ATTN: RF PCB-LAYOUT DESIGN ENGINEERS, I need some help!

[ZenSafari]

Hello--
I am currently constructing a miniaturized spectrum analysis unit and
am having some troubles with my local oscillator sources. The problem
is that my VCO output (in a PLL) is rife with noise...not only phase
noise but broadband noise upto about 3GHz. I need to stabalize my LO
sources so that when I drive my mixers I am not injecting additional
frequencies into the mixer.

For those of you with RF PCB layout experience, can you give me some
hints as to how to best layout a PCB for the LO source? I have
separated my digital and analog ground planes (digital ground for
Analog Devices PLL synth chip) but on my prototype PCB I realized today
that some of my analog ground overlaps the digital gournd on a
different layer...oops. anyways, for those of you with extensive
epxerience in this area, i could sure use your help as to how to get my
LO source outputs to remain spectrally pure.

If I am unclear, please let me know and I can clarify further.

Thanks in advance,
Chris

 

[Joerg]

Hello Chris,

... I have
separated my digital and analog ground planes (digital ground for
Analog Devices PLL synth chip) but on my prototype PCB I realized today
that some of my analog ground overlaps the digital gournd on a
different layer...oops. ...

That may be your problem right there. In my experience splitting grounds
has never really worked. Definitely not in circuits that must operate
above the audio band and it seems you are quite a few orders of
magnitude above.

Try to tie them together. But not with any wires, it needs to be
multiple connections with next to nothing in inductance. IOW copper tape
and stuff like that. Watch you fingers to avoid those nasty copper tape
cuts.

Regards, Joerg

 

[John Larkin]

Hello Chris,


That may be your problem right there. In my experience splitting grounds
has never really worked.
Right.


Definitely not in circuits that must operate
above the audio band and it seems you are quite a few orders of
magnitude above.

Try to tie them together.

Or use just one solid ground plane.

John

 

[Joerg]

Hello John,

Or use just one solid ground plane.

Yes, that's what I meant. Considering the time it takes to have another
stuffed PCB in hand it is often worth to try to connect split planes in
as many locations as possible, to somewhat mimic a solid plane. It'll
look ugly but you can go on debugging. In parallel I'd order a board
with a solid plane.

Did you swap out those BAV99 for BAT54?

Regards, Joerg

 

[John Larkin]

Hello John,

Yes, that's what I meant. Considering the time it takes to have another
stuffed PCB in hand it is often worth to try to connect split planes in
as many locations as possible, to somewhat mimic a solid plane. It'll
look ugly but you can go on debugging. In parallel I'd order a board
with a solid plane.

Did you swap out those BAV99 for BAT54?

Nope. The BAVs seem to be working fine (this is the +-18 volt floating
power supply, 16 on a board, now running a "soft" square wave at 45
KHz.) No sign of reverse-recovery snaps. One minor screwup is that
even a little ripple at 45KHz shoots right through the output opamps
(psrr sucks at 45K!) so next rev we'll use an r-c-r-c power supply
filter to zap the ripple harder. But the board (16 isolated analog
voltage/thermocouple-simulation outputs, 4 ref junction RTDs, uP, 2
big FPGAs, 12K lines of code) works first-try as designed... just a
few value tweaks, not a single kluge!

It's our first project with the new guy I designed it with, and I met
him on this very ng! I knew there was a reason to waste so much time
here.

John

 

[Joerg]

Hello John,

Nope. The BAVs seem to be working fine (this is the +-18 volt floating
power supply, 16 on a board, now running a "soft" square wave at 45
KHz.) No sign of reverse-recovery snaps. One minor screwup is that
even a little ripple at 45KHz shoots right through the output opamps
(psrr sucks at 45K!) so next rev we'll use an r-c-r-c power supply
filter to zap the ripple harder. But the board (16 isolated analog
voltage/thermocouple-simulation outputs, 4 ref junction RTDs, uP, 2
big FPGAs, 12K lines of code) works first-try as designed... just a
few value tweaks, not a single kluge!

Cool. What I found on isolated power supplies was that the ESR of the
filter caps after the diodes begins to matter. For the very same reason,
PSRR. At 60Hz the PSRR would take care of things but not at tens of kHz.

On pulse echo systems I have it easier than you did. I can synchronize
the soft square wave to the pulse repetition rate and none of the ripple
shows up. But the transformers have to be pretty wideband for that,
usually 10:1.

It's our first project with the new guy I designed it with, and I met
him on this very ng! I knew there was a reason to waste so much time
here.

That is great. I bet that 80% or more of all engineers do not even know
that usenet exists.

Regards, Joerg

 

[ZenSafari]

I do, in fact, have the ground planes tied together at one point via a
strip of copper. I'm not sure that using one ground plane will help as
I'm afraid that any of the higher-frequency RF components (3GHz to 4GHz
) may couple into the ground plane and radiate throughout my PCB
causing the output of my LO source to be rife with spurs. I'm wondering
if my problem lies in the overlapping of the analog and digital
grounds; there may be some parasitic capacitance playing in here...it
is, afterall, a 4-layer board.

 

[Joerg]

Hello Chris,

I do, in fact, have the ground planes tied together at one point via a
strip of copper. ...

That ain't enough. Try it in more than one place, lots more.

... I'm not sure that using one ground plane will help as
I'm afraid that any of the higher-frequency RF components (3GHz to 4GHz
) may couple into the ground plane and radiate throughout my PCB
causing the output of my LO source to be rife with spurs. I'm wondering
if my problem lies in the overlapping of the analog and digital
grounds; there may be some parasitic capacitance playing in here...it
is, afterall, a 4-layer board.

It could be. Two planes connected in one place may form a pretty good
dipole antenna which can pick up and radiate. And you don't want
antennas in your board. That is one reason why a common plane is usually
better.

Regards, Joerg

 

[Rene Tschaggelar]

Hello--
I am currently constructing a miniaturized spectrum analysis unit and
am having some troubles with my local oscillator sources. The problem
is that my VCO output (in a PLL) is rife with noise...not only phase
noise but broadband noise upto about 3GHz. I need to stabalize my LO
sources so that when I drive my mixers I am not injecting additional
frequencies into the mixer.

For those of you with RF PCB layout experience, can you give me some
hints as to how to best layout a PCB for the LO source? I have
separated my digital and analog ground planes (digital ground for
Analog Devices PLL synth chip) but on my prototype PCB I realized today
that some of my analog ground overlaps the digital gournd on a
different layer...oops. anyways, for those of you with extensive
epxerience in this area, i could sure use your help as to how to get my
LO source outputs to remain spectrally pure.

If I am unclear, please let me know and I can clarify further.

I'd put the RF stuff in a box and have the controlling
wires though the wall with T filters. You can also put
the lot into a box and separate the sections with
internal walls.

Rene

 

[ZenSafari]

Rene--
Yes, you are right...I would do a lot better if I isolated the RF
components. The problem is, however, I do not have that luxury for this
system. Everything pretty much has to be on one PCB. In fact, I've
noticed that some of the copper traces on my board are radiating. Most
of this radiation is from signals in the 6GHz range and above...turns
out that the mixers I am using produce very strong 2nd and 3rd order
harmonic terms and these high-frequency harmonics are radiating on my
short copper traces. Does anyone out there have some experience doing
PCB layouts for telecom industry? CDMA/GSM standards...etc.? I fee like
PCB layout gurus would run into the same problem as I am having when
making these devices seeing as how components inside cellular phones
these days are jam-packed.

Thanks again for the posts. Any help is greatly appreciated.

 

[Joerg]

Hello Chris,

... Does anyone out there have some experience doing
PCB layouts for telecom industry? CDMA/GSM standards...etc.? I fee like
PCB layout gurus would run into the same problem as I am having when
making these devices seeing as how components inside cellular phones
these days are jam-packed.

You have to strictly adhere to trace impedance rules or your traces will
sing. The minute your trace impedance varies or a trace isn't terminated
with its characteristic impedance at least at one end it starts to
radiate. Refer to an older ECL data book with trace impedance calcs or
use an electronic cheat sheet like this one:
http://www.emclab.umr.edu/pcbtlc2/index.html

Also, avoid sharp 90 degree bends because that will disturb impedance.
At 6GHz this kind of stuff really matters.

