Alexander,
maybe "every boardhouse" was a bit too optimistic, but 1:1 is very common (at
least all our standard PCB manufacturers can do that). I read papers about
board houses that can do 1.5:1 on request (I think coast to coast PCB offered
that), and even papers about how to do 3:1 see here:
http://ieeexplore.ieee.org/document/795855/
I also read articles about electrolytes and processes that claim >40:1 thru
hole plating (really impressive cross section images shown there, unfortunately
I can't find the paper anymore). But as you said it all that comes at a cost,
and the yield is usually bad.
I think we can agree that for blind vias you should always design for aspect
ratios <1 and for thru holes 15:1 and you will find many board shops that can
build it. If you need to push the envelope, finding a manufacturer will be
tricky, and cost will rise.
BR,
Gert
----------------------------------------
HARTING AG & Co. KG, Postfach 11 33, 32325 Espelkamp; Marienwerderstraße 3,
32339 Espelkamp
Generalbevollmächtigte Gesellschafterin: Dipl.-Hdl. Margrit Harting
Persönlich haftende Gesellschafterin: HARTING WiMa AG (Luxemburg) & Co. KG;
Amtsgericht Bad Oeynhausen; HRA 8259; persönlich haftende Gesellschafterin:
HARTING Führungs AG (Registre de Commerce et des Sociétés Luxembourg), B
170749, Luxemburg
Vorstand: Dipl.-Kfm. Philip F. W. Harting (Vorsitzender), Dipl.-Kffr. Maresa W.
M. Harting-Hertz, Dipl.-Kfm. Dr.-Ing. E. h. Dietmar Harting, Dr. rer. nat.
Frank Brode, Dipl.-Ing. (FH), Dipl.-Wirtsch.-Ing. (FH) Andreas Conrad, Dr. iur.
Michael Pütz;
Sitz der Gesellschaft: Espelkamp; Amtsgericht Bad Oeynhausen; HRA 9021; UST-ld
Nr. DE812136745
-----Original Message-----
From: Alexander Ippich [mailto:alexander.ippich@xxxxxxxxxxxxxxx]
Sent: Monday, June 12, 2017 10:43 AM
To: Havermann, Gert <Gert.Havermann@xxxxxxxxxxx>
Cc: si-list@xxxxxxxxxxxxx; Alexander Ippich <alexander.ippich@xxxxxxxxxxxxxxx>
Subject: RE: [SI-LIST] Re: Blind Vias & Plating Question
Gert,
I do disagree with your statement that every board shop can handle an aspect
ratio of 1:1.
My experience is, that for real blind vias (i.e. vias that have to be plated
from one end and not still being a through via during plating), aspect ratios
that are exceeding 0.8:1 are very difficult. So for the 7mil drill depth, the
via diameter would have to be close to 9mils.
I have not yet seen anybody being able to do an aspect ratio of 2:1 for blind
vias (through vias are different, many shops routinely plate aspect ratios of
larger than 10:1 (sometimes going even to 20:1).
But I absolutely agree with your statement that PCB processes and technologies
are very complex and that it is always a good idea to talk to your board house
of choice as early as possible. Otherwise, people tend to end up with designs
that cannot be produced or are very expensive.
It is very tempting to use all these nice blind and buried vias and do
sequential lamination in the design software. But it is very important to
understand, that it may be far from easy on the manufacturing floor after the
Gerber output.
Best regards,
alex
----------------------------------------------------------------------------------------------------------------------------------------
Alexander Ippich
Senior Signal Integrity Engineer
OEM Marketing Europe
Tel.: +49 170 / 63 68 571
e-mail: alexander.ippich@xxxxxxxxxxxxxxx
web: www.isola-group.com
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On ;
Behalf Of Havermann, Gert
Sent: Monday, June 12, 2017 10:17 AM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Blind Vias & Plating Question
Hi SI Guy,
You are missing the most important information: Drill Diameter!!
