Stacked microvia or microvia in PADS layout

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

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

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.

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

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 .

Pcb Vision said:

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 .

Click to expand...

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?

*I would download this book and have a read:
https://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

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

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.