Continue to Site

Welcome to

Welcome to our site! is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

VIA size on the board - what are the factors?

Not open for further replies.


Member level 3
Jul 24, 2002
Reaction score
Trophy points
Activity points
industry via size

Hello all,
i want to know ,all the factors on which i can choose the size of a via on my board.

best regards

via size, high current

hi .. i do not understand the question, did you mean the factors which can influence via size ?? It can be software dependand anyway I am using 24mil hole,40mil plane for normal signals and 31mil hole, 62 mil plane for Vcc etc.



via size and inductance

Hello cancel,
let me be specific here......i want to know, why the vias used for power and ground are having big size than the vias used for signals......does this depends on the current carrying capacity of vias???or is it manufacturing constraint..???

why do people use different via sizes in there designs??

i have read in one of the application note that.....the diameter of via must be at least equal to the trace width divided by 3......

so....are there any other factors on which one can decide the via size??

thanks for response.....

best regards

Typical values for the majority of factories.
The relation of diameter of a drill to thickness of the PCB: ~1/6
Minimal diameter of a drill via: Dmin = 0.3 mm
Contact platform of via: Dmin + 0.4 mm
Clearing in a ground plane: Dmin + 0.9 mm

Hello ZmGor,
You have mentioned the method(or formula to be specific) to calculate contact pad and clearance pad of minimum via.

Is this some standard or you just follow the above concept.

Some manufactuerers can even achieve minimum via of 6 mil(0.15 mm) diameter.

where from you got the figure of .3 mm??

is there any document with you,which can be helpful in the study of via ??

best regrds

ZmGor said:
Typical values for the majority of factories.
The relation of diameter of a drill to thickness of the PCB: ~1/6
Minimal diameter of a drill via: Dmin = 0.3 mm
Contact platform of via: Dmin + 0.4 mm
Clearing in a ground plane: Dmin + 0.9 mm

These meanings are suitable for manufacturing PCB almost at any factory with an accuracy class not below 5.
More rigid requirements demand the coordination with a factory the manufacturer, and it is not enough such factories.

On the size via.
For reduction of inductance of leading of a Power/Ground it is possible to use the increased size via, or more than 1 via for one pad.

Minimal diameter of a drill via: Dim=0.1mm (mechanical drill)
If you use UV laser, may be .04mm.
But it is more expensive when the diameter is less then 0.3mm.
If the current for vias is not the problem ,I think the hole size depend on you track density.
.45mm-.9mm is very cheap,and the position tolerance is better.

The minimum size of the via drilled hole is relative to the thickness of the PCB. The ratio is between 1:5 and 1:6 depending on you board manufacturer.
A 1.6mm PCB would have a minimun via drill size of around 0.3mm. This is the board thickness to hole plating ratio. If the hole is any smaller it becomes difficult to plate all the way throught the via hole.
Most board manufacturers would like to see a via hole to pad ratio of 1:2 so that the pad is twice the size of the drilled hole, smaller via pads run the risk of the hole breaking out from the side of the pad if the drill wanders as it cuts through the PCB material.
With blind via holes it is only possible to plate a hole as deep as its diameter, If the blind hole is 0.1mm diameter then its plating depth will then only be 0.1mm and this must be the maximum distance to the next layer in the stack.

Need more info please respond: :D

Phil 8O

Via size

see this calculator

:) perfect!

/ Warning #1 - No thanks at elektroda! /

via size..

actually wilson raised a very good question on via size here.unfortunately no one answer a technical reason or explanation for their via calculations.
I have been looking for a good solution for this via problem in my design.

most of the calculations available in market are mere claculations suitable for manufacturing easiness, i can't find a relevent standard say for 10 mil track u should have atleast a via with 20mil internal dia and 35 mil outside dia. so so...overall people prefer to put a unique and flexible dimensions interms of PCB manufacturing.

But to my surprise here are some catch points.. what via does to ur track is just form a 90 deg vertical bent to the signal you are trying to feed. so no matter how much thickness the track got you still can place a via enclosed by a track, to be specific if the track is 30mil track you can connect it with a 15 mil via..there is no technical problem i could see..but when it comes to signal integrity issues and high speed signals..i am pretty sure there is something interesting to check with that vertical pass u created on the board by connecting tracks with vias.
if so....
i hope someone can contribute more on that aspect.

Synq- The problem is the question is very general, and the answer has many possibilities.

First is the problem of actually making the board - there are guidelines for the minimum drill size that the board manufacturer is able to use for a particular board thickness. The hole has to be drilled oversize to allow for plating the hole, and the oversize drill can't wipe out the copper annulus - that determines the minimum pad diameter before plating. The density of traces and other pads also places a practical layout size constraint for ensuring clean etching between board features.

Next is the electrical concern for the via. How much current will it have to carry? High current requires multiple vias and/or larger barrel diameter.

Signal integrity requires examining via characteristics for fast risetime signals and high frequency signals. Vias have both inductance and capacitance. The designer has to analyze those parameters if the signal cannot tolerate the distortion/reflection/attenuation/coupling that will be caused by the introduction of via inductance and capacitance.

The short answer is that you can use any convenient via size that meets manufacturing limitations for non-critical signal paths. If you are talking about fast, high frequency, signals - you need to do some engineering, and analyze the impedance and coupling characteristics of vias with respect to their surroundings on the board.

via size..


What u said is true for commercial manufacturing terms..but as the nanometry chip packages are flushing into market, the PCB manufacturers are forced to change the normal or conventional manufacturing process. Microvias of 5 mil and track clearence of 4 mil are now common practice in the industry(cost, i believe sucks well....)

the paper i uploaded will give some extra light into laser technology used against conventional etching and scaling process in Pcb.

here is one good pdf which i found on search and would like to share it with u all explains the plated through holes theory.....

hope will be helpful.......
anyway if anybody has some other interesting material or has some good views to share can contribute to the discussion......

best regards........


Try this doc from ultracad info on vias.

P :D


    Points: 2
    Helpful Answer Positive Rating

figure 2,3 in the file you attached is invisible.

yaa...i too do not have the file with those figures.....i tried to search but was not able to locate the file with figures 3 n 4....
sorry for that....


Not open for further replies.

Part and Inventory Search

Welcome to