EEVblog #1176 - 2 Layer vs 4 Layer PCB EMC TESTED!

[EEVblog]

What difference does a 4 layer PCB make to EMC radiated emissions compared to an identical 2 layer PCB? And why?

Dave does H-Field near-field probe testing on two otherwise identical PCB's.

Electromagnetic waves and the difference between near field and far field, and H-Field and E-field probes and wave impedance is also explained.

The PCB layout is then examined to look at loop area and by-passing and what effect this has.

[MT]

Would be interesting to see emission differences between same designed boards in which one is smt the other dip.

[EEVblog]

Would be interesting to see emission differences between same designed boards in which one is smt the other dip.

Wouldn't be any different if the layout remains otherwise identical.
Would anyone be interested in a 6 layer version with grounds on the outside layers?

[T3sl4co1l]

Can you stop bloody calling it "radiated" when you're measuring with a near field probe?  THANKS

Tim

[Matty]

Hello - I'm confused about the spectrum shown.  The harmonics are greater than the fundimental?
Is it because the higher frequency is traveling though the air better? or the switching are all out-of-phase a little bit and making the noise?

[abeyer]

Is there a design rule or analysis type thing in any layout tools that helps identify loop areas? Seems like it would be amenable to to automated analysis.

[MT]

Would be interesting to see emission differences between same designed boards in which one is smt the other dip.

Wouldn't be any different if the layout remains otherwise identical.

I argue it would for the "higgelypiggelywoppdiidoo"2 layer.

Would anyone be interested in a 6 layer version with grounds on the outside layers?

As prior life PCB dude, yes please, on teflon!

[T3sl4co1l]

Hello - I'm confused about the spectrum shown.  The harmonics are greater than the fundimental?
Is it because the higher frequency is traveling though the air better? or the switching are all out-of-phase a little bit and making the noise?

The H probe reads dI/dt, so the spectrum of a square current (harmonic amplitudes go as 1/f), as read by the probe, is ~flat (an ideal periodic impulse).

Connected to an integrator, you get ~the original current waveform again, uncalibrated of course (this isn't a current transformer, the gain will be arbitrary with distance!).  This can help recognizing sources when probing in the time domain (on the scope).

Tim

[satblip]

Superb video !

I have two questions in mind:

1) Does anyone have a reference for the probes and the preamp?

2) I have always had trouble to understand why we put the ground plane and VCC in the inside layers and not the outside layers. It is definitely the right way as every good designer does it, but I would have though that if the ground layer was on the outside plane, it would have act as a shield?

Thanks !

[KaneTW]

When you have signal layers on the inside, there's crosstalk for parallel signals on opposite sides. Having a DC plane prevents that.

Ideally you want your noisy signals buried in a stripline pattern, i.e. covered with ground/vcc above and below.

[johnlsenchak]

Information  overload  on the  one  !  LOL

[Neilm]

I wasn't suprised by this at all.

Many years ago there was a big change in the EMC regs for test equipment that affected the company I worked for. Many of there older instruments needed to be fix and as new instruments were in development, they didn't want to change any of the board test fixtures. I was given the task to fix these and was unofficially told to "add ferrites until they pass". Many of the failures were 2 layer boards with split power and 0V. Only one needed the split (for safety reasons).

I got a  grudging agreement to go try 4 layer boards with common 0V - grudging as "this will push up the board cost". It fixed all but 2 instruments (that we didn't sell many of anyway so they were obsoleted).

For one instrument - it ment we could replace 2 ferrites that cost about £4.00 with one that cost £0.70 more than covering the cost of the PCB.

Since then, 4 layer boards have been pretty much mandatory on all new products.

[mcinque]

This is a great demonstration.

And yes, I (and probably many other people) would be much interested to know what changes with 6 layers and ground outside!

[mrpackethead]

EMC aside, designing a four layer board is just SO much quicker than a two layer. 

[Ribster]

Loved the video!

