Interrogating Violations

There are essentially three methods of interrogating design violations - from the Messages panel, from the PCB panel and directly within the design workspace. The first method is solely associated with having run a Batch DRC.

From the Messages Panel

After running a Batch DRC, double-clicking a violation message in the Messages panel will cross probe to the object(s) causing that violation in the main design window. Note : The Create Violations option must be enabled as part of the DRC Report options in the Design Rule Checker dialog, for the cross probing to work.

From the PCB Panel

When running an Online or Batch DRC, any rule violations associated with a rule class or individual rule will be listed in the Violations region of the PCB panel, when the panel is configured in Rules mode.Clicking on a violation entry will apply filtering using the offending object(s) as the scope of the filter. The resulting view in the main design window will depend on the highlighting options enabled ( Mask / Dim/ Normal , Select , Zoom ) at the top of the panel.Double-clicking on a violation entry (or right-clicking on an entry and choosing Properties from the subsequent menu) will open the Violation Details dialog, which provides information about the rule being violated and the primitive(s) responsible.From this dialog you can highlight the offending object (causing it to flash in the workspace) and jump to it, effectively providing zoom and center.
Each specific rule can be enabled or disabled with respect to Design Rule Checking - directly from the PCB panel - using the corresponding option under the On column. With this option disabled, the rule will not be included in the DRC and no violations of it will be listed.

Double-clicking on a violation entry will open the Violation Details dialog, which provides information about the rule being violated and the primitive(s) responsible.
From this dialog you can highlight the offending object (causing it to flash in the workspace) and jump to it, effectively providing zoom and center.

Directly in the Workspace

You can interrogate violations associated with a particular design object directly within the PCB workspace. Position the cursor over the offending object you wish to interrogate, right-click and selectViolations from the pop-up menu. In the example image, the offending track near the top-left corner (denoted by a yellow marker for ease of reference) is being investigated.
You can either choose to investigate individual violations associated with that object, or all violations. Choosing the former will cause the object(s) involved in the indicated violation to be zoomed and centered in the main design window. The zoom level can be adjusted by clicking the Zoom Level button in the PCB panel and using the slide control.Irrespective of your choice, the Violation Details dialog will appear, providing details about the particular design rule that is being violated and the offending object(s). If you chose to Show All Violations , each of the individual violations will be listed in the dialog, from which to choose.Highlight and jump to the object(s) causing the violation as required using the Highlight and Jump buttons respectively.

You can either choose to investigate individual violations associated with an object, or all violations. Choosing the former will cause the object(s) involved to be zoomed and centered in the main design window.
Irrespective of your choice, the Violation Details dialog will appear, providing further violation details and controls for highlighting and jumping to the offending object(s).

For further information on design rules, see Design Rules. This comprehensive reference includes information about each of the individual rule types and their associated constraints.