Continue to Site

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.

Register Log in

minimum via size for four layer PCB?

Status
Not open for further replies.
T

treez

Guest
Is it true that minimum via sizes in four (or more) layer PCB's have to be bigger than for two layer boards?

Its just that i imaging its jolly difficult to line up the via holes when the layers/cores/prepregs are stuck together?.........and so the vias need to be larger in diameter?
 

Nothing like that. Your via size can be anything. Even it can very small.

But you must contact your manufacturer because minimum via size means minimum size hole(drill) and adds you more cost.

Best wishes :)
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
My suggestion is to use industry standard design rules that can be produced by any PCB manufacturer including prototype services like PCB pool or Multi-cb without additional costs. 0.3 mm drill and 0.15 mm copper width and clearance (0.6 mm via pads) applies both to 2-layer and multilayer boards. Smaller drills (0.2mm and 0.1mm copper structures are also managed by most manufacturers, with about 20 to 25% surcharge.

For mass production, it may be reasonable to use relaxed design rules (e.g 0.4 mm drill, 0.2 mm strcuture width) and get a cost benefit and higher reliability.
 
I don't think it will make any difference between 2 and 4 layers. When you get up to over 8 or 10 layer, then you have to worry about it. It is all about cost of pcb, some cheap place specify the minimum to be bigger. Call the place you fab your board.

I believe the main reason for bigger pads and vias for many layer boards is because they worry about the layers slide and have a slight offset when they press on it to form the board. I designed a 26 layer board, and I had to make the vias pad size bigger to ensure the drill land on all the pads in different layers. But that's an extreme. Talk to the fab house, we can't tell you the lower limit.

For high volume production and reliability, I would use more relaxed size to make sure the boards are reliable.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
No there are NOT any relation like that. There is an aspect ratio demanding the hole being maximum x times smaller than thickness of board/layers.
If Your board is 1.6 mm a standard high volume ratio is 1:8 having the should be bigger than 1.6/8 = 0.2. These drills dies very fast, so go to 0.3 would use a much much stronger drill and cost will be reduced significant.
The size of hole does not matter of numbers of layers but thickness. A 4 layer 1.6mm board needs larger holes than a 8 layer 0.8mm board.
Again many fabrics have a pricecurve corner near 0.2 - 0.3 mm drills, thus ask.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top