Parent page: PCB Objects
A violation object marks where one or more design objects are violating a design rule. Violation objects are also known as DRC (Design Rule Check) Error Markers. They are added to the design when a violation is detected by the online, or batch, Design Rule Check (DRC) feature.
Violation objects are automatically placed by the Design Rule Check feature; they are not objects that are placed or edited by the designer. When either the online DRC is running or the batch DRC is run, each design object that violates a design rule is marked by a violation object. The rules that are currently being checked are configured in the Design Rule Checker dialog. The dialog is accessed by using the Tools » Design Rule Check command from the main menus. Use it to configure which rules are to be online and/or batch checked.
There are two types of violation objects: DRC Error Markers and DRC Detail Markers.
The images below show how the two types of markers work together. The first image is zoomed out; the second image is zoomed in on the same violations. The first image shows clearance violations marked by a DRC Error Marker (in red); the right image shows both the red Error Marker and also the white Detail Marker, indicating that the clearance is less than the 6mil specified in the applicable Electrical Clearance design rule.
The presentation of the violation objects can be configured in the following ways.
The color of both types of markers is configured on the Layers & Colors tab of the View Configuration panel in the System Colors region.
The presentation behavior of these markers can be configured on the PCB Editor — DRC Violations Display page of the Preferences dialog. There are two aspects that can be configured (refer to the image below):
The enabled design rules determine which rules are checked and when they are checked (online and/or batch). How detected violations are then marked is determined by the Choose DRC Violations Display Style settings on the PCB Editor — DRC Violations Display page of the Preferences dialog.
As the designer, you can configure the display to show just the Violation Details (Detail Markers), or to show a Violation Overlay (Error Markers), or both. Enable the checkboxes as required, or right-click in the dialog to toggle multiple options on or off.
There are a number of ways violation information is displayed within the software. The violation markers (both Overlay and Detail) provide strong clues to the location and nature of the violation. For example, in the image below the via on the left has a detail marker that shows the diameter of the via is less than 1mm, so it must be smaller than the size allowed in the applicable Routing Via Style design rule. There is also a line drawn from the via to a pad that is nearby; this line is broken by a double-slash. This indicates that the net is un-routed (broken) between the via and pad. Use the detail markers to help interpret the error condition.
As well as the markers, all detected violations are detailed in the PCB Rules And Violations panel. The image below shows a section of the panel with the Clearance Constraint selected.
Click once on a violation to zoom to that violation in the design space; double-click on it to open the Violation Details dialog, which details both the Violated Rule and the Violating Primitives.
Violation objects can be removed by running the Reset Error Markers command (Tools » Reset Error Markers). Note that this simply removes the error markers; the underlying design rule violations must still be analyzed and resolved.
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.