In article
,
"Pete KE9OA" wrote:
I so use a CAD program. For the prototyping, I print out the artwork
on an Inkjet transparency, and use boards that have a photosensitized
resist. Our jobber wants 250 dollars for each prototype run, so it is
cheaper for me to do it myself. Once I get everything designed, we
will go to our board house, and have some real boards made up. It is
quite a bit of work, spotfacing all of the holes on the ground plane,
and soldering feedthrough wires, to connect the top ground plane to
the copper flood on the bottom side of the board, but it is the only
way to get a board with a nice low impedance RF ground. Another
interesting thing.................it is a good idea not to lay down
your ground vias on a fixed grid; instead, drop them around the board
in a pseudo-random fashion. This way, you can minimize the chances of
having resonances in the structure. I remember one project that I was
working on a few years back. The designer decided to lay down all of
the ground vias on a 50 mil grid. This was a 900MHz hybrid
synthesizer, that used a mixing scheme to translate the tuning range.
Anyway, the board had a very sharp resonant peak right in the middle
of the image band. The engineer that I was working with didn't
believe that this was the case, until we started drilling out the
vias with a Dremel tool.
This sounds to me like the problem resonance was just moved to a
different frequency by removing vias. The solution should have been to
add more ground vias.
Iım assuming the situation you are painting is a continuous ground
plane on the bottom with circuit features on the top of the board with
additional ground plane ³flood² on the top in a bid to provide more
isolation between circuit paths or just improving ground on the board.
To get patches of ground plane on the top of the board to behave the
same electrically as ground plane on the bottom the impedance must
remain low relative to the frequency of operation. To accomplish this a
number of vias must connect the patches or areas of ground plane on top
to the continuous ground plane on the bottom. The rule of thumb I use
is a 1/4 wave of the highest frequency of operation. The reason for the
1/4 wave is this is the minimum feature size that is likely to resonate
inadvertently in the design so for 900 MHz that would be about ~ 278 ps
for a 1/4 wave and at ~ 145 ps an inch for a FR4 type dielectric that
would be ~ 1.9 inches to propagate on the board. You donıt want any
ground plane features on the board top to be any longer than 1.9 inches
without a via to the ground plane below.
For example lets say you pick a via spacing of 1 inch to be safe and
you have two circuit traces going two a mixer on the board. These two
traces start several inches apart on the board and gradually come to
about .5 inches of each other as they approach the mixer. If you put
ground plane between them it will look like a finger pointed at the
mixer and with 1-inch regular grid placement of the vias none might
have connected this finger to the ground plane below. This finger can
then behave as a 1/4-wave stub if it is 1.9 inches long. This can be
fixed by adding (at least) one via at the end of the finger to the
ground plane below lowering the impedance next to the mixer so it canıt
move electrically.
A good way to check a PC board for undesired resonances is to take
the unpopulated board, and connect an SMA launch at each end of the
board (input and output). Connect a network analyzer, and you should
see a flat noise spectrum, if the board was properly designed.
I never thought of doing this. Thanks for the idea.
Another trick of the trade for checking VCOs is to connect a network
analyzer to the inpur of the VCO. Set up the analyzer for a Smith
Chart type of display. You will know if you have your feedback
capacitors optimized for the tuning range of interest, if you are
centered in the maximum magnitude region of negative resistance. This
was a pretty common technique at Rockwell. When I mentioned this to
the folks that I was working with in my department at Motorola, they
had never heard of this method.
I think I understand what you are describing here but I need more detail
to be sure.
--
Telamon
Ventura, California
|