Design Rule Setup

The design rules describe manufacturing constraints, and help Kicad ensure that the design you create can be manufactured correctly.

Design Rules Editor

The manufactuing config dialogue box is found under File > Board Setup.

Most values provided below have conversions, but Kicad will automatically convert to your preferred units if you enter a unit indicator. EG, entering 0.01in, 0.254mm, or 10 mil will provide the same end result.

Board Stackup > Physical Layers

This page lets you indicate the PCB layer count, and physical properties of the PCB.

Copper Layers should be set to 2, 4, or 6. Using other layer counts will often result in issues in exporting files for production.

All other values: These depend on which service you need for production, and provided here: OSH Park Services. Entering these values is only required if your design will use Kicad’s DRC/DRU tools to calculate controlled impedence. During production, we will disregard user-provided values, and use the stackup indicated for the selected service.

Board Stackup > Soldermask/Paste

Solder Mask Expansion should usually be set to 2mil (0.0508mm), which pairs well with our production tolerances. This can be decreased as needed, but increasing this value is not recommended. For additional information, see Understanding Stop Mask Expansion.

Solder Mask Expansion Web Width should usually be set to 0.

Tent Vias is optional, but typically recommended. When checked, vias will be inaccessible for soldering; When unchecked, they will be exposed. Vias and through holes used for components will always be exposed as indicated in their footprint.

Solder Paste options will vary, and depend on your assembler or stencil manufacturer.

Design Rules > Constraints

These vary slightly based on production service.

Setting 2 Layer Services 4 Layer 6 Layer
Minimum Clearance 6mil (0.1524mm) 5mil (0.127mm) 5mil (0.127mm)
Minimum track Width 6mil (0.1524mm) 5mil (0.127mm) 5mil (0.127mm)
Minimum Connection Width 6mil (0.1524mm) 5mil (0.127mm) 5mil (0.127mm)
Minimum Annular Ring 5mil (0.127mm) 4mil (0.1016mm) 4mil (0.1016mm)
Minimum Via Diameter 20mil (0.508mm) 18mil (0.508mm) 16mil (0.4064mm)
Copper to hole clearance 5mil (0.127mm) 5mil (0.127mm) 5mil (0.127mm)
Minimum Through Hole 10mil (0.254mm) 10mil (0.254mm) 8mil (0.2032mm)
Hole to hole clearance 5mil (0.127mm) 5mil (0.127mm) 5mil (0.127mm)
Minimum uVia diameter 20mil (0.508 mm) 18mil (0.508 mm) 16mil (0.4064 mm)
minimum uVia Hole 10mil (0.254mm) 10mil (0.254mm) 8mil (0.2032mm)
Silkscreen Min Item Clearance user preference    
Silkscreen Min Text Height user preference    
Silkscreen Min Text Thickness 5 mil (0.127mm) 5 mil (0.127mm) 5 mil (0.127mm)

Design Rules > Net Classes

These can be configured to user preferences, and allow customized DRC depending on the type of signal you’re routing.

The “Default” net class will use the minimum DRC values.