the designer should:
A new rule can also be created using the Design Rule Wizard. Access is made directly using the Design » Rule Wizard command, or by clicking the Rule Wizard button, at the bottom of the PCB Rules and Constraints Editor dialog.
Use the pages of the Wizard to create a new design rule. Steps involve:
To quickly create an identical copy of an existing rule, use the duplicate feature. This feature can be accessed in two ways:
The duplicate rule will be named the same as the original, with the addition of a suffix (e.g. _1) to distinguish it. It's definition (scope, constraints, etc) will be identical to that of the original. In terms of priority, it will be given the next priority below that of the original rule. So, for example, if the original rule has priority 1, the duplicate will be given priority 2.
Main page: Scoping Design Rules
For the PCB rules system to know what objects a given rule applies to, it needs to know the scope of that rule - the extent of its application. Scoping, or targeting the rule, is performed in the PCB Rules and Constraints Editor dialog.
Rather than being restricted to a predefined list of possible target options, each design rule is scoped by writing what is called a Query. A query is essentially an instruction to the software that defines the set of design objects to be targeted. Queries are written using query keywords. In the same way that a query can be written in a Filter panel to find a specific set of objects, so to a query is written to define the objects that each rule targets. An example might be:
InNet('VBAT') And OnLayer('Bottom Layer')
If this query were to be used as the scope for a Width rule, whenever you route the VBAT net and switched to the bottom layer, the track width would automatically change to the width specified as part of that rule's constraints. Also, upon running a design rule check, any VBAT net routing on the bottom layer would have to have the specified width, or it would be flagged as a violation.
Simple scoping options are provided that allow you to quickly generate scope queries targeting:
Simply select one of the options and, if required, use the applicable drop-down list(s) to select the appropriate target, such as a Net or Layer. The query string (logical query expression) will appear in the Full Query region to the right.
The Advanced (Query) option enables you to write your own, maybe more complex, but also more specific query. You can type your own specific query for the rule scope directly into the Full Query region. Alternatively, two features are available to help in the creation of logical query expressions - the Query Builder and the Query Helper. These can be very useful when unsure of the syntax of a query, or the possible keywords available for use.
To simplify the process of defining and managing rules, the idea is to define general rules that cover broad requirements and then override these with specific rules in specific situations. For this to be possible, you need to be able to prioritize the rules, to indicate which one to use when an object is targeted by multiple rules of the same type.
For example, to specify the most commonly used routing width on the board, you define a single rule that applies to every net on the board. This rule can then be overridden for a specific net (or a class of nets for that matter) by adding another rule of the same type, but with a higher priority.
Another example could be the solder mask requirements - here you would define one mask rule that targeted every pad and via on the board, which could then be overridden for the pads in a specific footprint-kind. This footprint-specific rule could further be overridden for a specific pad in that footprint, if required.
An important aspect of managing the rules is ensuring that all the priorities are set appropriately. When a new rule is created, it defaults to the highest priority. Use the Priorities button at the bottom of the PCB Rules and Constraints Editor dialog to configure the priorities in the Edit Rule Priorities dialog.
Initially, the dialog will list all rule instances for the rule type that is currently selected in the PCB Rules and Constraints Editor dialog. Use the Rule Type field to change the rule type and hence list the specific rules defined for that type. The defined rules are listed in order of current priority - from 1 (highest priority) downwards. Select a rule entry and use the Increase Priority and Decrease Priority buttons to move it up or down in the priority order respectively.
Rules, of course, can be modified at any time. Indeed, to arrive at the final working set of rules often involves a few key refinements here and there. Typically this involves the scoping, to ensure the target design objects are being 'picked up' by the respective rule(s) as required. Simply select an existing rule in the PCB Rules and Constraints Editor dialog and make changes as necessary to its scoping and constraint attributes.
Changes made to existing rule definitions are highlighted in both the folder-tree pane and the applicable summary lists. Such entries are distinguished by the rule name becoming bold and an asterisk displayed to the right of the name. The asterisk is used to reflect that the rule is an existing rule that has been modified, rather than a newly created rule (which is displayed bold without an asterisk).
If a rule is detected as being invalid by the system - for example it has an issue with its scoping query expression, or a value for a constraint that is not allowed - it will be flagged as being invalid. Such a rule will be highlighted in red - within the PCB Rules and Constraints Editor dialog - both in the left-hand rule tree, and any summary view (rule category, or rule type) in which the rule appears. A warning message will also appear should you attempt to close the dialog.
In the rules-driven environment of Altium Designer's PCB Editor, it is not uncommon to build up a rather impressive and comprehensive array of rules with which to successfully constrain your boards. For whatever reason along the way, you may wish to disable some rules - perhaps they are not applicable to the board in question, or perhaps they need to be temporarily disabled to ease the load on the Design Rule Checker (and speeding its performance as a result!). Disabling is a good way of keeping such rules, just in case they are needed again in the future.
