[SI-LIST] Re: Designing PCB Stackups

hi

most of the people advices to not to specify exact material types, leave 
this decision for the production people, based on everyday actual pricing 
and stock info. this way its cheapest to manufacture, and the lead times are 
shortest. this is typical in the industry.

i dont advice this, because: crosstalk. if a production technician adjusts 
layer thicknesses (chosing a different material) they can make the original 
impedance values on the board, requested by the designer company, but the 
crosstalk levels will change. this is something what a PCB manufacturer and 
any of their employees can not understand, just a HW design engineer or a 
signal integrity engineer.
 we had a processorboard, where the manufacturer changed a dielectric layer 
from 50um to 75um, then the impedances were correct, but the crosstalk 
levels (simulated) increased by aroud 50%.
what i would do, is to chose a pcb manufacturer, send a rough stackup, ask 
if its ok for them or advice another stackup. then fix the materials, and 
use those forever for that board, in its lifetime. managers and purchasing 
people wouldnt like it, but thats the only way to have not just controleld 
impedance, but controlled crosstalk levels as well.
a common misunderstanding in the industry, is that a lot of people specify 
trace-to-trace clearances based on the trace width. (like d>2*w). it should 
be specified based on the dielectric thickness (like d>2*h). if you 
understand this, then its quite obvious why is it bad if the manufacturer 
specifies/changes the thicknesses during production.
the best is if you calculate the impedances (you need a good field solver, 
like Polar-si8000 or MMTL...), and check the resulting trace widths and 
dielectric thicknesses, to see if you can get good noise imunity and good 
circuit density on your board.
the first methos worked well 15 years ago when people had 2 controlled 
impedance traces on a PCB, and it was easy to maintain proper distance to 
other traces. if you check a DIMM memory module (you are from Micron, 
wright?), its full of controlled impedance traces, closely spaced because of 
the density.

regards,
Istvan Nagy
Concurrent Technologies Plc, UK


----- Original Message ----- 
From: <codymiller@xxxxxxxxxx>
To: <si-list@xxxxxxxxxxxxx>
Sent: Wednesday, December 10, 2008 2:08 PM
Subject: [SI-LIST] Designing PCB Stackups


> All,
>
> I have a general question regarding PCB stackup design. I am evaluating
> how we design our pcb stackups in our group now and I would like to put
> a procedure together or a set of rules of thumb to properly design a
> stackup. I would like the procedure to ask all the right questions up
> front.
>
> One question that came up is do PCB designers typically design with
> vendor specific materials in mind or do they design with generic prepreg
> and core materials. I see some pros and cons to both. What is typical in
> the industry.
>
> Any advice would be appreciated as well as if you know of any
> papers/resources on the web that could be helpful.
>
> Thanks,
> Cody
> ------------------------------------------------------------------
> 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:
> http://www.freelists.org/webpage/si-list
>
> For help:
> si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
>
> List technical documents are available at:
>                http://www.si-list.net
>
> List archives are viewable at:
> http://www.freelists.org/archives/si-list
> or at our remote archives:
> http://groups.yahoo.com/group/si-list/messages
> 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:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field


List technical documents are available at:
                http://www.si-list.net

List archives are viewable at:     
                http://www.freelists.org/archives/si-list
or at our remote archives:
                http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu

Other related posts: