RF Board PCB Layout - RF Cafe Forums
Post subject: RF Board PCB Layout
Mon Jun 07, 2004 4:06 pm
I am about to enter
into a PCB layout of RF board, which is basically an Up/Down Converter
that operates between 700-2000MHz.
I have few questions regarding
the PCB layout:
1) Supply voltage distribution:
I allocate voltage supply planes in an internal layer of the PCB
and connect these planes to the relevant components through plated
2) Use of via holes:
The componenet side
(Top layer) has GND plane (all the area which is not used for microstrip
traces), should I connect this GND plane to the internal GND plane
with plated via holes ONLY in the circumference of the board, or
in addition to these via holes should I also add via holes near
GND pins of RF components like Mixers, Couplers LC Filters etc?
The sensitive circuits are in the down conversion chain, should
I avoid routing the voltage planes beneath these circuits? Should
I use traces in the top layer to route the voltages to the components
of thes circuits?
Your inputs are highly appreciated.
- IR :)
Unread postPosted: Tue Jun 08, 2004 11:28 am
1) Do NOT use voltage supply planes. They are a great way
for providing leakage between circuits. The inductance of a series
meandering line (sometimes augmented with chokes) is your friend.
This inductance in conjunction with well placed decoupling caps
will decouple your circuits from each other.
are generally a bad idea. They will tend to produce a glitch in
the decoupling response. Instead use the largest cap you can get
2) Stitch the ground planes together with vias
at less than .3" spacing. You do not want significant runs of ground
plane not stitched.
Unread postPosted: Tue Jun 08, 2004 3:54 pm
thanks for the input, however I still have uncleared questions:
Do I need to put additional via holes near RF components beside
the stitching in the circumference of the board?
devices on the board are Gain Blocks, most manufacturers of these
kind of devices recommend to put a RFC (RF Choke) that will produce
reactance of few hundreds of ohms in the desired frequency band
(lowest frequency of course), bypassed with few values of decoupling
capacitors. You advised not to use several values of capacitors,
suppose I can live with that, but how should I connect these gain
blocks to the same voltage? I need to distribute the voltage to
them in some way and they are scattered all over the board...
Many thanks, I will be happy for more inputs.
Unread postPosted: Tue Jun 08, 2004 4:57 pm
Yes, you should
have at least one via very near each gnd of a component. I meant
to stitch vias based on a grid, not just around the edge.
The use of double caps would be OK if it weren’t for the small
amount of inductance between them (1 to 2nH). Check it out on a
simulator or try it in the lab.
The series inductors are
typically chained in series with a cap at the VCC pin of each device.
I generally do not recommend the star arrangement.
Post subject: Using a large single capacitor
Unread postPosted: Thu Jun 10, 2004 8:15 am
One person suggested
that using multiple caps is a bad idea. This person obviously lacks
experience in high frequency design. The biggest mistake that designers
make is to use one large capacitor for decoupling thinking that
it will de-couple all frequencies as long as it is large enough.
There is something call "ESR" in capacitors, it is a resonance frequency
where the capacitance is optimum. Below this point you are fine,
using a capacitor above this point and you mine as well put in an
inductor. Use multiple capacitors of various values , including
a large value, to de-couple across the entire frequency band.
Also, place a minimum of two ground vias as close to the termination
of any shunt component. Remember, that the RF ground is below and
vias connect to the RF ground. Vias also have inductance, the higher
the frequency, the higher the inductive reactance. Using more vias,
as close as possible will minimize this inductance.
Unread postPosted: Thu
Jun 10, 2004 12:08 pm
To the above post, I think you mean
SRF not ESR for the cap. All the post I have read hear have metrits
to certain applications.
The user must understand a component,
there are almost no general rules for PCB layout. Some components
are specifically used at their SRF.
If good RF work could
be summed up in a few rules, then I am out of a job.
Thu Jun 10, 2004 12:29 pm
I am the person that said that
double caps in decoupling networks are a bad idea. I will thank
you not to make comments about my experience, which exceeds 30 years.
Just sweep your double caps and you will find a parallel resonance
in the middle of it all. Try it you might learn something.
The last time I looked ESR was equivalent series resistance.
It is not a resonance. Caps do have a self-resonance. That is the
frequency above which the reactance is inductive.
Unread postPosted: Fri Jun
11, 2004 10:09 am
One person doubted that using multiple
caps is a bad idea. This person obviously lacks knowledge in fundamental
theory. The Foster’s theorem claims that the derivative of input
impedance is positive function for any reactive one-port circuit.
