Design for EMC (RF emmission)

Go To Last Post
24 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi all, I've had great success with the level of support and knowledge here in the past, and hopefully you guys can shed some light on my most recent puzzle. I've got a system that I need to pass through the FCC Class B limits. I'm about 3 dB over the Class B limits (we're good for Class A, which is a relief), but I need to know what I can do to lower the emissions. I am *not* an RF engineer, and unfortunately my EM classes from university seem pretty useless in this situation. Here is the setup: -20Mhz Processor, isolated from 10Mhz D/A...using SPI communications. -DC/DC Power supply to provide power on the isolated side -two layer PCB -Digital ground plane on the processor side (bottom of PCB only) -separate analog & digital ground planes on D/A side, connected only at one point. (bottom of PCB). Currently, the problem emissions are occuring between the 50-80Mhz ranges....seems that much of it is radiating via the wire connections. Here are my questions: 1) Will lowering the processor voltage help in this regard? Currently running at 5V 2) I read that putting small resistors (10-50 ohm???) in series with the data lines (going through isolation) may "round the edges" producing less noise? 3) I was told that having separate analog/digital ground planes doesn't make sense. Should I just make one big one? 4) Ground extends to the output connections . Should the ground plane include the connectors, or should I run a trace from the connector to ground. 5) Should I put another ground plane on the TOP side of the board? 6) I've read a bit on ferrite beads. Any recommendations on WHERE to put them and how to calculate them? I'm reading a few books on the subject now, but I'd like to get some insight from real developers! Thanks in advance

Last Edited: Wed. Jun 24, 2015 - 11:06 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

sepparate analogue / digital ground planes are not here to eliminate EMI/EMC per se.

Tell us a bit about packaging...what kind of enclosure are you using.

EMI/EMC interfrence may be dueto a number of cuaases and generaly falls into radiated or conducted interference.

ferrite beads will no doubt help provided you selct the right grade of material.

the principle of operation is simply that ferrite material is lossy and will exhibit higher losses at higher frequencies.

by threading the wire through a bead a series impedance is effectively placed in the line. The lossier the material the higher the value of series impedance.

But beore you go fitting beads or filter capacitors tell us about the packaging

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi, thanks for the quick reply.

The packaging is a plastic box, and the terminal blocks extend outside of it. There is very little I can do in terms of sheilding the device, so I think I have to reduce the emissions on the PCB, instead of trying to "contain" them. The emissions in questions are radiated. The circuit passed conducted emissions without problem, I think mainly because its 24VAC powered.

At the lab, the engineer told us to try to merge the ground planes together in as many points as possible. I quickly soldered it as much as I could and we did notice a significant decrease in radiated emissions at higher frequencies....however, I don't know what impact this would have on the accuracy of the D/A.

I was also told to shorten and strengthen the ground traces leading to the filter caps from the I/O lines to the A/D...its on my list of to-dos, but if I can implement a few improvements at that same time, it would be good, and save me from redesigning the board over and over.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

plaaaastic box is a problem...

there are a couple of inexpensive things you can do in the lab...

a) wrap your board in a sheet or two of paper and follow that with a sheet of aluminium foil grounded through a munting scre in the box and check the radiated prolem.

If it brings you witihn spec then spend some money on a flexible ( mylar ) printed circuit board such that copper i on the outside of a wrap around shtee t which will be gorunded and tack soldered from outside into a shielding sleeve and then packaged within box.

b) take your plastic boxes to a vacum deposiotn shop who can metalize the inside of your box and that will bring the radiated component down

c) try the ferrite bead solution select ferrite beads made from a material designed for HF applications to mind comes NEOSID F8 grade of material.
Best thing to do is talk toYour suppliers of ferrite components and obtain data sheets on various grades of materials that they supply.
Also try placing small valu caps at the very terminal blockbut make sure ferrite beads are between the the caps and active I/O pins on the offending active device..in other words form an L section low pass filter out of the bead and the capacitor. The choice of capacitor is to be made after you settle on the bead but witiiin specifications for capacitive load of the active I/O device

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Lots to think about. Any comments on my #1-#5 ideas? Will any of those suggestions work/help? When using a small "sniffer" probe we deduced that the radiation is coming from the I/O wires coming into the box.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

For the lab only: what about graphite treatment (with a pencil) of the plastic box inside?

