Suggestion - Faraday's Cage

[migsantiago]

Hi!

I would like to learn more about Faraday Cages, how to design them and know if they're actually working.

Some tips about Ground planes and grid sizes.

Thanks!! 

[Mechatrommer]

just build a big box or round metal enclosure... with holes just enuf for you to peek out (to be safe) and there should be
1) no high volt generation from inside the enclosure
2) no body part protruding out of it
3) no part or object poking in
with that i guess you should be safe then with condition that the cage does not melt

[Mechatrommer]

how to test it? put a cat inside and fire it with a lightning bolt. if the cat is still alive, then its working

[Simon]

how to test it? put a cat inside and fire it with a lightning bolt. if the cat is still alive, then its working

you won't get away with that in the UK if the cat is killed 

[alm]

Don't be a wuss. If you have faith science and technology, get inside the cage yourself!

[migsantiago]

That's funny guys, but I really want to know good tips, please don't mock it. 

There are special things to follow when designing a Faraday's cage such as GND connection from the cage to the GND circuit and the grid size of the GND planes used on the circuit board. The grid size is essential to know which magnetic frequencies are rejected, for example, the grid in a microwave oven has special dimensions.

I have designed some Faraday Cages before, but I know they are not as good as a professional one.

[Simon]

I think you'd want the grid pitch to be like 1/10 the wavelength you want to block

[jahonen]

Gridded grounds are pretty much a thing of the past. Grid size is a concern only if you must see through the shielding.

Generally, on PCB solid planes are the best, as they will have lowest possible impedance. Same applies to the walls of a Faraday cage. One important thing is the seams of the box if the box can be opened. One must ensure that there is no long open narrow slots in the seams. Otherwise the seams will compromise otherwise good shielding. Same goes for feedthroughs (a Faraday cage is pretty much useless by itself, since all things to be shielded must be inside it). Any single unfiltered feedthrough will weaken the shielding effectiveness. Generally, feedthrough capacitors are used.

Things become even better if you can stack several solid ground planes to your PCB, connected together with fair number of vias. Take a look at RF/microwave boards, there are lot of ground vias. At very high frequencies (>10 GHz), surface roughness starts to play a role.

Regards,
Janne

[Mechatrommer]

sorry if the mocking is unwanted. but maybe if you specify more detail of your application and dimension will helps. coz i was assuming that you want to build something like this or this and why the opening is really necessary for you? what emf you want to try avoid from? wiki should be able to explain the purpose of faraday cage quite ok.

[allanw]

If the Faraday cage is opaque, is the cat both dead and alive until you open the cage?

[migsantiago]

PIC microcontrollers are very susceptible to be affected by noise, specially by Relays that commute AC power.

What I normally do to avoid noise is:

- Add 0.1uF capacitors close to my PIC and to every IC.
- Add a 330uF (or whatever the datasheet suggests) at the power supply.
- Use an aluminum box with aluminum covers. Completely metallic and input connection holes are small.
- This aluminum box has a cable which goes to the GND of the circuit. This cable is connected to the aluminum box with a screw.
- I use solid ground planes. (I was unsure about the gridded planes, so I always used solid ones, thx Janne for the info).
- Both faces of the board have GND planes.

We recently started using star grounds so that every circuit gets its own gnd line directly from the power supply.

What I don't know is this... is it good to connect the circuit GND to the AC outlet GND?

And another thing a friend asked me, if I am using a star-gnd connection such as this one (enclosed in the blue box):

http://img696.imageshack.us/img696/2345/planomp3.jpg


As you can see, that GND line is using a star connection. The GND line for every part is unique because every part has its own GND path.

The problem we have is that we were not sure about adding a GND plane. If we used a GND plane, the star-GND lines would be useless since the GND plane would interconnect them. But if we didn't use a GND plane, we would not have a Faraday cage.

I decided that we could still use the star-GND lines and also the GND planes, but... the GND planes would only be connected in one single spot (yellow oval which goes to the GND node with a 0 ohm dummy resistor, pins 1 and 2).

So, is it OK to make this connection? Is it useless?

This board is going to use relays to power some unknown AC stuff, so noise may be present.

Thanks for reading. I hope I made myself clear this time.

[Time]

If the Faraday cage is opaque, is the cat both dead and alive until you open the cage?

Only if the 'diabolical' mechanism that might kill the cat is truely random.    According to Schrodinger atleast

[Neilm]

We recently started using star grounds so that every circuit gets its own gnd line directly from the power supply.

Speaking from an EMI perspective ... YUCK.

If you want to have good immunity from EMI the best thing you can do is add a ground plane and don't have separate returns. Current will always use the path of least resistance so a single unbroken ground plane over the whole board will allow the return currents to go where they want. The only reason to have separate grounds is if there is a safety reason.

In answer to your specific questions connecting the GND of the circuit to the AC outlet Earth would depend on your application.

With good layout you might find that you have no don't need a metal enclosure unless required for safety reasons.

If you want more information go to http://www.compliance-club.com/. Look at past articles by Keith Armstrong who I have found can take what is quite a complex area of electronics and distill it down so even I can understand it.

Yours

Neil

[migsantiago]

Speaking from an EMI perspective ... YUCK.

If you want to have good immunity from EMI the best thing you can do is add a ground plane and don't have separate returns. Current will always use the path of least resistance so a single unbroken ground plane over the whole board will allow the return currents to go where they want. The only reason to have separate grounds is if there is a safety reason.

Hello Neil.

We read that it was a good idea to use star GND lines when there are power and control devices. A power device can be an AC relay and a control device can be a PIC microcontroller.

Control devices might be affected by the noise generated by the power devices, so, a starred-GND line would reduce this problem by giving each device its own GND line.

Would this be a valid safety reason to use starred-gnd lines?

Of course, if the circuit is solely conformed by control devices and no power devices at all, a starred-gnd connection would be useless... isn't it?

I will check that page out. Thanks for the link.

http://www.compliance-club.com/Search.aspx?keyword=Keith%20Armstrong

And what do you think of the board picture I posted above? According to your comments we'd better avoid the star connection and use the GND solid planes instead. The board only includes control devices and no power devices (for now).

Thanks!

[scrat]

As far as I know, the problem is quite debated, since some people say it is better to have split ground with star-connection, while others say that a continuous ground plane is the best thing.
Some time ago I was looking for information on this issue and found some documents from Analog Devices, like this: http://www.analog.com/static/imported-files/application_notes/573185595135053265003392595605308453835483630769AN214.pdf
My impression was that choices are usually based on experience...
Somewhere I found an article where an expert said the best thing to do is to have a continuous ground plane, and to keep especially in mind current flows. In a good layout (principally components positions), currents will flow in confined areas, so that each functional block's current won't flow across other areas. This is the principle that seems to me the more logical, but many people tend to separate ground planes between analog, digital (and power, if speaking about power converters or motor drives).
However, IMHO the approach of thinking about "how currents flow" is very interesting: even if it doesn't solve your problems, it forces you to consider some effects you could have missed by only looking at "voltages".

[Neilm]

Control devices might be affected by the noise generated by the power devices, so, a starred-GND line would reduce this problem by giving each device its own GND line.

Would this be a valid safety reason to use starred-gnd lines?

In my experience the only reason for having isolated grounds is if isolation is required. For example galvanic isolation on Ethernet connections or having to meet CAT ratings on input connections.

In your case I would look at having a continuous ground plane, but carefully laying out the sections on the PCB. I quite agree with scrat on partitioning circuit board layout. Again this is something covered by Keith Armstrong. He has done a book on layout of circuit boards for EMC and I would recommend it if you regularly have problems.

I recently had to review all the instruments we make at work when the EMC standard we have to meet changed. In all but two cases, simply adding a ground plane and commoning all the star pointed grounds fixed the problem. In several cases the instruments now perform better than they originally did. One instrument I saved over £5 by eliminating ferrites that add to be added to get it to pass originally, just by spending a bit more on the bare PCB. The two that we didn't get past were so old we have now discontinued them.

The thinking on EMC has changed a lot over the last decades. When I was at university 15 years ago it was never covered. But ICs have changed a lot over that time. An OP07 from 20 years ago may look identical to one bought yesterday, but advances in silicone mean that they will react totally differently to noise (even if that noise is way out of spec). Therefore things that were considered good practice 10 or 20 years ago are now shown to be less effective (or worse) now. Unfortunately, many senior engineers learned to do layout 10 or 20 years ago and can blindly follow what the learned then as "that is the way we always do it".

