PCB Design Rules

AISLER’s Design Rule Rating of your PCB

Last Updated: 13.09.2023

We classify your PCB as “Simple” or “Complex”, depending on the complexity of your design. Take a look at the table below to see which features make a board complex or simple. A board is classified as complex as soon as it has at least one complex feature. Each class is compatible with specific products that can be selected and ordered at the end of the ordering process. Please make sure to select Beautiful Boards HD (Surface Finish: ENIG) if your copper design includes complex line widths and/or spacings.

feature Simple Complex
min. drill diameter ≥ 0.3 mm ≥ 0.1 mm
no. of layers 2 4, 6
contains castellated holes :heavy_multiplication_x: :heavy_check_mark:
min. trace width/spacing 200 µm/150 µm 125 µm/125 µm

Design Rule Files

We provide preconfigured design rule files for Eagle, KiCad and DipTrace on Github .


The following design rules should be respected if you want to manufacture yor PCBs with us.

All listed values are minimum values.

Symbol Description Simple Complex
a min. trace width 200 μm 125 μm
b min. trace spacing 150 μm 125 μm
c min. trace pitch 350 μm 250 μm
d min. spacing trace / trace 150 μm 125 μm
e min. spacing trace / via-pad 150 μm 125 μm
f min. spacing trace / copper fill 150 μm 150 μm
g min. spacing trace / SMD-pad 150 μm 125 μm
h min. spacing via-pad / via-pad 150 μm 125 μm
i min. spacing via-pad / copper fill 150 μm 150 μm
j min. spacing via-pad / SMD-pad 150 μm 125 μm
k min. spacing copper fill / copper fill 200 μm 200 μm
l min. spacing PCB edge / trace 300 μm 300 μm
m min. spacing PCB edge / pad 300 μm 300 μm
n min. spacing PCB edge / copper fill 300 μm 300 μm
o min. spacing NPTH / SMD-pad 250 μm 250 μm
p min. spacing NPTH / via-pad 250 μm 250 μm
q min. spacing NPTH / trace 250 μm 250 μm
r min. spacing NPTH / copper fill 250 μm 250 μm
s min. annular ring 200 μm 200 μm
t min. drill distance NPTH/NPTH 300 μm 300 μm
u min. drill distance PTH/PTH 300 μm 300 μm
v min. drill distance NPTH/PTH 300 μm 300 μm
w min. spacing SMD-pad / SMD-pad 150 μm 125 μm
x min. diameter SMD-pad 200 μm 125 μm

Please note:

  • The Copper clearance values reference the base copper structure covered by soldermask. It is necessary to include a soldermask dam in between Pads to prevent bridging when using HASL as surface finish.

  • Burried, blind, micro or tented vias are not supported

  • User defined subpanels are not allowed, see also here

  • Soldermask openings should have the size of the underlying pad, as the openings are automatically enlarged by us.

  • The Stencil openings should be as large as the pad, they will be automatically adjusted by us.

Our design rules define the minimum manufacture capabilities for the standard PCB Pools. Passing the DRC check is a good start, but, does not guarantee a working design.