___(°)^(°)___
A(VR)staroth

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Is it a 16Mhz AVR? Do you have the CLKOPT fuse on? Do you fail because you are radiating a nice clean 16mhz sine wave? These items might correlate well with the problem you are having.

Imagecraft compiler user

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

1) my guesstimate is that it will help ~4dB. But then you probably can't run 20MHz.
2) a good idea for signal integrity anyways.
'small' is probably in the 80 ohm range. Google for 'trace impedance calculator', and calculate the impedance for your tracks. Subtract 25 ohms for the AVR output FETs, and 10 ohms more for lost reflection, and you typically end up with 100 ohms. When you have it right, the waveform at the destination looks nice, clean, and sharp. To measure this, don't use a big capacitive scope probe with a long inductive ground leads. 'High speed digital design - a handbook of black magic' explains how to build a suitable probe: place a 50 ohm termination resistor inside a BNC that goes on the scope, attach a suitable length of 50 ohm coax, solder 2*450ohm 1206SMTs in series with the center conductor, and use that as a probe. A meter of RG174 does perfectly well with 250MHz clocks.
I did this for a 36MHz clock net and got 20dB.
3) from the emission perspective it doesn't really matter.
4) doesn't really matter, unless the tract to ground is run alongside something noisy. It's just a longer wire.
5) one ground plane suffices. Just make sure you have a ground return under/up against all fast signals so as not to create radiating loops.
6) put good decoupling caps (100nF 0508 are nice) right up against the chip's power pins, and place ferrites in the VCC wires feeding those caps. This technique gave me 30dB in a design that was failing by preventing the noise from coupling out onto the VCC wires (and out through the regulator).

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

And to add a little bit to 2):
Adding a resistor matching the trace impedance to a signal being driven by a fast driver will not round the signal seen at the receiving end.
At the transmitter, after the resistor, if it's a 100 ohm trace and a 100 ohm resistor (including driver Zo), one sees a half-step for twice the delay of the trace. What happens is that the VCC voltage is divided by the output impedance and the trace impedance, resulting in a step of 0.5VCC propagating out along the track. When it hits the end it gets reflected, meaning another 0.5VCC pulse traveling back towards the receiver. Thus, the receiver sees a good step of 0.5+0.5=1*VCC, and the driver sees 0.5VCC for the duration of the trip 'out and back home'. This is called source termination and is useful when there is only one receiver, and that receiver is at the end of the wire. (in reality this also holds for, say, 2 input at the end of a 50 mm wire). If you have multiple recipients along the wire, end termination has advantages.
When the impedance driving a trace is low, for example feeding a 100 ohm trace with 10 ohms, the edge will propagate back and forth multiple times, and the pulse current is higher. If the noise is radiated through the power supply, and we then add a 90 ohm series resistor, we get a 6dB reduction in initial current, and 6-12dB from not having standing waves on the trace.

If the series resistor is larger than the impedance of the trace you get a staircase waveform at the receiver, which, depending on the trace length, may or may not violate edge rates at the receiver. For example, if you place 400 ohm in series with a 100 ohm trace, the propagated step is 1.0V in a 5V system, meaning the receiver sees an initial step of 0V->2V, which is probably bad..

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I would look at your power decoupling and check the ground net and other higher current nets on the PCB for loops. My guess is that you are getting radiated emissions from a large current loop.

Remember to slow your signals down where possible also.

Check this out

http://edaboard.com/viewtopic.php?t=95127&highlight=pcb+emc

Also search EDAboard for "EMC for Product Designers" It is quite a good text on EMC.

Hope this helps

oddbudman

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Guys, thanks so much for all of the great information. This is really a learning experience for me. I will implement some of the suggestions (specifically calculating the series resistors, and implementing better power supply decoupling).

