KiCad Rule Areas (Keepouts): Block Copper, Vias, and Parts

Keepouts in KiCad are rule areas

KiCad does not have a separate “keepout layer” you draw on. Instead you draw a rule area: a polygon on one or more copper layers with a list of things it forbids. The same polygon tool is used for keepouts and for areas that custom rules refer to by name.

Typical reasons to draw one:

• the area under and around a Wi-Fi or Bluetooth module antenna, where the module maker asks for no copper and no components;
• a mounting-hole or screw-head region where copper must not be touched by a washer;
• a slot or cutout area near the board edge;
• a region where an enclosure feature or connector body needs clearance;
• a zone where you do not want vias, for example under a pad that will be soldered with a thick stencil.

How to draw one

1. In the PCB editor choose Place, then Add Rule Area.
2. Click to draw the polygon and double-click to finish.
3. In the dialog, choose the layers it applies to (all copper layers for an antenna keepout, or just the layers you care about).
4. Tick what is not allowed: tracks, vias, pads, copper pours, and footprints are separate options. A copper-only keepout leaves parts alone, and a footprint keepout blocks placement without touching existing zones.
5. Optionally give the area a name, which lets custom rules refer to it.

Check the result by refilling zones and running DRC. A copper keepout should carve a hole out of ground pours on the layers you selected, and any track or via inside a forbidden region should produce a violation.

Refill after every change

Zone fills are cached. If you add or move a rule area and the pour does not change, refill all zones before you conclude the keepout did nothing. Many “keepout does not work” reports are a stale fill. It is also the reason to run DRC with refill enabled when you check a board for release.

Worked example: antenna keepout under a module

Modules with a PCB trace antenna publish a keepout in their hardware design guide: a rectangle at the antenna end of the module where no copper, no ground plane, and no components should exist on any layer, plus a requirement that the antenna overhang or sit at the board edge. The exact dimensions come from that module’s datasheet and are not the same across parts.

1. Place the module so the antenna end sits at the board edge or overhangs it, as the datasheet shows.
2. Draw a rule area over the datasheet’s keepout rectangle, extended slightly past the antenna on all sides.
3. Select all copper layers and forbid tracks, vias, pads, and copper pours; add footprints if parts nearby could intrude.
4. Refill zones and run DRC.
5. Look at the plotted layers in a viewer to confirm no copper survived in that region (Gerber viewer check).

ESP32 carriers are the common case; the basics of laying them out are in ESP32-C3 carrier board basics.

Rule area versus courtyard versus edge cuts

These three are often mixed up:

• Rule area: your explicit instruction to the DRC about where something is forbidden.
• Courtyard: the outline around a footprint that keeps other footprints a minimum distance away. See courtyard and keepout terms.
• Edge.Cuts: the board outline. Copper clearance to it is governed by the edge clearance rule, not by a rule area.

Mistakes to avoid

• Drawing the area on one layer when the restriction applies to all of them.
• Forgetting that a keepout stops zones but you may still have a pad or track route running through it from before. DRC will tell you.
• Using a keepout to hide a real clearance error. If you need a different spacing, set it with a rule so the reason is visible.
• Copying keepout dimensions from another board. Use the datasheet for the exact part and revision you are using.