[SI-LIST] Re: Designing PCB Stackups
- From: "Bill Stube" <Bill.Stube@xxxxxxxxxx>
- To: <si-list@xxxxxxxxxxxxx>
- Date: Mon, 15 Dec 2008 16:00:22 -0600
In my experience, each fabricator has sufficient variation in their
process that a different fabricator will give different plating
thicknesses, final trace widths, dielectric thicknesses, impedance, etc,
even if you specify the same material. There are also lot to lot
material variations to consider. If possible, it is nice to pick one
fabricator and stick with them through your prototypes, verification
testing, and production but this will not solve all of your problems.
If you plan to move to a "low cost" fabricator, do so as early in your
design process as practical.
While specifying the material helps you to limit your variables, I think
the best approach is to do the following.
1.) Design a stackup based on your design requirements and work with
multiple PCB fabricators to ensure you aren't designing yourself into a
corner. You can also quote these vendors early on to make your
purchasing folks happy.
2.) Simulate your design or system across process corners which are
realistic for your design. Fast/Slow model corners as well as high/low
impedance or relevant PCB parameters.
3.) As simulations require, force tighter requirements onto your PCB
layout, materials, or fabricator.
4.) Close the loop on your simulations by analyzing your boards when
they come back for the same parameters you simulated.
Working with multiple vendors or your target vendor early on as well as
thoroughly simulating your design will help to give you a functional
board as well as an acceptable manufacturing yield. If you company is
willing to pay for it, you could request your vendor fabricates two or
three separate lots at your PCB corners. This would give you a good
sample set for testing of your PCB corners.
Bill Stube
Hardware Engineer II - Digital Systems
Plexus Technology Group
http://www.plexus.com/
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
On Behalf Of V S
Sent: Thursday, December 11, 2008 12:23 PM
To: codymiller@xxxxxxxxxx; si-list@xxxxxxxxxxxxx; Istvan Nagy
Subject: [SI-LIST] Re: Designing PCB Stackups
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
------------------------------------------------------------------
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:
