Thanks Mike but I'm just going by what I read.  For example, Brian Young in
"Digital Signal Integrity" says " In contrast to parallel termination at the
load, source termination allows the signal to reflect off the load and
travel back to the source, where is absorbed by series termination. The
series termination can be implemented as either the output impedance of the
driver or as a resistor in series with the driver, in which case the driver
must have an output impedance lower than the characteristic impedance to the
transmission line.  The resistor can be implemented within the driver
itself, where it is often referred to as ballast, or it can be implemented
externally on the PCB".  pp 400.

The above is consistent with what I read elsewhere, as in the Hall, Hall and
McHall book on transmission line theory, High-Speed Digital System Design: A
Handbook of Interconnect Theory and Design Practices.

So my manufactures reference design has a characteristic impedance of 63
ohms, with a 10 ohm series resistor roughly creating a match for the 50-ohm
driver.  I used this fact to validate my understanding of the above
paragraph though I certainly don't have enough experience with this to be
sure.  Hence my question.

The board is 4-layer with each signal layer referenced to a plane.

Thanks for the +/- 10 percent data, that will be helpful in deciding about
the actual material to use.


regards,
Tim Hutcheson
[EMAIL PROTECTED]




> -----Original Message-----
> From: Mike Reagan [mailto:[EMAIL PROTECTED]]
> Sent: Monday, August 06, 2001 3:05 PM
> To: Protel EDA Forum
> Subject: Re: [PEDA] 5/5 Manufacturing Issues
>
>
>
> > > I have discovered that I might be able to remove about 200 source
> resistors
> > > from my 5/5 mil design if I can manufacture with exact
> impedance match a
> > > 4-layer FR4 board.
>
> Tim,
> I have to respond to your concerns and about controlled
> impedance. First of
> all if the resistors you are claiming to eliminate are located at
> the source
> as is a commmon practice,   These resistors are not  in the circuit for
> impedance purposes.  I will stay away from all the math, but the resistors
> are in the circuit to increase the R value of  the first time
> constant which
> directly effects the risetime of the pulse. By slowing the leading edge of
> the pulse you reduce much higher frequencies inhereent to  the fundamental
> 133 MHZ.
>
> Second in order to gain "controlled impedance"  every layer must be
> referenced to a plane layer. For internal layers that means signal layers
> must be sandwiched between (read non split) planes.
>
> And last, even the best materials will yeild +/- 10 percent of your target
> impedance.   Variations in thickness of the pregreg and epoxies
> will ocurre
> with any material  you choose.  The purpose of choosing a high speed
> laminate is to reduce losses caused by absorbtion.   Controlled impedance
> can be achieved on cardboard, if you understand the properties
> well enough.
>
> I would not attempt to elimante your 200 resistors, they are in
> your circuit
> to reduce the leading edge risetime not a controlled impedance matching.
>
> Mike Reagan
> EDSI
> Frederick Md
>
>
>
>
>
>  It seems that laminates down to about 2.5 mil are
> > > available but conventional wisdom is to not go below 4 mil and
> preferably
> > > stay at 5 mil.  I would need to use about 3.5 mil of FR4
> material to try
> to
> > > get a 50-ohm impedance match with my processor.  The question
> is whether
> or
> > > not films are available in such precise thick nesses and are
> the results
> > > reproducible enough.  I would expect that the first prototypes would
> give me
> > > my baseline and I would go from there but only if the process is
> repeatable.
> > > Any thoughts by anyone would be appreciated.  I have committed all of
> the
> > > calculations to my calc and verified them with numerous examples so I
> would
> > > be able to verify any suggestions quickly, in so far as calculations
> go...
> > > ;-)  My design is for 66/100/133 mhz operation.
> > >
> > >
> >
> > I do some RF design though I wouldn't really claim to be an RF engineer.
> All
> > the info I have seen and heard says that FR-4 is not a good bet for
> tightly
> > controlled impedances - too much variation in thickness, dielectric
> constant,
> > etc. You may need to switch to PTFE or some of the newer Rogers
> materials
> for
> > the board. Depending on your assembly costs, etc., the more expensive
> board
> > material might still be more cost-effective overall, and you'll get more
> > repeatable designs. But I'm not so sure you can really
> eliminate that many
> > parts - I'm having trouble visualizing a design where the use of
> > controlled-impedance traces would eliminate the need for termination
> > resistors. The input pins where the lines terminate are still
> high-impedance,
> > and require some sort of termination to avoid reflections. On the other
> hand,
> > from my perspective 133 MHz is practically DC anyway, so you might get
> away
> > without them - but I wouldn't necessarily bet a board turn on that!
> >
> > Steve Hendrix
> >

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to