To disable a rule, simply toggle the corresponding Enable option for that rule in one of the relevant summary lists, on the right-hand side of the PCB Rules and Constraints Editor dialog. A disabled rule will also appear with a 'greyed-out' appearance.
To delete a single design rule from within the PCB Rules and Constraints Editor dialog:
The rule name will appear bold with strike-through highlighting to distinguish it as being a deletion that is yet to be 'applied'.
Many rule types have default rules created when a new PCB document is created. In a similar fashion, if all specific rules for one of those rule types are deleted, the default rule will be re-added automatically the next time the PCB Rules and Constraints Editor dialog is accessed. Alternatively, default rules can be created again by clicking the Create Default Rules button, at the bottom of the dialog.
Depending on the board design, a fair number of design rules may need to be defined, with scopes that range from the very simple, to the very complex. It is a good idea to check that the rules defined do indeed target their intended objects. Care at the rule definition stage can save wasted time and effort tracing violations caused through incorrect rule scoping.
There are essentially two methods for verifying rule scopes - either by selecting design objects and interrogating the rules that currently apply to them, or by taking a rule and observing which objects fall under its scope.
For any placed object in the current design, you can quickly access information about which unary design rules apply to that object. Simply position the cursor over the object, right-click, and select Applicable Unary Rules. All defined design rules that could be applied to the selected object are analyzed and listed in the Applicable Rules dialog.
Each rule listed in the dialog will have either a tick () or a cross () next to it. A tick indicates the rule with the highest priority out of all applicable rules of the same type - this is the rule currently applied. Lower priority rules of the same type are listed with a cross next to them, indicating that they are applicable but, as they are not the highest priority rule, they are not currently applied.
In a similar fashion, you can also access information about the binary design rules that apply between two placed objects in a design. Simply position the cursor over any object, right-click and select Applicable Binary Rules. Follow the prompts to select two objects in the design. The Applicable Rules dialog will then appear, displaying all binary design rules that apply between those objects.
If, rather than seeing which rules apply to an object (or between two objects) you would prefer to pick a rule and see which objects that rule applies to, this can be achieved from the PCB Rules And Violations panel. The panel lists all currently defined rules for the design. All rules can be viewed, or you can browse specifically by rule type - provided at least one rule of any given type has been defined for the active design. As you click on a specific rule in the Rules region of the panel, filtering will be applied, using the rule as the scope of the filter. Only those design objects that fall under the scope of the rule will be filtered. By employing the Mask (or Dim) highlighting feature, you can quickly see the resulting objects targeted by the rule.
Design rules can be exported from, and imported to, the PCB Rules and Constraints Editor dialog. This allows you to save and load favorite rule definitions between different designs.
In both cases, you can choose which types of design rules to export/import.
A report of currently defined design rules can be generated from within the PCB Rules and Constraints Editor dialog. The report can cater for all rule categories, a specific rule category, or a specific rule type. A report can be generated by:
The Report Preview dialog will appear, with the appropriate report already loaded. Use this dialog to inspect the report using various page/zoom controls, before ultimately exporting it to file, or printing it.
Design constraints (rules) can be defined prior to PCB layout, by adding parameters that are configured as design rule directives to the schematic source document(s). The scope of the corresponding PCB design rule, created when the design is transferred to the PCB document, is determined by the nature of the object to which the parameter (added as a rule) is assigned. The following table summarizes the schematic parameter-to-PCB rule scope options that are supported.
|Add a Parameter (as a rule) to a...||From...||For a PCB Rule Scope of...|
|Pin||the Parameters tab of the Pin Properties dialog.||Pad|
|Port||the Parameters tab of the Port Properties dialog.||Net|
|Wire||the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the wire using the Place » Directives » PCB Layout command.||Net|
|Bus||the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the bus using the Place » Directives » PCB Layout command.||Net Class|
|Harness||the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the harness using the Place » Directives » PCB Layout command.||Net Class|
|Blanket||the Parameters dialog, after placing a PCB Layout Directive (Parameter Set object) on the edge of the blanket using the Place » Directives » PCB Layout command. Include a ClassName parameter to create a net class for all nets covered by the blanket, which will then be used for the rule scope.||Net Class|
|Component||the Parameters region of the Properties for Schematic Component dialog.||Component|
|Sheet Symbol||the Parameters tab of the Sheet Symbol dialog.||Component Class|
|Device Sheet Symbol||the Parameters tab of the Sheet Symbol dialog.||Component Class|
|Managed Sheet Symbol||the Parameters region of the Properties for Managed Sheet Instance dialog.||Component Class|
|Sheet||the Parameters tab of the Document Options dialog (Design » Document Options).||All Objects|
In each case, the method of adding a rule-based parameter is the same. From the respective tab or dialog, simply perform the following:
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.