Stacked Micro-vias?

"Byron Jacquot"  skrev i nyhetsmeldingen:

1680887219.01416258258811.JavaMail.jive@flcspu-csapp-01.premierfarnell.com

...

I'm working on a layout for a very dense BGA part, with a 0.4mm ball

spacing.  Yes, I know this is expensive, cutting edge PCB technology.

I'm using the IPC recommendations for the part, which calls for an array

of "stacked micro-vias."  The micro-vias are arranged as an inverted

pyramid - the outer row of balls are routed on the surface of the board,

the second row on the next layer down, and so on.  Refer to slides 33 to

50 in the following presentation for an illustration of this technique.

Im sorry if I tell you things you already know here, but maybe its useful to

others.

First I have to ask, what is the reason for picking microvia technology over

very small normal vias?

0.4mm pith should be doable with 0.25mm drill? Remember smd pad can overlap

the rest-ring.

https://dcchapters.ipc.org/assets/pnw/presentations/20120726_microbga.pdf

The part I'm using has 4 rows of balls, so I'm anticipating 4 signal

layers, possibly 5.

I'm having trouble figuring out how to specify this in Eagle.  Some of

the documentation I see tells me that it only does micro-vias between

adjacent layers.  Is that true?

I guess you have to specify the inner vias as blind vias, but keep drill

diameter tiny. I guess you know the limitations on core/prepreg thickness

for this? I'd rather use normal bigger (0.25mm) blind vias if you really

need it, but I guess you should manage with microvias + one blind between

all inner layers only, and maybe full through all layers if you already have

throughhole components. If you dont have through hole's, you can save a

process by not having it.

A 8 layer typical blind via setup is this:[2:(1(2+345*67)*16):7]

or if you dont have through holes:[2:1(2+345*67)*16:7]

if you REALLY want to throw money at it you can do madness like this

:[2:(((12+3)4)(5*(67*16))):7]

but you MUST talk to the manufacturer before doing mad stacks. You better

stay with any of the HDI standards.

At the moment, I've got a layer spec that allows me to use blind,

regular-size vias between the surface and varying deeper layers.  But as

soon as I try to use a micro-via within a BGA ball, it only lets me do

one layer.  Anything deeper, and it tells me "Can't set via to layer 3

at (x,y)."

To go deeper than 2nd layer, you need to add new via under it. I guess you

can save some money by offsetting the blind via from the microvia, so that

via doesnt need to be plugged with copper.

Eagle doesnt let us set microvias between inner layer, but a blind

definition ought to look the same in the gerbers as long as drill diameter

is small.

It does let you define microvias from outer to an inner, like with

, but again, talk to the manufacturer. They will

most likely protest (or take your money and run).

Have I found a limitiation of the tool, or do I just need to tweak my

layer stackup?

The only limitation I know is the inner microvia type, but as I mentioned, a

blind will do. What I dont know is if Eagle DRC will handle inner vias with

tiny drill as an exception, as it seems to do with outer microvias. Also, I

dont know if any manufacturers offer "buried microvias", but I dont see why

it should be a problem? (other than cost)

I notice a lot of people expect a PCB to come out ready from the files Eagle

generates. At best, the manufacturer will see a simple board, and pick some

standard material and process parameters without telling you.

For more complex boards (like this) and high end manufacturers, you need to

get involved in the stackup definition, material selection and manufacture

method.

I'm following the recommendations of both a board fab house and contract assembler.  They've referred me to the IPC recommendations for these packages, which call for stacked micro vias.  I'm listening to their advice, and trying to get it to translate into a board design.  I'm also finding that even 1 mil difference in capabilities changes what I can do significantly, like dog bones and staggered holes.

The layer specim workinf from is 3 prepreg + 2 layer core + 3 layer prepreg, with blind vias possible from the top to the next 3 layers, plus through vias.  In the parlance: [4:(1+2+3+(4*13)+14+15+16)]

(A related question: are board spec strings getting mangled by the forum software? Is there some better way to format them so they don't get mangled?)

With that stackup, I can do regular-size blind vias between 1-2, 1-3 and 1-4.  It's when I step down to in-pad micro-vias deeper than one layer that things don't work so well.  The system will let me do micro vias from 1 to 2, but no deeper.

I've also figured out how to fool it into letting me drop a really tiny blind via within the pad that goes deeper.  I set my regular via restrings and hole limits to the same as for micro-vias, then I lay trace from the pad, making a zigzag within the pad, leading back to the center, and then I change layers, and it lets me go deeper.  It just feels risky setting the DRC like that - I'm bypassing an otherwise sensible and useful check.

Byron Jacquot wrote on Fri, 21 November 2014 11:42

(A related question: are board spec strings getting mangled by the

forum

software? Is there some better way to format them so they don't get

mangled?)............

The Element14 access to the CadSoft Eagle newsgroup forums is a badly

implemented web front end with many shortcomings and this is yet another

example.

A better web experience is the front end/replication provided by

http://www.eaglecentral.ca/forums/

It has the best search facility. You need to request write access but that

arrives quickly.

I use it when on the move and when I need to search.

Keeping an eye on the daily posts is best/quickest using a newsreader.

Postings just arrive like emails and you can apply filters to filter out

threads or individuals. My filters all apply to Element14 to reduce the

amount crap that it generates.

