How to reduce radiated emissions

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

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.

-- Bill Sloman, Nijmegen

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.

You need to add split power and ground planes.

;)

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

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

Tinfoil hat?

Good Luck! Rich

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,
Fred.

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.

-- Bill Sloman, Nijmegen