MTI TN1014:
Stitch Vias
Stitch
vias (and via fences) are often used to tie ground planes and ground metal
pours to planes. The common rule of
thumb is to locate stitch vias no further apart than 
and preferably as
often as
.
There
are numerous reasons to use ground via stitching on a multilayer PCB. Some of the reasons are:
w
Prevention
of coupling into nearby traces and metal pour.
w
Prevention
of waveguide signal propagation, shielding/isolation of circuit blocks, and the
reduction of slot radiation from the edges of a PCB.
w
Completion
of a robust power distribution design. Reduction
of series inductance to active and passive parts. For more detailed info on PDN (power
distribution networks) in PCB, see [2].
w
Signal
integrity, in particular for signals that transition planes.
w
Thermal
reasons (not covered in this tech note).
Rules of
thumb are useful, but nothing beats analysis and a valid simulation for
support. Two analytical approaches are
illustrated and explained. This
technical note continues with an examination of stitch via usage, and a
rationale for selecting the distance/density of stitch vias.
First, a
key consideration; 
. This is the guided
wavelength. We know that the free space wavelength
of a sine wave is simply:
or 
but in a
dielectric, the wavelength is shorter, and must be multiplied by 
; the inverse of the square root of the dielectric
constant. The dielectric constant number
to use is obvious if we are interested in coax, or striplines, since the signal
conductor is buried in the dielectric.
For microstrip, a portion of the electric field is in air, and the
effective dielectric constant must be used [3], [4], [5]. For microstrip on FR4 type material (
), results in an 
. In this case, the guided wavelength
will be ~0.58 times the free space wavelength. The equations in [3] are one way to
approximate the effective dielectric constant, however, the best way to obtain
the actual effective dielectric constant for your particular application is by
using electromagnetic field solver analysis.
I have had
no trouble in finding guidance in reference books regarding stitch vias when it
came to inner planes and waveguide modes.
However, no luck in looking for a rationale for stitch vias to tie down
a metal ground pour near microstrip on the outer layers of a PCB. The approach I favor is based on coupled
microstrip.
Let’s
take a look at a simple example:
As we
know from coupled microstrip theory [6], the best coupling (our worst problems)
will occur when the coupled length is 
, 
, 
…
We use
an EM field solver to plot the reflections (S11) caused by the nearby ground
pour:
A
significant reflection is seen at 
, and the reflections are huge
at 
and 
. Obviously not a problem if your
signal is a 433MHz sine wave, but large reflections would certainly corrupt the
edges of a 1.25GHz (2.5 Gbit) rectangular signal.
Adding a
few stitch vias:
2 vias: 3
vias:
Again,
we analyze and plot the reflections on our microstrip:
In
short, vias placed every 
has the effect of reducing the
coupling at 
, and
eliminating problems up to 
. This would be OK for sine waves
at ,
but perhaps not quite sufficient for digital signals where we want to preserve
signal integrity. Recall that to preserve a digital signal’s edges, we
typically consider up to at least the 5th harmonic of the digital signal’s
fundamental frequency. Thus the
guideline to locate stitch vias no further apart than and preferably as
often as looks pretty good.
We are
also interested in using stitch vias to help us out with a PCB’s internal
power/ground planes.
We can
consider the parallel planes in a PCB as a rectangular resonant cavity with physical size of a x b x d, see [1]:
Pozar
notes that for b<a<d, the dominant resonant mode will be the TE101
mode. Since we do not normally
fabricate our PC boards with magnetic materials, μr = 1.
Side note: With regards to waveguide signal propagation
between two parallel conductive planes, there is some interesting current work
in making constructive use of this effect.
At this time, the key phrase is “Substrate Integrated Waveguide (SIW)”.
The
equation (all dimensions in meters) simplifies to:
For
example: FR4 like material (εr
~ 4)
Where
m,l = 1, 2 3… , and a,d are the width and length of the PCB in meters. In
many cases we can pretty much ignore the thickness (plane separation distance)
in the equations above.
The
following example considers a 6 inch by 10 inch FR4 board with a power plane
and ground plane. Using the equation
above, we find that the first four resonances are at 573.52MHz, 768.19MHz, and
1026.88MHz, and 1147.03MHz, followed by many more resonances above 1200MHz.
After
placing a stripline port on either side of the plane pair (see the following
page). Shorting each of the striplines
to the ground plane, we can evaluate the
coupling between the short lines on either end of the board:
Note: The magnitude of each resonance is heavily
influenced by our coupling into the waveguide.
As expected, our very short shorted striplines do not couple well at low
frequencies. We can also take a look at the current density in one of
the power planes as seen in the following page.
At
573MHz:
At
1147MHz:
We can
perform a simple experiment by placing a single sparse via fence across the width
of the board. The vias are spaced about
0.5 inch apart:
Simulating
the structure shows that the coupling is reduced by about 40dB:
We can
do much better at lower frequencies with a stitch via field. The field has stitch vias on roughly 1 inch
centers between the two planes:
The
density of stitch vias, and their location depends entirely on what is critical
in your application (for example: shielding, isolation, signal or PDN quality,. As usual, an analysis of the system
requirements as well as possible coupling is highly recommended. Given available resources, it is to our
advantage to support the analysis with field solver simulations, then follow up
with measurements on a test board or with appropriate tests on the first
fabricated boards (sneaking in engineering measurement capability is a
time-honored tradition).
References:
[1]
David M. Pozar. Microwave Engineering, 2nd Edition.
[2] Istvan Novak and Jason Miller, Frequency Domain Characterization of Power
Distribution Networks.
[3] E. Hammerstad and O. Jensen, “Accurate
Models for Microstrip Computer-Aided Design,” Microwave Symposium Digest, 1980 MTT-S International, pp407-409
[4]
Manfred Kirschning and Rolf Jansen, “Accurate Wide-Range Design Equations for
the Frequency Dependent Characteristic of Parallel Coupled Microstrip Lines,” IEEE Transactions
on Microwave Theory and Techniques, Vol. MTT-32, No 1, pp83-90, Jan. 1984.
[5] Hong
and Lancaster. Microstrip Filters for RF/Microwave Applications.
[6]
Mongia, Bahl and Bhartia. RF and Microwave Coupled-Line Circuits..