All the best

Warren

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Just to report back about my hair-brained scheme:

I've also figured out how to fool it into letting me drop a really tiny blind via within the pad that goes deeper.  I set my regular via restrings and hole limits to the same as for micro-vias, then I lay trace from the pad, making a zigzag within the pad, leading back to the center, and then I change layers, and it lets me go deeper.  It just feels risky setting the DRC like that - I'm bypassing an otherwise sensible and useful check.

That won't work so well, aside from the risk introduced by bypassing the DRC.  I had a careful discussion with my PCB fabricator, and the CAM files aren't suitable for their machinery.

When I generate the drill files, I get a file per blind drill depth: 01 to 02, 01 to 03, and 01 to 04.  The contents are mutually exclusive; a hole in the 01 to 04 file only exists in that file, even though it passes through layers 2 and 3.

The problem arises in what is expected by the drill machine.  Stacked or staggered micro vias are laser ablated & plated after each lamination pass - layer 3 is laminated atop layer 4, then the micro vias between those layers are drilled, plated & plugged.  Then layer 2 is laminated on, and the next layer in the stack is drilled, plated and plugged - but only when it's in the appropriate drill files.

I suppose I could try to solve this with a script on the Excellon files, but that's not exactly moving this design towards completion, and still pretty risky, in terms of using tools that help me make functional boards.

I've had some direct dialogue with CadSoft, I'll update here if I learn anything new.

...and minutes after I wrote that, I heard from Cadsoft support, ann I think we've got it solved.  It's not terribly easy, but it's working to the degree that I've tested it.  CAM jobs are giving me 0102, 0203 and 0304 files, with the microvias present in each.

There are several pieces to this.

First, in the DRC, set the layer spec to allow blind vias between the adjacent layers: in this case 1 to 2, 2 to 3  and 3 to 4.

[2:(1+[3:2+[4:3+4*13+14]+15+16])]

Second, also in the DRC, set the min. micro via to a size smaller than the minimum drill.  In my current setup, that's: 0.5mm drills and  0.05mm microvias.

Then, then you want to stack micro vias from 1 to 4, it goes something like this:

1. Select the route tool.
2. Click on the BGA pad in question
3. Middle-click, and jump to layer 2.
4. Route trace a tiny bit away and click to solidify.  You'll get the microvia in the pad.
5. Make sure that the via diameter in the menu bar is set to the microvia size - 0.05mm.
6. Middle-click, and select layer 3.
7. Route a tiny bit away again, click, and you'll get the 2-3 microvia.
8. Middle click, and select layer 4.
9. Route a tiny bit away again, click, and you'll get the 3-4 microvia.
10. Finally, you can route away from the stack on layer 4.
11. This has created some staggered mircovias - all slightly misaligned from each other.  To make a true stacked microvia, go back, and move the vias atop each other.

Not quite a easy as just selecting layer 4 back in step 3.

"Byron Jacquot"  skrev i nyhetsmeldingen:

627571281.801417566480605.JavaMail.jive@flcspu-csapp-01.premierfarnell.com

...

First, in the DRC, set the layer spec to allow blind vias between the

adjacent layers: in this case 1 to 2, 2 to 3  and 3 to 4.

[2:(1[3:21516])]

Thanks for sharing. I would never guess this format. The example text in the

DRC setup doesnt cover it all, nor exlpain well enough (And I admit Im too

lazy to study the manual in details).

Byron Jacquot wrote on Wed, 03 December 2014 13:27

...and minutes after I wrote that, I heard from Cadsoft support, ann I

think we've got it solved.  It's not terribly easy, but it's working

to

the degree that I've tested it.  CAM jobs are giving me 0102, 0203

and

0304 files, with the microvias present in each.

 

There are several pieces to this.

 

First, in the DRC, set the layer spec to allow blind vias between the

adjacent layers: in this case 1 to 2, 2 to 3  and 3 to 4.

[2:(1[3:21516])]

 

 

Second, also in the DRC, set the min. micro via to a size smaller than

the minimum drill.  In my current setup, that's: 0.5mm drills and 

0.05mm microvias.

 

 

Then, then you want to stack micro vias from 1 to 4, it goes something

like this:

 

 

1. Select the route tool.

2. Click on the BGA pad in question

3. Middle-click, and jump to layer 2.

4. Route trace a tiny bit away and click to solidify.  You'll get the

microvia in the pad.

5. Make sure that the via diameter in the menu bar is set to the

microvia size - 0.05mm.

6. Middle-click, and select layer 3.

7. Route a tiny bit away again, click, and you'll get the 2-3

microvia.

8. Middle click, and select layer 4.

9. Route a tiny bit away again, click, and you'll get the 3-4

microvia.

10. Finally, you can route away from the stack on layer 4.

11. This has created some staggered mircovias - all slightly

misaligned

from each other.  To make a true stacked microvia, go back, and move

the

vias atop each other.

 

Not quite a easy as just selecting layer 4 back in step 3.

 

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/133617

On the basis of that written above, a ULP could do it all from the initial

microvia placed between layer 1 and 2. You would place the initial microvia

and then run the ULP, specifying the final layer.

Warren 

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

I must say this conversation got me so confused I loved it. I learned a lot here.