If you do layouts out of house you need a very exprienced RF layouter or
you have to coach pretty much through the whole session. I am lucky that
I have a good layouter 1/2 hour's drive from here. Don't know about 6GHz
stuff but he did all my RF boards intuitively right with very little
input from me.

Regards, Joerg

 

[Meindert Sprang]

Rene--
Yes, you are right...I would do a lot better if I isolated the RF
components. The problem is, however, I do not have that luxury for this
system. Everything pretty much has to be on one PCB. In fact, I've
noticed that some of the copper traces on my board are radiating. Most
of this radiation is from signals in the 6GHz range and above...turns
out that the mixers I am using produce very strong 2nd and 3rd order
harmonic terms and these high-frequency harmonics are radiating on my
short copper traces. Does anyone out there have some experience doing
PCB layouts for telecom industry? CDMA/GSM standards...etc.? I fee like
PCB layout gurus would run into the same problem as I am having when
making these devices seeing as how components inside cellular phones
these days are jam-packed.

Having just separate ground planes is not sufficient. A PCB can act as a
waveguide at high frequencies, so you have to block the path *inside* the
PCB. Open a cell phone and you'll see how it is done: a ground trace around
a circuit on one side and closely spaced vias from this ground trace to the
ground plane on the other side. This creates a faraday cage inside the PCB.

Meindert

 

[ZenSafari]

Having just separate ground planes is not sufficient. A PCB can act as a

waveguide at high frequencies, so you have to block the path *inside* the
PCB. Open a cell phone and you'll see how it is done: a ground trace around
a circuit on one side and closely spaced vias from this ground trace to the
ground plane on the other side. This creates a faraday cage inside the PCB.

Meindert

Wow, thanks for all of the great advice you guys have offered me. I
have two questions, still.

1) I figured that even if my PCB traces were not 50ohm traces that I
would avoid transmission line effects if I kept the traces very short
(relative to the wavelength, of course). 50ohm lines on FR4 are
something like 62mils wide...too wide for me to work with. I suppose
what is happening is that my PCB traces, although short, look like
quarter-wave antennas to the high-frequency harmonics (6GHz and above)
that "live" on my board. Is there ANY way around this? How do I get rid
of these nasty harmonics? Attaining 50dB of isolation on a PCB seems
ridiculous to me unless I start enclosing the critical parts in Faraday
cages and use hard-pipe to connect filter components. Do i have ANY
other options at all?

2) Meindert - Thanks for the cell phone advice. I will pop one open as
soon as I can. I guess I'm wondering: Do the cell phone guys isolate
the VCO from the PLL or is it all done on one circuit board? The idea
of creating a Faraday cage on the PCB is very interesting to me...

It seems to me that RF circuit design is a bit of a black-magic art
form. I'm very green when it comes to doing RF circuit layouts so this
is probably why I'm running into so many issues. Again, thanks for all
of the handy advice, I will surely put it to good use.

-Chris

 

[Joerg]

Hello Chris,

1) I figured that even if my PCB traces were not 50ohm traces that I
would avoid transmission line effects if I kept the traces very short
(relative to the wavelength, of course). 50ohm lines on FR4 are
something like 62mils wide...too wide for me to work with. I suppose
what is happening is that my PCB traces, although short, look like
quarter-wave antennas to the high-frequency harmonics (6GHz and above)
that "live" on my board. Is there ANY way around this? How do I get rid
of these nasty harmonics? Attaining 50dB of isolation on a PCB seems
ridiculous to me unless I start enclosing the critical parts in Faraday
cages and use hard-pipe to connect filter components. Do i have ANY
other options at all?

Short of reducing the FR4 thickness between trace and ground plane it's
going to be difficult. You could try a little loop at the device that
you suspect generates harmonics, kind of a poor man's low pass.

It seems to me that RF circuit design is a bit of a black-magic art
form. I'm very green when it comes to doing RF circuit layouts so this
is probably why I'm running into so many issues. Again, thanks for all
of the handy advice, I will surely put it to good use.

It is black magic. That's why you really need this book: Johnson, Graham
"High Speed Digital Design - A Handbook of Black Magic". Seriously,
that's its title. Pretty much a must on the desk of anyone doing
circuits like you are designing.

Regards, Joerg