Basic design rules are configured in the Constraints section of the Board Setup dialog. Constraints in this section apply to the entire board and should be set to the values recommended by your board manufacturer. Any minimum value set here is an absolute minimum and cannot be overridden with a more specific design rule. For example, if you need the copper clearance on part of a board to be 0.2mm and in the rest 0.3mm, you must enter 0.2mm for the minimum copper clearance in the Constraints section and use a net class or custom rule to set the larger 0.3mm clearance.

In addition to setting minimum clearances, a number of features can be configured here:

The pre-defined sizes section allows you to define the track and via dimensions you want to have available while routing tracks. Net classes can be used to define the default dimensions for tracks and vias in different nets (see below) but defining a list of sizes in this section will allow you to step through these sizes while routing. For example, you may want the default track width on a board to be 0.2 mm, but use 0.3 mm for some sections that carry more current, and 0.15 mm for some sections where space is limited. You can define each of these track widths in the Board Setup dialog and then switch between them when routing traces.

The teardrops section lets you set default parameters for various types of teardrops. There are different settings for teardrop connections to round objects, rectangular objects, and teardrop connections between tracks. The default teardrop parameters can be overridden when teardrops are added, and also changed in the properties for individual connected items. See the teardrops documentation for more information.

The length-tuning patterns section lets you set default parameters for each type of length-tuning pattern (single-track length, differential-pair length, and differential-pair skew). These defaults can be overridden in the properties of each tuning pattern added to the board. See the length tuning documentation for more information.

The Net Classes section allows you to configure routing and clearance rules for different classes of nets.

More than one net class can be assigned to a net. For nets with multiple net classes assigned, an effective aggregate net class is formed, taking any net class properties from the highest priority net class which has that property set. Net class priority is determined by the ordering in the Schematic or Board Setup dialogs. The Default net class is used as a fallback for any missing properties after all explicit net classes have been considered; this means that nets may be part of the Default net class even if they have other net classes explicitly assigned.

Net classes may be created and edited in either the Schematic or Board Setup dialogs.

The upper portion of the Net Classes section contains a table showing the net classes in the design and the design rules that apply to each net class. Every class has values for copper clearance, track width, via sizes, and differential pair sizes. These values will be used when creating tracks and vias unless a more specific rule overrides them (see Custom Rules below).

The track widths and via sizes defined for each net class are used when the track width and via size controls are set to "use netclass values" in the PCB editor. These widths and sizes are considered the default, or optimal, sizes for that net class. They are not minimum or maximum values. Manually changing the track width or via size to a different value from that defined in the Net Classes section will not result in a DRC violation. To restrict track width or via size to specific values, use Custom Rules.

Each net class can also have a color assigned to it. Depending on how net colors are configured in the appearance panel, net class colors can override the default color for ratsnest lines or copper objects. In addition to arbitrary colors for each net class, you can set all net classes to use the same color as configured for them in the schematic editor by clicking the Import colors from schematic button. To use a layer’s default color instead of overriding it with a custom net class color, set the net class color to transparent.

The lower portion of the Net Classes section lists pattern-based net class assignments. Working with pattern-based net class assignments is explained in the Schematic Editor documentation; pattern-based assignments can be edited in either the Board or Schematic Setup windows.

Note that pattern-based assignments can be created directly from the PCB editing canvas by right clicking a copper track or zone and clicking Assign netclass…​. Net classes can also be assigned in the schematic using net class directives or labels instead of pattern-based assignments.

The Custom Rules section contains a text editor for creating design rules using the custom rules language. Custom rules are used to create specific design rule checks that are not covered by the basic constraints or net class settings.

Custom rules will only be applied if there are no errors in the custom rules definitions. Use the Check Rule Syntax button to test the definitions and fix any problems before closing Board Setup.

See Custom Design Rules in the Advanced Topics chapter for more information on the custom rules language as well as example rules.

The Violation Severity section allows you to configure the severity of each type of design rule check. Each rule may be set to create an error marker, a warning marker, or no marker (ignored).

For descriptions of each violation type, and how to ignore individual violations without disabling all violations of that type, see the DRC documentation.