Yours

Neil

[migsantiago]

Experience... an important thing I'm lacking.

I think we can leave it with the starred connection for now (unless my friend changes his mind ). We'll manufacture the boards with a chinese company and I hope the first batch has no problems with noise.

We are being cautious because it's a PIC24 with an MP3 hardware codec. The codec had a lot of noise problems which resetted it so often. We found out that we forgot to connect some NC terminals and the problem was fixed, but we don't want it to happen with the client, so we implemented all the stuff I wrote above.

Thanks for your reply. And those Armstrong articles you recommended are quite interesting for EMI protection.

[NiHaoMike]

Current will always use the path of least resistance so a single unbroken ground plane over the whole board will allow the return currents to go where they want.

Not always. If the current is flowing through a trace on the top of the board and returning through the ground plane, the return current will try to follow the trace due to magnetic effects. I think Dave actually went over that in one of the recent episodes.

[Strube09]

Thought I would chime in on this one. I too have struggled with using separate grounds/star grounds/solid plane grounds/isolated grounds.

I work a lot with SMPS (mainly buck) and a lot of EMC and other tutorials I have seen seem to suggest different things when it comes to grounding. However, the more common ones I have seen (and used) is having a ground for the analog control and a ground for the power path with a solid plane ground that these attach to. These then tie together at one point and typically at the control IC. There are even many IC's that have two separate ground points (analog ground and power ground. Usually these will tie everything together at these points. This keeps the ground references at the same potential and keeps the noisy power ground from affecting and inducing noise onto the sensitive feedback and analog ground.

The biggest deal I have noticed is just to keep your loop currents as small as possible. While A solid ground provides shielding I have gotten away with short wide ground traces for the return currents on the main power returns. The nice ground plane also reduces the inductance of the traces on the top layer too.

I am still learning by failing but so far I have only had one device fail EMC and was quickly resolved with come chokes on the input power line. Oh and the one that failed EMC had a solid ground plane on the bottom layer.

Any good reading material suggestions (well as good as this stuff can get) would be great.

Strube

[jahonen]

Current will always use the path of least resistance so a single unbroken ground plane over the whole board will allow the return currents to go where they want.

Not always. If the current is flowing through a trace on the top of the board and returning through the ground plane, the return current will try to follow the trace due to magnetic effects. I think Dave actually went over that in one of the recent episodes.

This is simple to understand that any natural system will minimize stored energy. In this case the energy in the loop inductance is to be minimized. Because loop inductance is proportional to the loop area (in 3D-fashion!), the energy minimum is achieved when return current flows just under the actual signal in the plane. It really is that simple. It is a bit strange that people seems to keep less attention to the return current than the signal current, even if in reality, the return current is just as important than the signal current. If you don't believe me, then try the following: take battery and connect a lamp to the battery with two wires. Let's call the wire from lamp to negative battery the wire where return current flows. Now, I'll bet if either one of the wires is cut that lamp turns off That proves that return current is just as important as the signal current.

What I have observed at work, is that fewer grounds you'll have, less problems there usually are. I really hate it when I see the "standard" recommendation in DAC or ADC datasheets that one should split the ground plane. Strangely, there usually are no measurements to support this claim that split ground will work any better... That is usually not necessary, when correct partitioning of the circuits is done.

I once built a D-class audio amplifier using Tripath (RIP) module. In the datasheet, they recommended ground split and star grounding etc. The result was a EMC disaster, with heavy resonances in MHz frequency range, strong audible noise (rectified at preamplifier BJT input stage) and in addition that amplifier tried to blow up on self oscillations very easily. When it finally did actually blow up, I decided to design the PCB from ground up using single contiguous ground plane. Result? Amplifier now behaves very nicely, I could remove most of the EMI suppression IO-filters. No sign of instabilities whatsoever. And the audibly noise was gone. I wonder why they so much recommended that star ground

Here is a comparison of ground common mode RF noise voltages between old and new board:



As you can see, the levels dropped 20-30 dB! Since then, my conclusion has been that it is better to follow physical principles instead of application notes, as physics usually wins on dispute situations

Regards,
Janne

[migsantiago]

Excelent, another opinion that rejects split GND lines. 