Once I have a new prototype and we do some RF testing I will report back.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Ok, so we did up a new layout with the following changes:

1) Series caps in line with the isolaiton chip
2) dual ground planes (top + bottom)
3) decoupling caps VERY close to processor + A/D pins
4) Better routing to keep bottom ground plane as clear as possible
5) Added ferrite as per Atmel APP Note.

Basically, there was very little improvement....I was really disappointed. After spending a bunch of time in the lab, it turns out that most of the noise is coming out of the input lines. I bought a "Near Field" EMC probe from Credence Technologies which I can use to pinpoint the source of the EMI. It looks like the whole ground plane is being very noisy.....

So I started pulling components one by one....
1) Pulled A/D -- no change
2) Pulled Isolator -- no change
3) Pulled DC/DC converter -- QUIET!!!!

So I pulled the DC/DC converter (we need it on there for isolation between input/output) and just shorted the GND1&2 and Vout1&2 (basically no isolation), and the board is QUIET!!!

I also tried with two power supplies and it remained relatively quiet!

I put the isolator and the A/D back on and it is still QUIET!!!

Here is the kicker: With ONLY the GND of the DC/DC connected to my isolated side, it is still noisy. This is also true if I connect ONLY the Vdd.

What the heck is happening? The DC/DC is running at only 150kHz (at the lab the problem frequencies were around 40-70 MHz). It can't be the 400th harmonic of the DC/DC????

I tried bypass caps (0.1uF) as well as 1000ohm ferrite chips to the DC/DC without any visible improvement.

I tried the DC/DC converter on its own and at first it doesn't look noisy, but when I added some longer leads to the output, it appears noisy towards the end of the leads. The only thing I can think of is that the DC/DC converter coupled with the large ground plane I've got going is causing issues.

Anyone have ANY suggestions?

We pass Class A without issues, but we're aiming for Class B, and we're about 3dB away. :(

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:
What the heck is happening? The DC/DC is running at only 150kHz (at the lab the problem frequencies were around 40-70 MHz). It can't be the 400th harmonic of the DC/DC????

Why can't it be? It is designed to be energy-effective, so switching must be very rapid, even though the frequency is only 150kHz.

I have nothing to advise, but I'm very interested in your results too.

The Dark Boxes are coming.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

^^^ well, it must be the noise generated by the DC/DC converter. I hooked one up directly (ie: without anything), and it lights up my near field probe like a Christmas Tree! So....what can I do about it? I've tried a liberal application of ferrite beads (right at the output of the device), as well as caps, and LC filters, and nothing seems to make much difference....mind you, I'm not doing anything overly scientifically, but more by trial and error.

One thing to note: it seems to be noise only on the OUTPUT side. The input side of the converter seems relatively quiet.

Thanks for any insights :)

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Interesting, is the output DC clean per se? So it's only radio noise, or is the noise also present in the DC it outputs? Because if its output is clean, there must be a way to wrap the beast in grounded tin foil, like people suggested in the beginning, and it might solve the problem. Even, maybe there are stock shielding cases that can be fixed on PCB's.

I was going to ask which DC/DC converters to avoid, but then I guess they are all the same stuff...

The Dark Boxes are coming.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Without seeing the emission plot one can only take a wild guess, but I'd say the diodes on the DC/DC secondary. When they turn off, their capacitance will ring with the stray inductance of the secondary, resulting in a high frequency common mode being seen between the input and output GND of the converter. Typically manifests itself as 'dense grass' rather than a single carrier. 50MHz sounds about right.

1) Short it out: capacitance across to short out the RF. Something like 2*1nF would be about right. Placement is everything, a 100nF leaded part soldered across @50MHz is rather inductive. In some applications, a few nF across the converter may be out, so,

2) Disonnect it: Insert a common mode choke on the DC/DC converter's output. You can get suitable types in SO8-like footprints. 1kOhm+ impedance at your problematic frequency. It's a bit low in frequency to solve with ferrite beads.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Even though the DC/DC converter input appears to be clean, try a ferrite there anyway.

