F5.2 Fabrication layer requirements

The fabrication layers are used to display the simplified mechanical outline of components on the PCB.

KiCad refers to the fabrication layers as:

F.Fab - Front fabrication layer
B.Fab - Back fabrication layer

The following elements must be provided on the fabrication layer(s)

Simplified component outline must be provided on F.Fab layer
1. Outline uses line width between {0.10mm and 0.15mm} (recommended 0.10mm)
2. Outline should be simplified and not display complex features
3. For outlines based on the component body shape, the nominal size is used
Footprint polarisation / location of pin-1 is drawn
1. For IC packages, bevel is drawn at corner next to pin-1
2. Bevel should be 1mm or 25% of package size (whichever is smaller)
3. For connectors, a small arrow indicator drawn next to pin-1 should be used
Component value (footprint name) must be displayed on the F.Fab layer
1. Recommended text size = 1.0mm
2. Allowable text size = {0.5mm to 1.0mm}
3. Text thickness should be approximately 15% of text size ( with allowances for variation for aesthetic reasons)
4. Placed below (positive y direction) the part outline.
A second copy of the reference designator (RefDes) must be provided on the F.Fab layer. To add a second RefDes item, add a text object with the value ${REFERENCE}
1. RefDes must be centered on component body (inside component outline)
2. Orientation of RefDes should match major component axis
3. Size of text should be scaled to match component size
  1. It is recommended to scale it such that 4 characters fit without overlapping other features of the same layer.
  2. If it is not possible to fit at least 3 characters with the text size restrictions, then the reference should be moved outside (but scaled to smallest allowable text size)
4. Recommended text size = 1.00mm
5. Allowable text size = {0.5mm to 1.0mm}
6. Text thickness should be approximately 15% of text size (with allowances for variation for aesthetic reasons)

Edit on GitLab