Tim:

Dude, your math is like, sooo narley!

The driver absorbs 5/6, and the resistors absorbs the "remaining" 1/10 ?

Bogus!  ;-)

But seriously:
I haven't read what the authors said, so I can't comment on the validity of
it.

Best regards,
Ivan Baggett
Bagotronix Inc.
website:  www.bagotronix.com


----- Original Message -----
From: "Tim Hutcheson" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Monday, August 06, 2001 4:55 PM
Subject: Re: [PEDA] 5/5 Manufacturing Issues


> Actually I was thinking the authors meant that the driver absorbs about
5/6
> of the signal at frequency, while the resistor "absorbs" the remaining
1/10,
> at any frequency. Is that incorrect?
>
> Tim
>
> -----Original Message-----
> From: Bagotronix Tech Support [mailto:[EMAIL PROTECTED]]
> Sent: Monday, August 06, 2001 3:35 PM
> To: Protel EDA Forum
> Subject: Re: [PEDA] 5/5 Manufacturing Issues
>
>
> Tim:
>
> Keep in mind that only a resistor can "absorb".  A PCB trace cannot absorb
> anything.  If you really need a reflection absorbed at the source, you
> really need a resistor to absorb it.  Remember that when impedances are
> specified as one simple number (i.e. 50 ohm), that it is really the
> magnitude of the impedance.  That one simple number doesn't tell you about
> the complex (real +/- j*imaginary) impedance.  So a 50 ohm resistor is
> pretty much 50 + j0 ohms.  A 50 ohm trace is more like 0 + j50 ohms.  The
> difference is that the resistor can match impedances by absorbing
reflected
> energy (because of the real component of impedance), the trace cannot.
>
> Best regards,
> Ivan Baggett
> Bagotronix Inc.
> website:  www.bagotronix.com
>
>
> ----- Original Message -----
> From: "Tim Hutcheson" <[EMAIL PROTECTED]>
> To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> Sent: Monday, August 06, 2001 4:24 PM
> Subject: Re: [PEDA] 5/5 Manufacturing Issues
>
>
> > 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