Maker Pro
Maker Pro

How to reduce radiated emissions

Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????
 
E

Eeyore

Jan 1, 1970
0
Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????

PCB redesign.

Graham
 
M

martin griffith

Jan 1, 1970
0
On 29 Mar 2007 02:27:34 -0700, in sci.electronics.design
Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????
as Eeyore said, pcb redesign, but check out Page 54 in AN70 from
linear.com, for how to determine what part of the PCB needs attention


martin
 
A

Ancient_Hacker

Jan 1, 1970
0
Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????

There's no panacea-- EMi can spin off in many ways, and some EMi
reduction methods actually increase EMI squirting out in other ways or
frequencies.

One way is to get a braod-band spectrum analyzer, put a tiny one-cm
loop on the end of the coax cable, and probe around for places that
generate a peak. Then tackle each peak one at a time, adding ferrite
beads, bypass caps, or simple series resistors AS CLOSE AS POSSIBLE to
the active elements. I mean like millimeters. You have to take EMI
problems slowly, scientifically, deliberately, quantitatively, and one
peak at a time.

As other have noted, to really do it right, one often has to redesign
the lead lengths, bypass cap locations, and ground planes.

Don't fret too much, many places eventually have to call in an EMI
consultant, or send the box off to a special EMI measurement and
abatement place. We have one here in Mn, conveniently placed in a EMI-
quiet cave, in a quiet valley.
 
There's no panacea-- EMi can spin off in many ways, and some EMi
reduction methods actually increase EMI squirting out in other ways or
frequencies.

One way is to get a braod-band spectrum analyzer, put a tiny one-cm
loop on the end of the coax cable, and probe around for places that
generate a peak. Then tackle each peak one at a time, adding ferrite
beads, bypass caps, or simple series resistors AS CLOSE AS POSSIBLE to
the active elements. I mean like millimeters. You have to take EMI
problems slowly, scientifically, deliberately, quantitatively, and one
peak at a time.

As other have noted, to really do it right, one often has to redesign
the lead lengths, bypass cap locations, and ground planes.

Don't fret too much, many places eventually have to call in an EMI
consultant, or send the box off to a special EMI measurement and
abatement place. We have one here in Mn, conveniently placed in a EMI-
quiet cave, in a quiet valley.

Been there, done that. Ancient Hacker is right.

One thing that helped me a lot when I was younger was switching from
double-sided (two layer) printed circuit boards to four layer boards
where the two inner layers were devoted to a ground plane and a single
power plane. Where the two layer board had been barely good enough
when fitted with a grounded screen plate, the four layer boards
performed better, even without the screening plate. The are lots of
other tricks that can reduce emissions and the sensitivity to incoming
electromagnetic radiation, mostly involved reducing the dimensions of
the transmitting and receiving loops, and finding them involves the
slow systematic search that Ancient Hacker talks about.

Of course, once you have found a few transmitting and receiving loops,
you do start to get a better feels for low-EMC circuit layout and
construction.
 
A

Ancient_Hacker

Jan 1, 1970
0
Another good learning method-- tear into a dead TV set-- in order to
pick up off the air signals they need to have exceptionally good
shielding of all the radiative areas, which includes almost everything
except the audio amp.

Note how they place metal shield boxes over the top and bottom of
critical areas, how there are ferrite beads on various transistor
leads, how there's at least a ground copper pour around the single-
sided PC boards, if not another signal and poured ground layer on the
flip side..

In one particularly noisy board I designed long ago, particularly edgy
signals had to be rounded off by RC filters right at the source
pins.
 
R

Richard Henry

Jan 1, 1970
0
Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????

You need to add split power and ground planes.

;)
 
P

Paul Mathews

Jan 1, 1970
0
Can you post a picture of the board? What clocks do you have on board?
And what emitted frequencies are you seeing? There are many
possibilities here.

What does the gadget do?

