Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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

Stacked microvia or microvia in PADS layout

Status
Not open for further replies.

viperpaki007

Full Member level 5
Joined
Jul 2, 2008
Messages
270
Helped
11
Reputation
22
Reaction score
8
Trophy points
1,298
Location
Finland
Activity points
3,393
Hi,

I need to route the 2nd inner layer of 0.4mm pitch BGA package to bottom signal layer in a 4 layer PCB board. I have seen that people use microvias on the BGA pads to route the traces to lower layers. In addition, i have also read that the aspect ratio of microvias should be around 1/0.8 (diameter/depth) to meet manufacturer restrictions. This means that i cannot have microvia depth of more than 80um if my microvia depth is 100um. In a 4 layer PCB, a microvia from top to bottom layer will certainly have much deeper depth than 80um. How should i put a microvia in such situation then? Should i use a stacked microvia in this situation?. More importantly, if i have to use a stacked microvia then how can i define a stacked microvia in PADS layout?

BR
 

Pcb Vision

Newbie level 6
Joined
Oct 14, 2011
Messages
13
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,283
Activity points
1,368
Hi,

you can use Microvia 1-2 buried via 2-3 and 3-4 to make the connection between top to bottom , buried holes 2-3 must be filled by resin and then plating copper to cover them, then the microvia 1-2 and 3-4 can staked on buried holes B2-3, this type of design was defined as VOP. microvia holes 1-2 and 3-4 shall be drilled by laser machine.

Koen
 

viperpaki007

Full Member level 5
Joined
Jul 2, 2008
Messages
270
Helped
11
Reputation
22
Reaction score
8
Trophy points
1,298
Location
Finland
Activity points
3,393
Hi Pcb Vision,

Thank you for the explanation, but how i can do these things in PADS layout? So far i am unable to find any options for stacked microvia or burried microvia.
 

Pcb Vision

Newbie level 6
Joined
Oct 14, 2011
Messages
13
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,283
Activity points
1,368
Sorry,
i am not professional in PCB layout, and i am professional in PCB fabrication and quality problem shooting.
hope you can settle this case earlier.

Koen.Hu
 

Pcb Vision

Newbie level 6
Joined
Oct 14, 2011
Messages
13
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,283
Activity points
1,368
Hello,

i think out the characters of this kind of design , there are some difference compared to conventional 4L boards , conventional PCB has one drill tap only for through hole, but for stacked via design, there will be four type of drill holes
1. Blind via holes L1-2
2. buried via holes B2-3
3. blind via holes L3-4
4. through holes between top to bottom

when you design the stackvia holes, you must ensure the blind holes were desgined at the same location with buried via B2-3, and inner pads must be kept for each buried via holes, hope above information can help you finish your design . by the way, i can help you to reveiw your design to confirm if it is well designed when you finished the design.i familiar with cell phone boards design which usually use stack-via .
 

viperpaki007

Full Member level 5
Joined
Jul 2, 2008
Messages
270
Helped
11
Reputation
22
Reaction score
8
Trophy points
1,298
Location
Finland
Activity points
3,393
Hello,

when you design the stackvia holes, you must ensure the blind holes were desgined at the same location with buried via B2-3, and inner pads must be kept for each buried via holes, hope above information can help you finish your design . by the way, i can help you to reveiw your design to confirm if it is well designed when you finished the design.i familiar with cell phone boards design which usually use stack-via .

Hi Pcb vision,

So u mean that my burried via(L2-L3) should be exactly below the microvia (L1-L2)? If this is the case, then will this not cause clearance violations in inner layers as burried vias are much bigger in size then microvias and will be overlapping withe each. Is there a possibility to use stacked microvias as well?
 

marce

Advanced Member level 5
Joined
Feb 23, 2010
Messages
2,010
Helped
622
Reputation
1,244
Reaction score
606
Trophy points
1,393
Location
UNITED KINGDOM
Activity points
13,922
*I would download this book and have a read:
http://hdihandbook.com/
Also IPC-2226 specification, abd finaly have a look at Wurth Electronics site, lots of good information on doing HDI boards.
Stacked micro vias is the more expensive option, non stacked (dog bone) connected microvia boards are cheeper to manufacture.
A bit more info:
www.dnu.no/arkiv3/HDI Technology Presentation.pdf

Look up: HDI PCB design, in google
 

Pcb Vision

Newbie level 6
Joined
Oct 14, 2011
Messages
13
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,283
Activity points
1,368
Hello Viper,

yes, i mean the microvia should be designed on the top of buried via holes B2-3, you know normal huried via holes size is about 0.2-0.3mm, and the microvia holes is around 0.1mm, even if there are some misalignment during drilling microvia , the misalignment is still no more than 0.1mm, and also, buried via holes B2-3 have the responding annular ring , the little clearance will not affect the connection between L1-2 to B2-3.
Since stacked via holes are made normally with laser machine, you know laser is hard to drill the laminate which are thicker than 0.1mm. i have the experience in stackvwillia holes, if you design stackvia holes for a four layers boards, the production cost will be high and the final boards thickness will be thin( about 0.3-0.4mm).
hope you can get my meaning.

Koen.Hu
 

Pcb Vision

Newbie level 6
Joined
Oct 14, 2011
Messages
13
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,283
Activity points
1,368
Hi,

you also can use normail via holes (diameter 0.2mm)will be designed on BGA pads, in order to avoid the quality issue, you can required via holes in BGA pads capped , in this way, manufacture will plugged these via holes with resin after copper plating for these via holes and then plating to cover these holes, the cap thickness on these via holes is about 10um. this way can avoid the difficulty in aspect ratio. but the cost will be a little higher normal conventional technology.
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top