Inspecting a board

Measurement tool

The measurement tool allows you to make distance and angle measurements between points on the PCB. To activate the tool, click the icon in the right toolbar, or use the hotkey Ctrl+Shift+M. Once the tool is active, click once to set the measurement start point, then click again to finish a measurement.

Design rule checking

The design rule checker is used to verify that the PCB meets all the requirements established in the Board Setup dialog and that all pads are connected according to the netlist or schematic. KiCad can automatically prevent some design rule violations while routing tracks, but many others cannot be prevented automatically. This means it is important to use the design rule checker before creating manufacturing files for a PCB.

To use the design rule checker, click the icon in the top toolbar, or select Design Rules Checker from the Inspect menu.

The top section of the DRC Control window contains some options that control the design rule checker:

Refill all zones before performing DRC: when enabled, zones will be refilled every time the design rule checker is run. Disabling this option may result in incorrect DRC results if zones have not been refilled manually.

Report all errors for each track: when enabled, all clearance errors will be reported for each track segment. When disabled, only the first error will be reported. Enabling this option will result in the design rule checker running more slowly.

Test for parity between PCB and schematic: when enabled, the design rule checker will test for differences between the schematic and PCB in addition to testing the PCB design rules. This option has no effect when running the PCB editor in standalone mode.

After running DRC, any violations will be shown in the center part of the DRC Control window. Rule violations, unconnected items, and differences between the schematic and the PCB are shown in three different tabs. The controls below the list of violations can be used to show or hide violations depending on their severity. A report file in plain text format can be created after running DRC using the Save button.

Each violation involves one or more object on the PCB. In the list of violations, the objects involved are listed below the violation. Clicking on the violation in the list view will move the PCB Editor view so that the affected area is centered. Clicking on one of the objects involved in a violation will highlight the object.

Right-clicking a violation in the list view will open a context menu with additional actions including excluding the selected violation. Excluded violations are hidden unless the Exclusions checkbox is enabled at the bottom of the DRC Control window. Excluded violations are remembered between runs of the design rule checker.

Clearance and constraint resolution

The clearance and constraint resolution tools allow you to inspect which clearance and design constraint rules apply to selected items. These tools can help when designing PCBs with complex design rules where it is not always clear which rules apply to an object.

To inspect the clearance rules that apply between two objects, select both objects and choose Clearance Resolution from the Inspect menu. The Clearance Report dialog will show the clearance required between the objects on each copper layer, as well as the design rules that resulted in that clearance.

To inspect the design constraints that apply to an object, select it and choose Consraints Resolution from the Inspect menu. The Constraints Report dialog will show any constraints that apply to the object.

3D viewer

Net inspector

The Net Inspector allows you to view statistics about all the nets in a board. To open the inspector, click the icon at the top of the Nets section of the Appearance panel, or select Net Inspector from the Inspect menu.

Clicking a net in the list will highlight that net on the board. Clicking a column title allows you to sort the list of nets by that column.

The Group By field allows you to combine different nets together and view the total length of the combined nets. For example, if you have two nets named DATA0 and DATA0_EXT, using a Group By value of DATA0* will create a group containing both nets. More complicated groupings can be created by changing the Group By mode from Wildcard to RegEx (regular expressions). The substring (Substr) variants of the Group By mode will create groups for each set of nets that matches the pattern differently.

For example, if you have the nets U1D+, U1D-, U2D+, and U2D-, the grouping pattern U*D will match all four nets in Wildcard mode, creating a single group U*D. In Wildcard Substr mode, it will match all four nets, but create two different groups: U1D and U2D.

Pad Count and Via Count show the number of pads (surface mount and through hole) and vias on a net. Via Length shows the total height of each via (not accounting for which copper layers the via connects to). In other words, Via Length is equal to Via Count multipled by the stackup height of the board. Track Length shows the total length of all track segments in a net, not accounting for topology. Die length shows the total of all Pad to Die Length values set for pads on the net.