Janne, about that picture you posted... are you using a multi-layer board? Did the 4 layer board improve noise rejection?

[Strube09]

So quick question for the single ground plane guys/Gals?

Do you just stitch to the ground layer with a via whenever and where ever is convenient? Or do you use like the digital signals together and they all tie to the ground layer together? I was told this was a good way to do it because it keeps all of the digital grounds at the same potential. If they are stitched all over the board ground paths may have a Vdrop that can cause errors.

I use digital as an example but I work with many SMPS that have analog feedback signals and high current power signals. I was disciplined into keeping these separate and tie them at one point to keep the controller feed back an power signals at the same potential and keep the high current (mainly high di/dt and dv/dt singals) from interfering with the sensitive analog circuits.

Strube

[Neilm]

I try to make sure that each GND connection is taken to the GNd plane by a dedicated via as close to the pin as I can. If there are two connections beside each other they may share a via but not usually. (I really annoy the guy at work who lays them out).

To separate high current signal returns and other signal returns I would use the positioning of components to keep the returns separate. I have been working on an instrument that is measuring milli-volts at one point and has 20A being switched at another point. Careful attention to routing has meant that there were no problems when the 20A was switched.

Neil

[jahonen]

Do you just stitch to the ground layer with a via whenever and where ever is convenient? Or do you use like the digital signals together and they all tie to the ground layer together? I was told this was a good way to do it because it keeps all of the digital grounds at the same potential. If they are stitched all over the board ground paths may have a Vdrop that can cause errors.

Yes, ground pins of IC's are best connected directly to the ground plane, although optimal way to route decoupling capacitors depends on the layer stacking. See here, pages 99-112. For logic applications, definitely correct way for ground connection is to connect the ground pins directly. Ground plane impedance is so small that I would be amazed if voltage differences of digital IC ground pins would cause a problem.

There are some exceptions I have used on the single ground plane concept. Namely, I have applied a "ground over ground" principle on a steering of step-down switching regulator ground currents, where I placed separate local ground above the main ground plane. Capacitive coupling keeps them tightly coupled at higher frequencies. I think that clean ground is the most important single thing to achieve low EMI levels. If there is a lot of ground noise (common mode), then your game is basically over. It usually means re-spin of the PCB and/or general system design.

However, I have not compared that method to single ground plane version, though, so there is still room for the experiment. Now that I have a spectrum analyzer, it makes it easy to check the goodness of any solution. I may very well turn out that there is no advantage to make that separate (but still tightly coupled) region.

Janne, about that picture you posted... are you using a multi-layer board? Did the 4 layer board improve noise rejection?

Yes, I used multilayer. No way to make substantially better board otherwise. Multilayer usually greatly enhances EMC properties, from both (radiated) immunity and emission perspective. And since the ground plane impedance is low, ground noise voltage between two points is small, important thing in audio application.

Main reason for goodness of multilayer board is that signal and respective return current are very close to each other which implies low inductance of the loop. Small loop area makes it difficult for the external intererence field to couple. Also, nearness of ground plane reduces crosstalk of the signals. You can think two traces as a transformer, where the aggressor trace is the primary and victim trace is the secondary. Traces are coupled to each other via mutual inductance. Ground plane couples with each trace and reduces this mutual inductance. Same applies also if you route star ground traces beside each other, they will also be coupled inductively to each other, so there is noise coupling between them even if they do not share the same copper.

And yes, thinner 2-sided PCB is better, but two-sided board with 0.2 mm dielectric is not mechanically very robust

Of course, conducted EMI or susceptibility might still be a problem with multilayer board, and needs to be handled via suitable filtering at IO-ports.

Regards,
Janne

[scrat]

What I have observed at work, is that fewer grounds you'll have, less problems there usually are. I really hate it when I see the "standard" recommendation in DAC or ADC datasheets that one should split the ground plane. Strangely, there usually are no measurements to support this claim that split ground will work any better... That is usually not necessary, when correct partitioning of the circuits is done.

The really strange thing I found was that they recommend to join the two split grounds at the ADC... Why do they take out of the package two separate pins for ground, if then you have to externally connect them just out the chip?
This is a great enigma to me.