Blind via plating only works up to a certain aspect ratio (Drill diameter/Drill
Depth). Every Boardshop can handle an aspect ratio of 1:1, some can do 1:2 or
even better. That would mean for standard processes with your 6-Layer board and
approx. 7mil drilldepth (L1-L3) can have a minimum Drill diameter of 7mil. If
you want to use Laser drilling, then usually the next copper Layer is the max
drilldepth, but some board houses can drill furtheron to the next layer. The
next thing is that if you want to contact on all three layers, that is another
critical task not every boardhouse can perform.
If your Design already violates the aspect ratio of the boardhouse, then they
need to treat the holes as buried vias and that means inner layer plating (with
the added cost). For better impedance control the boardhouse can use a special
masking process in order to plate only the annual ring of the via, but not the
traces. This is nice for Test fixtures or other low volume PCB, but for high
volume designs this is a tough task because high volume depends on a fixed
process, and that means a standard process.
I could go on forever talking about processes and technologies because PCB is a
real complex piece of technologie these days. You need to know the technology
you want to use in great detail, or talk to the boardhouse to learn about the
details. This is especially true for Signal integrity.
Btw: Why did you decide to use blind vias from L1-L3 and L4-L6? Would
Backdrilling be an option or is it really the high density you need?
BR,
Gert
----------------------------------------
HARTING AG & Co. KG, Postfach 11 33, 32325 Espelkamp; Marienwerderstraße 3,
32339 Espelkamp Generalbevollmächtigte Gesellschafterin: Dipl.-Hdl. Margrit
Harting Persönlich haftende Gesellschafterin: HARTING WiMa AG (Luxemburg) & Co.
KG; Amtsgericht Bad Oeynhausen; HRA 8259; persönlich haftende
Gesellschafterin: HARTING Führungs AG (Registre de Commerce et des Sociétés
Luxembourg), B 170749, Luxemburg
Vorstand: Dipl.-Kfm. Philip F. W. Harting (Vorsitzender), Dipl.-Kffr. Maresa W.
M. Harting-Hertz, Dipl.-Kfm. Dr.-Ing. E. h. Dietmar Harting, Dr. rer.
nat. Frank Brode, Dipl.-Ing. (FH), Dipl.-Wirtsch.-Ing. (FH) Andreas Conrad, Dr.
iur. Michael Pütz; Sitz der Gesellschaft: Espelkamp; Amtsgericht Bad
Oeynhausen; HRA 9021; UST-ld Nr. DE812136745
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On ;
Behalf Of Loyer, Jeff
Sent: Sunday, June 11, 2017 7:22 PM
To: CurtM@xxxxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Blind Vias & Plating Question
Hi Curt,
The dielectric thicknesses on the designs I'm thinking of are something
like:
* L1-L2 PP: 2.7 mil
* L2-L3 Core: 4 mil
* L3-L4 PP: whatever thickness is takes to reach target overall thickness
* L4-L5 Core: 4 mil
* L5-L6 PP: 2.7 mil
Laser drilled blind via through ~7 mils of dielectric to reach from L1 to L3.
Cannot be stacked since this isn't a build-up (multi-lamination) design.
Likewise for L6 to L4. Does that make sense?
Another other option is to make the design w/ PTH's and have those vias
backdrilled, be sure to provide enough clearance around the vias to accommodate
that.
Jeff Loyer
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On ;
Behalf Of Curt McNamara
Sent: Sunday, June 11, 2017 9:58 AM
To: silistguy@xxxxxxxxx; si-list@xxxxxxxxxxxxx; dmarc-noreply@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Blind Vias & Plating Question
Jeff, would these be stacked micro vias? Since they go from L1 to L3.
On the original posters design, there are six layers. If L1-L2 and L2-L3 are
four mils, the total dielectric thickness for the significant layers would be
16 mils. I have done that with flex, usually PCBs are a bit thicker.
Curt
https://goo.gl/images/4VKCV6
________________________________
From: si-list-bounce@xxxxxxxxxxxxx <si-list-bounce@xxxxxxxxxxxxx> on behalf of
Loyer, Jeff <dmarc-noreply@xxxxxxxxxxxxx>
Sent: Sunday, June 11, 2017 10:57:57 AM
To: silistguy@xxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Blind Vias & Plating Question
I agree with Istvan. There are fab houses that can laser drill through the
outer two dielectric layers without requiring build-up layers. I would shop
for a fab house that can do this. As Istvan noted, it will depend on your
dielectric thickness, I assume you're using standard thicknesses (3-4 mil) for
the significant layers. Else, you'll be forced to use build-up technology.
