Welcome to EDAboard.com

Welcome to our site! EDAboard.com 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.

Need refernces on standard via sizes

Status
Not open for further replies.

Rame

Full Member level 6
Joined
Dec 23, 2005
Messages
373
Helped
47
Reputation
94
Reaction score
7
Trophy points
1,298
Location
BANGALORE
Activity points
3,810
what is the min via size can be used?

Hi Folks,

Can anyone refer some links r send some pdf's realted to standard via sizes used.


Rerads
RAME
 

attylus76

Junior Member level 2
Joined
May 25, 2004
Messages
24
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
210
Re: Min Via Size

Hi Rame,

Who realizez the circuit to yuo declares that the holes can be realized until a 0,3mm. The pad it must be increased the 24mils respect to hole. generally I use holes from 0,6mm and pad from 0.7mm
 

Miles

Newbie level 2
Joined
Mar 7, 2006
Messages
2
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,312
Re: Min Via Size

Hello

Generally you should try to use vias bigger than minimum size. However for most manufacturers you may use vias as small as 1/5th of board thickness in diameter. As such I'm not sure there are standards for the sizes...

I hope that was helpful.
 

House_Cat

Advanced Member level 4
Joined
Feb 21, 2002
Messages
1,371
Helped
406
Reputation
812
Reaction score
98
Trophy points
1,328
Location
USA
Activity points
16,416
Re: Min Via Size

The size of a via is driven by several different engineering concerns. There is no such thing as "standard size vias".

For very high frequency circuits, you want to keep the inductance of your vias as small as possible. This translates into small diameter vias. On the other end of the spectrum is a via used for power - it may have to be large diameter to provide enough copper to carry high current without excessive heating.

How small the via can be is determined by how thick the circuit board will be when you are done. Board fabricators call this the "aspect ratio". How large a via can be is determined by the drill and route capabilities of your PCB fabricator.

The size of the annulus of copper you need to use is determined by your drill size. When a via is drilled by the fabricator, he has to use a bit that is 2-3mils larger than the final plated size of the hole - this is to make room for the copper plate inside the hole. He also needs a large enough annulus on both the top and bottom of the board to allow the plating process to proceed properly. Normally this is at least 4mils greater radius than the drill size. For example, you choose a finished hole size of 15mils. That will make the drill size about 18mils and the copper annulus will have to be at least 18mils+8mils=26mils.

One of the largest board manufacturers in the world is Merix. They have a manual available on their website that discusses the physical limitations for manufacturing a board. It is called their "Design for Manufacturabiltiy (DFM) Manual", and you can get it at: https://www.merix.com/DFMrevb11904.pdf
 

    Rame

    Points: 2
    Helpful Answer Positive Rating

Rame

Full Member level 6
Joined
Dec 23, 2005
Messages
373
Helped
47
Reputation
94
Reaction score
7
Trophy points
1,298
Location
BANGALORE
Activity points
3,810
Re: Min Via Size

Hi House cat,

Thanx for the details and do appreciate for the pdf link you had refer,its really informative.



Regards

Rame
 

krishnanice

Newbie level 5
Joined
Apr 8, 2006
Messages
10
Helped
0
Reputation
8
Reaction score
0
Trophy points
1,281
Activity points
1,371
Min Via Size

Well, Mr. House Cat - Thank you for the support. I learned something that I never knew :)
 

andre_teprom

Super Moderator
Staff member
Joined
Nov 7, 2006
Messages
9,299
Helped
1,161
Reputation
2,341
Reaction score
1,151
Trophy points
1,403
Location
Brazil
Activity points
54,161
Re: Min Via Size

A usefull criterion is :

( Via_Diameter - Hole_Diameter ) > 20 mils
 

chinta

Member level 2
Joined
Nov 9, 2006
Messages
51
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,286
Activity points
1,521
Min Via Size

you use from 0.2mm to 0.4mm depends on density and requirements. also you can go to the HDI method where you can use 0.076mm micro vias, but manufacturing will be expensive.
 

vijaya_narayana

Full Member level 3
Joined
Jun 12, 2007
Messages
172
Helped
11
Reputation
22
Reaction score
1
Trophy points
1,298
Location
India
Activity points
2,159
Re: Min Via Size

the minimum via size depends upon the PCB Processing unit also they must be capable of processing the minimum via size that we use in the design
i am using a via size of 0.2 to 0.3mm
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top