Which in turn means that between any two zeros there is pole, and
visa versa. By other words, any reactive one-port circuit which
has low input impedance at frequencies f1 and f2 inevitably has
high impedance in-between.
My two backs
Mon Jun 14, 2004 1:48 pm
Well said Oleg.
about the inverse. The inverse of decoupling is the coupling cap.
We don't see any one paralleling coupling caps because the zero
would be immediately apparent in a wide band circuit.
Post subject: PCB's for VHF/UHF
Unread postPosted: Wed Jun 16, 2004 3:09 am
IMHO, the use
of both power plane layers and decoupling capacitors is recommended
if it is a multi layer board design. Using simple traces as supply
lines will make them act as microstrip transmission lines. Also
the use of chokes must be verified as a choke together with a decoupling
capacitor will have a resonance somewhere in the spectrum. If this
resonance falls within a multiple of the operating frequency there
will be problems. If you plan to use a choke, make sure that the
Q of the decoupling network is low enough not to cause ringing effects.
Use power planes where possible but make sure
that the ground plane layer is SOLID! with absolutely no slots in
it and place the power plane underneath the GND layer. If the power
plane layer is properly designed, it will act as one very good chip
capacitor with exellent decoupling properties - but only if the
connection to the top (signal layer) is made using very short connections.
1 mm of trace or via is equivalent to 0.7-1 nH which may be enough
to impair the decoupling function.
Use minimum two via holes
per decoupling capacitor.
Use copper fills all over the top
layer, keeping a distance to the RF traces big enough not to make
the copper/trace forming a co-planar waveguide, since this will
result in changes to the caracteristic impedance of RF traces. Stitch
the area fills with via holes so there is no possibility that any
copper could act as a patch antenna.
The use of heat relief
tracks between decoupling capacitors and the copper fill requires
special attention. It is best to avoid this all together, but such
boards are often impossible to assemble due to the amount of heat
required during the soldering process.
Then it is easy enough
to specify one trace and work with this, but since the inductance
is 0.7~1nH/mm the series inductance will impair the decoupling seen
over a broad bandwith, so try to use minimum two trace s per capacitor.
Use decoupling capacitors with NP0 material for VHF/UHF if you
are using off the shelf components.
It is recommendable to
paralell a eg 1nF capacitor with a ~27-100pF for VHF/UHF use.
Sure, you can make use of the series resonance formed by the
capacitans and the internal inductans of the capacitors, but performance
change as manufacturers improve their processes. Never rely fully
on such effects although they may seem clever at first.
lower frewquency decoupling, use X5R or X7R material. Do not even
consider others as Y5V. Theese materials are voltage and heavily
temperature dependant. Some of the moderns high efficiency materials
also exhibit piezo electric effects and may actually generate noise
if the circuit board placed in a vibrating environment(!) We used
such capacitors in an EL high voltage driver and we could hear the
high voltage oscillator...
Unread postPosted: Wed Jun 16, 2004
I wish to thank you all guys for the useful advice.
I will take it all under consideration in the board layout.
- :-D IR
Unread postPosted: Wed Jun 16, 2004 3:32 pm
You have gotten a lot of different advice. I suggest Looking
at the swept responses AND nodal impedances of ANY candidate decoupling
approach before you commit the success of your design to it.
While the double cap is a poor idea, it does not significantly
hurt you most of the time due most decoupling networks being over
built. For RF, the VCC plane is another matter. Given significant
complexity and gain it will hurt you more often than not.
Post subject: Double Caps
postPosted: Fri Jun 18, 2004 12:14 pm
You are correct I
meant SRF although many vendors will only give you graph of ESR
versus frequency making it so you have to determine the SRF by finding
the lowest resistance. I did not have a problem with Tonys comments.
He said that double caps are OK as long as you are aware were the
resonances are. The problem I had was from the suggestion that double
caps are "bad" and use the biggest cap you can find. This may be
fine at lower frequencies but you will probably have a nice inductor
at the higher frequencies.
Post subject: Double Caps
Unread postPosted: Fri Jun 18, 2004
You are correct I meant SRF although many vendors
will only give you graph of ESR versus frequency making it so you
have to determine the SRF by finding the lowest resistance. I did
not have a problem with Tonys comments. He said that double caps
are OK as long as you are aware where the resonances are. The problem
I had was from the suggestion that double caps are "bad" and use
the biggest cap you can find. This may be fine at lower frequencies
but you will probably have a nice inductor at the higher frequencies.