High Frequency Measurements
Douglas C. Smith
Address: P. O. Box 1457, Los Gatos,
Technical Tidbit - May 2003
Signal Paths Passing Through Ground and Power Planes, Effects on Immunity
Figure 1. Test Setup to Measure Immunity of a Test Board
Abstract: In 4 layer printed wiring boards, practical layouts require
paths to cross from the top signal layer to the bottom signal layer. Paths
that exist on both the top and bottom signal layers affect the emissions
and immunity characteristics of a circuit board. Results from a test of radiated
EMI are presented and discussed.
Discussion: Data was taken using the test setup shown in Figure 1.
A Fischer Custom Communications pulsed field generator
was used to generate fast impulse fields. This pulse generator is designed
to simulate a kind of pulsed field generated by ESD between small pieces
of metal at low voltages, a potent source of EMI. The generator was positioned
30 cm from a test board. The test board was constructed from a double sided
copper clad board with approximately 50 Ohm paths placed on the planes. Two
30 cm test paths were used. One was routed from an SMA connector to a 47
Ohm resistor over a continuos copper plane. The other 30 cm path was over
the same copper plane for 2/3 of its length and passed through the board
and was routed over the copper plane on the other side of the board for about
1/3 of its length. The two copper planes simulate the power and ground planes
of a 4 layer printed wiring board. The planes were shorted together at the
SMA connectors and at the loads, a total of 4 locations.
The paths were connected, one at a time, to an oscilloscope to measure the
EMI induced in each path. RG-142B/U high quality coaxial cable
was used to insure the interference measured was on the circuit board and
not due to the shield transfer impedance (essentially leakage through the
shield) of the coax cable.
Figure 2 shows the voltage induced in the path that penetrated the copper
planes. A peak voltage of over 200 mV was recorded along with a ringing frequency
between 400 and 500 MHz. The amplitude of the induced noise is a substantial
fraction of the noise margin for some of today's fast logic. Potentially such a waveform could disrupt sensitive circuits..
Noise Induced into Path That Passed Through the Planes
Figure 3 shows the induced voltage in the path that was
routed over a solid copper plane. The amplitude reached a peak of about 100
mV with very little ringing. Such a noise would have a lower risk of signal
corruption compared to that in Figure 2.
Noise Induced into Path Routed Over a Solid Plane
One way to think of the increased EMI in Figure 2 is
that the inter-plane impedance between the copper planes can develop a voltage
in response to the radiated EMI. This voltage is in series with the return
path of the signal line as the line crosses from being over the bottom plane
to the top plane. If the path stays over a solid plane, there is no opportunity
for this to happen. For board stack-ups with closer power-ground plane spacing,
the effect would be proportionally smaller, yielding lower observed EMI amplitudes
than shown here.
Another similar experiment is described in the paper "ESD Immunity in System Designs, System Field
Experiences and Effects of PWB Layout "(~950K)
where an IEC 61000-4-2 ESD generator is discharged to the same board at 3
kV (about the human level of threshold of feeling an ESD event). The path
that dives through the planes receives over 2 Volts of interference whereas
the path that stays over a single plane receives only about 300 mV of interference.
This is a greater difference than noted above, possibly due to the increased
energy at lower frequencies in the hand metal ESD waveform of the IEC generator
compared to the radiated field from small metal ESD. The lower frequency
energy would more closely match resonances in this board. Since currents
were injected directly on the board in the paper, different coupling mechanisms
are possible as well..
As one might expect, emissions from the two paths are different as well.
Data presented in my seminars show that the diving path has significantly
higher emissions, as much as 30 dB, than the straight path at several frequencies.
A similar experiment to this one, for paths crossing a break in a ground
plane, was described in the February 2003, Technical Tidbit
on this site. The effect of crossing a break in a ground plane is stronger
than passing through planes as evidenced in the data in that article.
Conclusion: The data shows that passing through copper planes
on a circuit board can lead to lowered immunity to radiated and conducted EMI. In general,
any board feature that disrupts the signal return path in a plane, will cause
lowered immunity to external EMI.
The data in the waveforms above was taken with an Agilent
Infinium 54845a oscilloscope.
Shorting the edges of the planes together (directly or through bypass
capacitors) and other techniques are discussed, and shown as experiments, in
my seminars. These techniques can reduce the amount of EMI induced in board
features such as diving through multiple ground or power planes.
Top of page
Questions or suggestions? Contact me at email@example.com
Copyright © 2003 Douglas C. Smith