[SI-LIST] Re: Designing PCB Stackups
- From: V S <for_si2003@xxxxxxxxx>
- To: codymiller@xxxxxxxxxx, si-list@xxxxxxxxxxxxx, Istvan Nagy <buenos@xxxxxxxxxxx>
- Date: Thu, 11 Dec 2008 11:23:15 -0800 (PST)
I agree. However, how can the impedance stay same when the thickness was
changed from 50um to 75 um. Obviously, the material used for the dielctric had
substantially different value. But that is a great lot of difference.I do not
expect the PCB house to change the trace thick, although they can and they so
sometimes.
That being said, I always specify the fab drawing with nominal values of the
thickness of the material and and assumed value of the dielectric constant. I
then let the PCB manufacturer give their own values. If the difference is not
great I usually approve. A difference like 50 um to 75 um is unusual. I usually
do not see that much of difference. If it is, it needs a closure look.
Vikas Shukla
http://referencedesigner.com
--- On Wed, 12/10/08, Istvan Nagy <buenos@xxxxxxxxxxx> wrote:
> From: Istvan Nagy <buenos@xxxxxxxxxxx>
> Subject: [SI-LIST] Re: Designing PCB Stackups
> To: codymiller@xxxxxxxxxx, si-list@xxxxxxxxxxxxx
> Date: Wednesday, December 10, 2008, 12:42 PM
> 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:
> > //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:
> > //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:
> //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:
> //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:
//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:
//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:
