PCB Stack

Hi

I am designing a PCB with a Virtex II Pro and some DDR memory so need to
use a controlled impedance board. I am going to use an 8 layer board. My
question is do I need to specify to the PCB manufacturer the various
thickness of each layer and the gaps or is there a standard that they will
use.

Cheers

Jon

'Controlled impedance' means just that, you (the engineer) specify the 
stackup so that the impedance meets the requirements for your design. 
Leaving it to the PCB manufacturer means that you're not controlling it but 
willing to accept whatever they may happen to make.

KJ

"maxascent" <maxascent@yahoo.co.uk> wrote in message 
news:66SdnZGmQa9ouKPZRVn_vA@giganews.com...
> Hi
>
> I am designing a PCB with a Virtex II Pro and some DDR memory so need to
> use a controlled impedance board. I am going to use an 8 layer board. My
> question is do I need to specify to the PCB manufacturer the various
> thickness of each layer and the gaps or is there a standard that they will
> use.
>
> Cheers
>
> Jon
>
> 

I understand what you are saying but is there any industry standard values
that are used. If I were to use these then I can adjust my track size to
get the impedance I need.

Cheers

Jon

maxascent wrote:
> Hi
> 
> I am designing a PCB with a Virtex II Pro and some DDR memory so need to
> use a controlled impedance board. I am going to use an 8 layer board. My
> question is do I need to specify to the PCB manufacturer the various
> thickness of each layer and the gaps or is there a standard that they will
> use.
Contact the PCB manufacturer and tell them the stackup (for example, 
signal, GND, 3.3V, signal), tell them the impedance that you want and 
have them tell you the design rules (for example, 5 mil lines and 5 mil 
spaces). Controlled impedance is a combination of line width and 
spacing, dielectric thickness and dielectric constant. The board 
manufacturer knows what dielectrics are available to them, so they can 
advise what rules to use for their dielectrics.

---
Joe Samson
Pixel Velocity

maxascent wrote:

> I understand what you are saying but is there any industry standard values
> that are used. If I were to use these then I can adjust my track size to
> get the impedance I need.

Yes, ask your manufacturer.

Rene
-- 
Ing.Buero R.Tschaggelar - http://www.ibrtses.com
& commercial newsgroups - http://www.talkto.net

maxascent wrote:

> Hi
> 
> I am designing a PCB with a Virtex II Pro and some DDR memory so need to
> use a controlled impedance board. I am going to use an 8 layer board. My
> question is do I need to specify to the PCB manufacturer the various
> thickness of each layer and the gaps or is there a standard that they will
> use.
> 
> Cheers
> 
> Jon

Our typical flow is:
   1) propose stackup,
   2) ask vendor for comments,
   3) if it's not laughable results from the new guy, evaluate the 
vendor's tweaks to the stackup,
   4) lay out with the requisite line widths.

There is no standard, only required dielectric thicknesses for your line 
widths or vice-versa.  If you specify impedances, they will tweak the 
line widths for the dielectrics they use by adding test coupons for TDR 
measurements to guarantee production within your tolerance.

"KJ" <kkjennings@sbcglobal.net> wrote in message
news:lSp%f.58590$F_3.44450@newssvr29.news.prodigy.net...
> 'Controlled impedance' means just that, you (the engineer) specify the
> stackup so that the impedance meets the requirements for your design.
> Leaving it to the PCB manufacturer means that you're not controlling it
but
> willing to accept whatever they may happen to make.
>

In most cases board manufacturers have much better abilities to control
impedance than board designers. I usually would run Polar impedance
calculator to make sure my design is feasible but would leave actual precise
control to the board house. In some cases where it matters (RF) I would add
some extra constraints such as, for example, dielectric thickness should be
at least 10 mil. The line widths don't have to be exact in the design. The
board house will fix them. Interestingly, our board house doesn't charge
extra if they need to decrease the line width to below 4 mil for the
impedance control purposes, but they do charge if the lines are below 4 mil
in the original design!

/Mikhail

"maxascent" <maxascent@yahoo.co.uk> wrote in message
news:66SdnZGmQa9ouKPZRVn_vA@giganews.com...
> Hi
>
> I am designing a PCB with a Virtex II Pro and some DDR memory so need to
> use a controlled impedance board. I am going to use an 8 layer board. My
> question is do I need to specify to the PCB manufacturer the various
> thickness of each layer and the gaps or is there a standard that they will
> use.

There is no standard, but most of the boards use FR4 material with the
dielectric constant of about 4.3. It works out that a 5 mil track with 5 mil
separation from a plane (assuming the second plane is at least 15 mil away)
gives you approximately 50 Ohm impedance.

How many layers of your stackup are planes? Generally speaking a 8-layer
board is not very convenient for impedance control. To make it easy you need
to have planes next to your top and bottom layers as well as the planes
separating each two internal signal layers. Consider 10 layers instead:

1. Top
2. Plane
3. In1
4. In2
5. Plane
6. Plane
7. In3
8. In4
9. Plane
10. Bottom

Note that there is an issue of copper balance, i.e. the stackup needs to be
symmetrical to prevent board warpage.

/Mikhail

"maxascent" <maxascent@yahoo.co.uk> wrote in message 
news:4a6dna5Wvce536PZRVn_vA@giganews.com...
>I understand what you are saying but is there any industry standard values
> that are used. If I were to use these then I can adjust my track size to
> get the impedance I need.
>

Not really, it's up to you to work out the details but they're not terribly 
difficult to work out then you'll find that in many cases you'll carry over 
what you did to your next design since it worked so good for you last time. 
Some of the constraints you'll have are:

1.  Overall board thickness.  If you have any through hole components 
(connectors now a days can be about it but don't overlook it or you'll find 
some part where the leads won't go all the way through and won't get 
properly soldered).  .062, .093 and .125" are some common thicknesses that 
are driven by the lead length of 'typical' industry parts.

2. Available dielectric materials to use and their thicknesses.  Unless 
you're doing something exotic the material is likely FR4.  Check with PCB 
suppliers for some common thicknesses that they have and their line 
thickness/spacing constraints.

3. Balanced stackup.  Whether you work your way from top to bottom or bottom 
to top the layers that are power/ground planes need to be symmetrical. 
(i.e. Top, Plane, Plane, Bottom is the simple case for a 4 layer board).  As 
you work your way in, the thicknesses of the layers need to be symmetric as 
well.

4.  If every layer needs to have controlled impedance then adjacent to each 
and every signal layer must be a power/ground plane layer. Some examples: 10 
layers would be (Top, Plane, Sig, Sig, Plane, Plane, Sig, Sig, Plane, 
Bottom).  12 layers would be (Top, Plane, Sig, Sig, Plane, Sig, Sig, Plane, 
Sig, Sig, Plane, Bottom).  You'll find that you'll have some difficulty 
working out an 8 layer arrangement so if it has to be 8 you'll need to make 
some tradeoffs.

5.  Minimum required line and trace widths that you need to actually route 
the board.  Except for power or other high current nets you'll likely be 
better off making everything the same line width and be done with it (but 
again, different applications have their exceptions).

6.  Impedance control.  For digital applications 'many' times you don't so 
much care what the actual impedance is just that it doesn't vary from layer 
to layer since odds are you won't be able to route everything on one layer. 
If that's the situation then you may want to work out a target impedance to 
shoot for and a layer to layer difference that must be met.  As an example, 
maybe you spec that you want the impedance of each signal layer to be 55+/- 
5 ohms.  That allows the supplier a relatively wide window to shoot for. 
But you also want to constrain them so that you don't have Sig1 = 50 ohms, 
Sig2 = 60 ohms so you need to have an additional spec that says what the 
largest layer to layer impedance differential you're willing to tolerate 
will be (2 ohms maybe).  The supplier really won't have much trouble meeting 
this spec since it will likely require them to use the same material and 
thickness for most of the layers.  What will make it difficult is the actual 
impedance of a layer is important and you can't trade off either overall 
board thickness or trace width.  Working out the math to figure out a rough 
cut at the impedance and stackup ahead of time will help, if not work with 
the supplier and talk through what your requirements are and they can pop 
out a stackup for you in nothing flat since that's they're business.

The PCB supplier is generally keenly interested in nailing #1, 2 and 3 to 
minimize their cost and come up with something that they can fabricate 
economically so you can expect them to help you get those right.  #4, 5 and 
6 though generally don't impact their costs directly they really are 
constraints that they need to be able to meet so you need to be the one 
driving them to make sure that the stackup meets your product requirements 
in those areas.

KJ 

Thanks all for the advice. Regarding my stack I was planning to do this :-

Top
Gnd
Power
Mid1
Mid2
Power
Gnd
Bottom

Does the above seem sensible or would it be better to use 10 layers?

Cheers

Jon