From: [email protected]
Date: Wed Jun 06 2001 - 06:20:54 PDT
Shoaib,
I haven't done much pure RF design (mainly due to lack of time), but I
developed/helped develop the manufacturing test equipment for some 60 IBM
products from 1977 through 1990, and have been developing Local Area Network
(LAN) adapters and controllers for Lexmark OptraImage products since then. My
last three controller card designs have had 100MHz memory buses on them, so I am
thoroughly entangled in RF design whether I want to or not. (Which I do-- I
have some 1600 books on RF design, antennas, electromagnetic fields, high-speed
design, and related subjects in my personal library, and plan to do some serious
experimenting when I retire.)
I have seen a number of cards that started out with clear areas or traces
running under crystals and oscillators, that we had to re-lay out to put a solid
ground under them for at least the topside layer. The problems are three-fold:
1. Without a ground under crystals and oscillators, the parasitic capacitance
to traces and other components is very
sensitive to manufacturing variations such as:
* The relative dielectric constant of the raw card.
* The position of the crystal/oscillator with respect to its mounting
pads.
* The positions of components near the crystal/oscillator on both sides of
the card.
2. Signals on traces running near the crystal/oscillator can couple into the
input side of the oscillator, causing jitter.
3. The voltages/currents on the crystal/oscillator can couple into traces that
go to cables, causing Radiated
Emissions problems.
A solid ground layer right under a crystal/oscillator provides parasitic
capacitance that is controlled solely by the stand-off height of the
crystal/oscillator from the board. For metal-can pin-through-hole crystals that
will lay flat, I like to leave off the solder mask under the crystal. Then I
either use a 3-pin crystal with the case soldered to ground, or solder a
grounded wire strap across the crystal to hold the crystal's case tight against
the card, to:
* Provide mechanical support for the crystal.
* Ensure that all cards will have the crystal in the same location, within very
tight tolerances.
* Ground the case of the crystal, so that parasitic capacitances are due solely
to the internal constuction of the
crystal and not due to the "stuff" around it.
For surface mount crystals and oscillators, whose X-,Y-, and angular-position
may vary from board-to-board, having a solid ground right under the component
ensures that the parasitic capacitance will be essentially the same no matter
what the crystal/oscillator's exact position may be. This may only amount to a
few picofarads, but I believe it helps tighten the frequency tolerance from
board-to-board.
Finally, a solid ground plane directly under a crystal/oscillator will act as a
shield to prevent crosstalk between the crystal/oscillator and other traces.
If you look closely at an VHF/UHF/microwave board, you will usually see that it
is double-sided construction. The component side will be an almost-solid
groundplane around the component-mounting pads, while all the traces are on the
other side of the card. There are many other good reasons, such as controlling
transmission-line impedances, for doing it this way. But the ones that I have
mentioned above are among the major design criteria.
John Barnes KS4GL
Advisory Engineer
Lexmark International
This construction provides:
* A well-controlled (parasitic capacitance
will be tighter.
we will remove the solder mask right under the crystal and use a 3-pin crystal
(can soldered to ground) or sometimes a wire strap across the
We have used 3-pin metal-can crystals, or a wire strap across HC-49/U 2-pin
metal-can crystals, to ensure that the crystal is held tight
A solid ground under
the crystal/oscillator tends to swamp out these other factors, making the
stand-off height
David Bengtson <dbengtson%[email protected]> on 06/06/2001
06:19:27 AM
Please respond to David Bengtson <dbengtson%[email protected]>
To: "Shoaib" <shoaib%[email protected]>
cc: si-list%[email protected] (bcc: John
Barnes/Lex/Lexmark)
Subject: Re: [SI-LIST] : Copper pour beneath oscillators,
Putting on my RF engineering hat, I will say that copper pours over
the entire board are evil tools of the devil. You are increasing your
parasitic capacitance in an "uncontrolled" fashion.
Speaking for the oscillator, putting copper under it will increase the
parasitic capicitance, potentially coupling noise into and out of the
oscillator.
Dave
On Tue, 5 Jun 2001 10:23:39 +0500, you wrote:
>Hi,
> I'm a novice and my question might sound stupid but nontheless its a
question to me. I'm desiging a board with 20 Mhz clock oscillators on it, i have
put copper pour on the vacant areas of the board and connected the copper to the
ground (common to all components), this copper also extends beneath the
oscillators. The designer of the circuit is not happy with it and says that it
will inflict all the noise generated by other components onto the oscillators
output and rather he suggests that copper beneath the oscillators should remain
unconnected this way any noise inflicted on or by the oscillator will remain
isolated and not cause any problems. Can anyone please explain as it is a little
confusing for me.
> Thanx in advance,
> Shoaib
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
This archive was generated by hypermail 2b29 : Thu Jun 21 2001 - 10:12:16 PDT