Jeff Loyer
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On ;
Behalf Of Curt McNamara
Sent: Saturday, June 10, 2017 5:38 PM
To: leeritchey <leeritchey@xxxxxxxxxxxxx>; silistguy@xxxxxxxxx;
si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Blind Vias & Plating Question
Lee and i are agreeing :-) that the board will most likely be drilled (and vias
plated) as a 3 layer structure. The plating process (required to fill the L1-3
vias) will increase copper thickness on L3.
Curt
________________________________
From: leeritchey <leeritchey@xxxxxxxxxxxxx>
Sent: Saturday, June 10, 2017 4:39:01 PM
To: Curt McNamara; silistguy@xxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: RE: [SI-LIST] Re: Blind Vias & Plating Question
Actually, a 6 lever boated will be built with L2 and L3 on a piece of laminate,
L4 and L5 on a,piece of laminate and the two outer layers as pieces of foil.
Sent via the Samsung Galaxy S(r) 6, an AT&T 4G LTE smartphone
-------- Original message --------
From: Curt McNamara <CurtM@xxxxxxxxxxx>
Date: 06/10/2017 9:04 AM (GMT-08:00)
To: silistguy@xxxxxxxxx, si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Blind Vias & Plating Question
Lots of great answers!
Here is my simple version:
PCB material (sometimes called clad) comes with copper on one or two sides.
Board houses often build from the center out.
So 3-4 (your inner layer pair) would (normally) be built by itself (as would
1-2 and 5-6).
Building a layer pair consists of:
-- imaging the circuits onto the bare copper
-- etching the unwanted copper away
-- drilling holes where vias go through the layer pair
-- plating the layer pair if there are via holes that don't pass through the
whole PCB. Plating is required to get copper in the via barrel.
In your case, they might have wanted to build 1-2, 3-4, and 5-6 separately.
Then laminate together, and plate through vias. However, then they would be
trying to build up via wall material with one side plugged (for your 1-3 and
4-6 vias). This probably can't be done with normal via aspect ratio.
Since you have vias from 1-3 and 4-6, this board will be made a different way.
How? As others have suggested, you have to ask them. It might be that they
built 1-2-3 and 4-5-6 so they could plate your 1-3 and 4-6. Then they would
laminate 1-2-3 to 4-5-6 and do final plating for through-board vias.
How do they build 1-2-3? With 1-2 or 2-3 as double sided clad, and then a
second operation to add the other layer as single sided clad. Followed by
drilling for the 1-3 vias, and finally plating to fill those via walls/barrels.
That may not be the explanation, however it could fit your description.
Curt
http://www.4pcb.com/media/presentation-how-to-build-pcb.pdf
Curt McNamara, P.E.
Engineering Consultant
612.305.0440 x248
www.npe-inc.com<http://www.npe-inc.com>
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On ;
Behalf Of SI Guy
Sent: Friday, June 9, 2017 3:59 PM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Blind Vias & Plating Question
Hi Experts,
I did my first design with blind vias. It's already starting to kick my ass
AFTER I've already designed it. I realize the importance of contacting board
shop before design, too bad boss doesn't allow the engineer to control that.
My question is then, experts, if blind vias are used say 1-3 and 4-6 on a 6
layer foil lamination board, do those inner layers also have to have plating in
addition to the bare copper thickness? Always?
I used 1/2 oz cu on all layers and expected only outer layers to have some
extra thickness from plating. Now a shop is saying no no no, 3 and 4 will be
plated too. Now my inner layer transmission line equations are jacked up!
Not to mention the outer layers too.
Sad day. =(
Any experience would help. What in the world is the right way to approach these
situations. Books and seminars say one thing but then life kicks your butt. So
frustrating!!!
Thank you, experts.
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
--
Any quotation or order confirmation provided with this communication is subject
to Isola’s standard terms and conditions of sale which can be found here
http://www.isola-group.com/about-us/terms-conditions/
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
