Is there any other information available about this receiver?
Is it meant to produced commercially?

"Pete KE9OA" wrote in message
...
The MW receiver is progressing pretty well.................I have
completed
the synthesizer, and am now doing the final pass on the receiver board
itself. MDS measures at .2uV right now, with strong signal handling up to
about 900mV.
Next week, I plan to design the sync detector, but there are a couple of
things to keep in mind. If there are two closely spaced signals, the
stronger signal will capture the system. For this reason, I may also
include
the envelope detector function.
The initial results are very encouraging....................in the "RF
Alley" that I live in, with three 50kW MW broadcasters, no overload
problems
were noted. I will keep all of you posted on the progress of the design.

Pete

Is it going to be in kit form? )

Behold, Photodano1 signalled from keyed 4-1000A filament:

Is it going to be in kit form? )

That'd be sooo coooool! :-D

--
Gregg
*It's probably useful, even if it can't be SPICE'd*
http://geek.scorpiorising.ca

No, this will be an assembled unit.

Photodano1 wrote in message
...
Is it going to be in kit form? )

Pete KE9OA wrote:

The MW receiver is progressing pretty well.................I have completed
the synthesizer, and am now doing the final pass on the receiver board
itself. MDS measures at .2uV right now, with strong signal handling up to
about 900mV.
Next week, I plan to design the sync detector, but there are a couple of
things to keep in mind. If there are two closely spaced signals, the
stronger signal will capture the system. For this reason, I may also include
the envelope detector function.
The initial results are very encouraging....................in the "RF
Alley" that I live in, with three 50kW MW broadcasters, no overload problems
were noted. I will keep all of you posted on the progress of the design.

Pete

How are you designing the PC board(s) for this receiver? Do you use some
CAD software?


-----= Posted via Newsfeeds.Com, Uncensored Usenet News =-----
http://www.newsfeeds.com - The #1 Newsgroup Service in the World!
-----== Over 100,000 Newsgroups - 19 Different Servers! =-----

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.
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.
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.

Pete

starman wrote in message
...
Pete KE9OA wrote:

The MW receiver is progressing pretty well.................I have
completed
the synthesizer, and am now doing the final pass on the receiver board
itself. MDS measures at .2uV right now, with strong signal handling up
to
about 900mV.
Next week, I plan to design the sync detector, but there are a couple of
things to keep in mind. If there are two closely spaced signals, the
stronger signal will capture the system. For this reason, I may also
include
the envelope detector function.
The initial results are very encouraging....................in the "RF
Alley" that I live in, with three 50kW MW broadcasters, no overload
problems
were noted. I will keep all of you posted on the progress of the
design.

Pete

How are you designing the PC board(s) for this receiver? Do you use some
CAD software?


-----= Posted via Newsfeeds.Com, Uncensored Usenet News =-----
http://www.newsfeeds.com - The #1 Newsgroup Service in the World!
-----== Over 100,000 Newsgroups - 19 Different Servers! =-----

Pete KE9OA wrote:

starman wrote in message


How are you designing the PC board(s) for this receiver? Do you use some
CAD software?

I do 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.
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.
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.

Pete

That's really interesting. I've studied how Drake designed the PC boards
for their R8 series of receivers. I'm going experiment with the
grounding system to see how it affects the synthesizer noise which shows
up at certain frequencies, mostly in the higher HF range. It's much less
on the 'B' model than earlier versions but I think there's still room
for improvement.

Thanks for the reply.


-----= Posted via Newsfeeds.Com, Uncensored Usenet News =-----
http://www.newsfeeds.com - The #1 Newsgroup Service in the World!
-----== Over 100,000 Newsgroups - 19 Different Servers! =-----

Anytime! Anyway, it is a good idea to bring in the power supply return
(ground) wire to the noisest part of the circuit board; this way, the ground
is "cleaner", the further you get away from that section of the board. When
you are laying out the board, make sure that you locate the low level RF
circuitry as far away as possible from the noisy circuitry, and NEVER
connect the ground return wiring from the power supply to the low level RF
section of the board. If this is done, the return currents of the noisy
circuitry will flow through the ground plane in the low level section. This
noise will modulate the RF section, and be superimposed on the RF output,
possibly causing undesirable spurs, high phase noise in the VCO, etc.
A decoupling network applied in this scenario won't be effective, because
you will be bypassing to a noisy ground system.
Another approach to a quiet design is to implement the topology described
above, but to take it to another level, by breaking up the ground plane,
having the segmented planes connected either by a thin trace, an inductor,
or a ferrite bead.
It all begins at the board layout level.............once you realize that
you can control the DC and AC (RF) current flow on the board, it becomes
much easier to come up with a good 1st or 2nd pass design.

If you do have the power supply components on the same circuit board as the
rest of the circuitry, ALWAYS locate them in the area of the noisy circuitry

On another note.........I did some field testing on the MW receiver today.
Hooked up to a 75 foot antenna, no overload was noted on any of the 50kW
broadcasters in my area. I can tune 20kHz from WBBM 780, WGN 720, and WMAQ
670, and no desense is noted. Part of the secret here is to have your AGC
voltage detected after the final selectivity determining element. I've
noticed with both my Drake SPR-4 and my SW8, that when you are within 10kHz
of a strong station, the modulation sidebands from that station capture the
AGC system. It doesn't have to be this way. Once I get this receiver project
completed, I will look into a way of cleaning up those AGC loops. I do
notice that my TR7 does not exhibit this symptom, to I need to compare the
differences.

starman wrote in message
...
Pete KE9OA wrote:

starman wrote in message


How are you designing the PC board(s) for this receiver? Do you use
some
CAD software?

I do 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.
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.
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.

Pete

That's really interesting. I've studied how Drake designed the PC boards
for their R8 series of receivers. I'm going experiment with the
grounding system to see how it affects the synthesizer noise which shows
up at certain frequencies, mostly in the higher HF range. It's much less
on the 'B' model than earlier versions but I think there's still room
for improvement.

Thanks for the reply.


-----= Posted via Newsfeeds.Com, Uncensored Usenet News =-----
http://www.newsfeeds.com - The #1 Newsgroup Service in the World!
-----== Over 100,000 Newsgroups - 19 Different Servers! =-----

Pete,

When you get the time, take a look at the PC board layout of an R8B,
especially the top RF board. I guess the lowest board with the
synthesizer should be considered the noisiest one. It's located under
the chassis, apparently for shielding purposes. The SW8 is similar. I'm
going to revisit my R8B with your PC board grounding suggestions in
mind. Thanks again.

Pete KE9OA wrote:

Anytime! Anyway, it is a good idea to bring in the power supply return
(ground) wire to the noisest part of the circuit board; this way, the ground
is "cleaner", the further you get away from that section of the board. When
you are laying out the board, make sure that you locate the low level RF
circuitry as far away as possible from the noisy circuitry, and NEVER
connect the ground return wiring from the power supply to the low level RF
section of the board. If this is done, the return currents of the noisy
circuitry will flow through the ground plane in the low level section. This
noise will modulate the RF section, and be superimposed on the RF output,
possibly causing undesirable spurs, high phase noise in the VCO, etc.

snipped


-----= Posted via Newsfeeds.Com, Uncensored Usenet News =-----
http://www.newsfeeds.com - The #1 Newsgroup Service in the World!
-----== Over 100,000 Newsgroups - 19 Different Servers! =-----

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.

I¹m 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 don¹t 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 can¹t
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