Try a copper-fill plane totally under the DC/DC (keeping in mind your isolation requirements).
You can get discs of ferrite, sometimes they help reduce radiated noise from a component (I often see them hanging over pin 40 of DIP 8751's.)

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

The oscilloscope shows a fairly clean DC output. The near field probes I'm using have a frequency range of 2Mhz .. 2 GHz. I've found that the near field probe doesn't detect much noise at the actual DC/DC converter (or even the output itself), but the noise comes from the end of the cables of the output (in my test setup)...on the board I think its the PCB traces and specifically the ground plane that's radiating the converter's noise, but the converter itself *seems* quiet.

I might be chasing a ghost here and it may even be that the converter is noisy, but that's not what failed us in the lab....however, the probe shows a SIGNIFICANT decrease in emmisions when the DC/DC converter is removed.

The problem is that I'm using the converter for isolation purposes. It is actually 12V in, 12V out, but I need 3kV isolation. If there were another way, trust me, I'd use it, because I've had nothing but bad luck with switching power supplies. Because of the isolation however, wrapping it in anything conductive is not an option, at least not the whole thing (ie: perhaps only the output side???

Here is one more bizzare phenomenon though: in my test setup, I have 15cm wires to the input +/- and output +/- pins hooked up. When I wrapped the output wires around a ferrite, I noticed that the noise decreased.... BUT it decreased between the ferrite and the output pins, NOT between the ferrite and the load!!! This seems backwards to me?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

KVP, thanks for the insight. This does make sense. At the lab, the specturm analyzer was showing three "mountains" between 50-~80 Mhz. These would shift around a bit, but it definitly wasn't a sharp peek. This may be good news that I am chasing the correct problem.

I will try your suggestions and report back. I'm having a hard time finding pertinant information on this on the web though. I would think that if DC/DC converters are such a problem for radio noise, then the manufacturer would have some suggestions on keeping them quiet!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

KVP, one more question. The notion of chokes is new to me. I found something like this:

http://www.vishay.com/docs/34158..., but I'm not entirely sure how I would hook it up? I assume pins V+ goes to 1 and out of 2 and GND goes to pin 4 and out of 3?

Should I just pick the highest impedance (ie: 2200)?

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

icm1206: Looks VERY good. I think I'm going to order some samples for myself :-)
If you can live with the 1.2 ohm series resistance and 200mA max, yes, go for the 2200. The datasheet I found doesn't have an impedance plot, but it goes like this:
Below the choke's resonant frequency, it's an inductor, and impedance rises with frequency. At some point the interwinding capacitance becomes dominant, and impedance starts dropping. Even if the resonant point is at 100MHz, it's still good.

hook-up is correct.

It's easier to sell a cheap-to-manufcture DC/DC converter if one doesn't say how noisy it is, so no, they don't.
The next time you're looking at a DCDC converter, consider building it out of a controller and a separate transformer. Linear technology has some pricey chips for this, but they're good, and they're quiet, and they tell you how to get them quiet.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

HI Guys....well I think I found the solution to the problem....sort of.

I talked to the mfg of the DC/DC converters. They suggested to put a cap between the input and output GND. Of course, this breaks the insulation, so I need to find a cap that is capable of 2500Vac. The difference is AMAZING though. My near field probe goes from full-tilt to almost nothing with the addition of a 150pF cap between the grounds.

Is this an acceptable method of filtering the RFI coming from the DC/DC? Does this revelation yeild any other ideas? I'm hoping I'm not chasing a stray ghost here, but everything you guys have stated seems to correlate with the findings/results (ie: the RFI looked like a "mountain" on the spectrum analyzer, rather than one specific peak--pointing to the converter).

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

KKP, the common mode choke I got didn't seem to do much....at least not as much as the input/output ground coupling via cap.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

[Moderator note: Due to a personal request, I am moving this thread from the Off Topic Forum to the AVR Forum, so this thread will be archived for the future. sbennet requested that this be done because it contains useful information that shouldn't be lost - EW]