John

I agree that you are unlikely to pass emissions by merely adding some
filter components. Books have been written on this subject, and you'll
find recommendations in previous threads on the same subject. However,
I'll add a couple of points here:
1) USB and other differential signaling schemes require absolutely
balanced lines, over a wide range of frequencies. Any amount of timing
skew or impedance imbalance results in differential mode EMI, which
beads and cable clamps will not filter, and the cables are excellent
antennas at certain frequencies.
2) Cable quality does matter.
3) You need to participate in any EMI testing to ensure that the pass/
fail criteria and apparatus setup are favorable to your equipment and
to direct the test tech so that data available from the test provide
you with the most useful diagnostic information.
4) During testing, you may be required to hook up auxiliary equipment,
such as a notebook computer. This equipment may have barely passed its
own radiated EMI tests, and you will be burdened with the field from
it as well. It pays to find out which auxiliary equipt is most quiet.

Some search terms for you: Mark Montrose, Keith Armstrong, Howard
Johnson, minimize loop area, EMI and slew rate control

Paul Mathews
 
J

John Larkin

Jan 1, 1970
0
Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????

Can you post a picture of the board? What clocks do you have on board?
And what emitted frequencies are you seeing? There are many
possibilities here.

What does the gadget do?

John
 
R

Rich Grise, Plainclothes Hippie

Jan 1, 1970
0
Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????

Tinfoil hat?

Good Luck!
Rich
 
Hi everyone,
we have developed a telematics prototype pcb which has to meet the
class B requirements of EU.It has many cables(like
RS232,USB,DB15,Audio jacks) connected to it.
But certain frequencies emitted by the pcb are very high.
I have tried options like shielding,enclosing with metallic
box,ferrite cores on the cables etc.. but in vain.
Can anyone please suggest the effective ways of reducing these
radiations????

Thanks to everyone for your valuable suggestions.
Please note that ours is a ten layer board out of which 2 are ground,2
are VCC planes completely.
we have even taken care of placing ferrite beads,decaps close to the
chips.What we have observed in our testing is that when we change the
position of power cable(cable through which power is fed to the pcb
from a battery) from vertical to horizontal position radiations are
minimised to great extent.Can anyone please explain why is this
happening????
 
F

Fred Bartoli

Jan 1, 1970
0
[email protected] a écrit :
Thanks to everyone for your valuable suggestions.
Please note that ours is a ten layer board out of which 2 are ground,2
are VCC planes completely.
we have even taken care of placing ferrite beads,decaps close to the
chips.What we have observed in our testing is that when we change the
position of power cable(cable through which power is fed to the pcb
from a battery) from vertical to horizontal position radiations are
minimised to great extent.Can anyone please explain why is this
happening????

That's because your board generates some mag field which couples with
your wire, inducing some voltage along it. Then the wire being a nice
antenna does its job.

This is a current loop related problem and to investigate this you need
an H field probe (small loop on a 50R coax cable end) and an SA.

But EMI testing on a board along is almost meaningless. For ex. in your
final product if your box is a metal box (i.e. no coupling to the
outside world), you might be able to set your power cable path so as to
minimize the coupling and be done with it.
 
Thanks to everyone for your valuable suggestions.
Please note that ours is a ten layer board out of which 2 are ground,2
are VCC planes completely.
we have even taken care of placing ferrite beads,decaps close to the
chips.What we have observed in our testing is that when we change the
position of power cable(cable through which power is fed to the pcb
from a battery) from vertical to horizontal position radiations are
minimised to great extent.Can anyone please explain why is this
happening????

You haven't decoupled the power supply carefully enough on the board.

Every time a logic gate changes state current is drawn from the power
supply, and flows through the on-board capacitances back into the
ground and from the back to the power supply.

If you decoupled the connections to the power supply with a big, low-
ESR capacitor where they hit the board, most of the high frequency
current circulates on the board up against your buried ground plane
and doesn't radiate much. The residual current circulates through the
pair of cables - power and ground return - that goes to your power
supply.

You can minimise this radiation by making your power connection
completely coaxial - heavy duty coaxial cable and appropriate coaxial
connectors - but nobody ever does. Twisting the two cables together
can reduce this radiation a lot, but the terminals on the board and on
the power supply are always far enough apart to leave two radiating
loops of significant area.

You can also reduce the high frequency current circulating through the
power feed by putting a more elaborate low pass filter structure at
the power input to the board - but the inductors have to be sized to
carry the DC current, which means they tend to be bulky and expensive.

Hope this helps.
 
Top