PCB Design Rules

AISLER’s Design Rule Rating of your PCB

Our goal is to provide the optimal product for you. That’s why 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 ≥ 0.2 mm
no. of layers 2 4
smallest necessary milling tool for cutouts 2.4 mm 1.6 mm
contains plated slots :heavy_multiplication_x: :heavy_check_mark:
min. trace width/spacing 200 µm/150 µm 125 µm/125 µm



Specifications

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 / ground plane 150 μm 150 μm
g min. spacing trace / BGA-pad 150 μm 125 μm
h min. spacing via-pad / via-pad 150 μm 125 μm
i min. spacing via-pad / ground plane 150 μm 150 μm
j min. spacing via-pad / BGA-pad 150 μm 125 μm
k min. spacing ground plane / ground plane 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 / ground plane 300 μm 300 μm
o min. spacing NPTH / BGA-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 / ground plane 250 μm 250 μm
s min. annular ring 200 μm 200 μm
t min. drill distance NPTH/NPTH 250 μm 250 μm
u min. drill distance PTH/PTH 250 μm 250 μm
v min. drill distance NPTH/PTH 250 μm 250 μm
w min. spacing BGA-pad / BGA-pad 150 μm 125 μm
x min. diameter BGA-pad 200 μm 125 μm

Please note:

  • burried, blind or tented vias are not supported
  • take extra care that you design your inner layers with positive polarity
  • t, u, v: drill distances refer to the tool diameter, please see here

Please also note that these rules are the bare minimum that we support. If you can leave some safety margins in your design, the PCBs will be more likely to work the way you intended them to.

2 Likes

Hello Christina, I have a suggestion here: Please add the hole to hole clearance too.

I took the value from your GitHub Repo which tells me 250 um.

Does this mean I cant use inner layers for ground planes?

Edit: I realise now what this means, the filled in area is where the copper is.

An additional question came up here: Could you add the BGA-Pad to BGA-Pad distance? And also the minimum BGA-Pad size?

PS: Thank you so much for adding the t, u and v values!

Hi @andreas_eet,

welcome to the community and thank you for the hint! The distance (t, u, v) is now listed above!

1 Like

Hi @CommanderLake,

welcome to the community!

“Edit: I realise now what this means, the filled in area is where the copper is.”

Exactly!

1 Like

Hi @andreas-eet,

thanks for this feedback, we will try to include this in our article, too!

Thank you!

1 Like

@christina , your posts states

Please also note that these rules are the bare minimum that we support. If you can leave some safety margins in your design, the PCBs will be more likely to work the way you intended them to.

is this mostly intended for traces and clearances or also for via sizes?
I am designing a PCB and using the smallest possible vias would be really beneficial (0.6/0.2)
is it save to use lots of these vias (around 30) or would it be better to go for (0.7/0.3)?

Hi @miloz,

welcome to the community!

In principle, this statement also refers to the dimension of vias. But if small vias (0.6/0.2) help you to realise your specific layout and thus bring you added value, then there is nothing to say against using them!

Best regards,
Manuel

Hi,
i stumbled across the same thing and still have some questions.
What polarity should be used for the outer layers?

I should be able to see the used polarity in KICAD, since copper traces and planes get displayed normal (positive) or inverted (negative) right?

Thanks in advance!

Nothing has to be negative.

1 Like

Is there a reason why the the eagle design rules on github are quite different from those above?
Which one should I use?

Hi @etik,

Welcome to the community!
I guess you mean the clearance/spacing values for simple? We included a little security margin and set them to 175 µm – if you need to, you can reduce those values to 150 µm in the .dru-file according to the table above.

In general, we try to keep the design rule files up to date. However, in case of doubt, the values listed above apply.

I would like to mention again that these values are minimum values. If your layout allows it, it does certainly make sense to design widths and distances with some safety margin.

Best regards,
Manuel

A post was merged into an existing topic: Plated and Non-Plated Slots and Cutouts

Hallo,

I am trying to route the LP8550, which have DSBGA 25 Footprint with 0.5 mm Pitch. Using this design-rules (4 Layer complex) it is impossible to route it.

If I kept the drill size 0.2 mm and tried to achieve outer-diameter from 0.35 mm (see Photo), is it possible to manufacture it?

One more question, are Ball-Pads supported?

I think that I and all Others will appreciate an article just about BGAs :smiley:.

Best Regards
Asmandar

Hi @kompass ,

Welcome to the community!

If I kept the drill size 0.2 mm and tried to achieve outer-diameter from 0.35 mm (see Photo), is it possible to manufacture it?

For BGAs with a pitch of 0.5 mm, we are at the limit of our technical capabilities.
Your suggestion to reduce the pad diameter to 0.35 mm - as I understand you - is not sufficient for a safe through-hole plating. Another problem with a 0.5 mm pitch is the minimum drill spacing (please see also here)

One more question, are Ball-Pads supported?

Do you mean via-in-pad? In principle, you can use via-in-pads in your layout and have them manufactured by us. However, please note that we do not fill the borehole. This allows solder to flow through the hole during assembly. When using our assembly service, via-in-pads are therefore not permitted.

I think that I and all Others will appreciate an article just about BGAs

Thanks for the feedback - it’s noted! :wink:

Best regards,
Manuel

1 Like