[Barny]

Superb video !
.
.
.
2) I have always had trouble to understand why we put the ground plane and VCC in the inside layers and not the outside layers. It is definitely the right way as every good designer does it, but I would have though that if the ground layer was on the outside plane, it would have act as a shield?
.
.
.

Its to get more capacity betwen VCC and Gnd.
The closer the layers, the higher the capacity.
(Plate capacitor)

[Doctorandus_P]

I wonder what kind of design rules you used for the inner layers.
Did the rows of the dip IC's cut big slots in those layers, or are the power layers sneaking between all pins?

This is an area where SMD is better than THT. Smaller SMD chips also are closer together, hence smaller loop area's and less ratiation. (And the near field radiation is also radiated, even though not very far, it certainly is not conducted).

I also would have loved to see a comparison with the board where you snapped off all the decoupling capacitors. What does that do with radiated noise?

Also not a single word about distributed capacitance between the power planes, but I think this only becomes really usefull in the GHz range.

15dB is a significant difference, but I do not find it shocking, it sort of gives me the idea that the original layout indeed is not too bad. The traces on that board are very coarse. It seems to be designed for home-etching. Any PCB factory can work with much finer design rules, and that would leave much more room for ground fills and via stitching.

I would love to see a teardown of those blue probes. Tear those down!
Is there any magnetics in there, or only an inductor? How much wiring?
Many loops of very thin strands?
Is the coil shielded? How about inter winding capacitance?
I know the're bloody expensive, but a detailed teardown & analysis is much more interesting than a blab about a dumpster dive.
I also would not be surprises if a piece of thin enameled copper wire wound on a corc would give comparable results. Coils of 230V relays are an easy source of thin wire if it's not glued together. A quality comparison between such a homebrew and the blue probes would also be very intersting. The blues are simply out of reach for almost all hobbyists.

Also, you've got CNC machines (mill, 3d printer) and a robotic arm.
You can attach the near field probes to one of those and then let a PC generate a "height map" or the radiated field. Especially if the resolution is high enough to see individual traces this can be a very usefull tool during pre-compliance testing of the first board revisions.
You can get nearer to the traces (higher resolution) on the bottom of the board.

If you want to do a follow up on this, I would also like to hear your opinion about dividing the budget between GND and Vcc planes on a 2-layer board.
I think it is best to:
1). Put decoupling caps as close to the IC's as feasible.
2). Connect the decoupling capacitors (not the IC's) to the power planes.
    This way the Capactitors filter more of the noise generated by the IC's.
    It keeps the GND plane cleaner.
3). Use Either GND (more traditional) or Vcc (uncommom) with as big an area as feasible.
4). Use lots of via stitching, every trace should have a small loop area with the GND plane.
5). The other Power net: Use some decent grit, but not too much area.

[EEVblog]

EMC aside, designing a four layer board is just SO much quicker than a two layer.

Yeah, no need to worry about power placement, it "just happens" at the end.

[EEVblog]

I wonder what kind of design rules you used for the inner layers.
Did the rows of the dip IC's cut big slots in those layers, or are the power layers sneaking between all pins?

You can watch the video:
It didn't flow through the pin pads, and still the performance was hugely better.

[mrpackethead]

EMC aside, designing a four layer board is just SO much quicker than a two layer.

Yeah, no need to worry about power placement, it "just happens" at the end.

Perhaps a little simplified, and true when you only have one power rail.  When you have six it needs a bit more help.

[Doctorandus_P]

I did watch through the video, and  find it astounding that you can get any work done while simultaneously & continuously talking & reading & responding to that text thing on the left.
If you had 5% of the experience with KiCad compared to Altium this would have been 2 minutes of work.

To Try to keep short I will only comment on one thing, because I found it too painfull to watch (as you also predicted @12:53 in the video).

You spend almost 10 minutes (From 49:25 to 58:09) talking about a feature KiCad presumedly does not have, and then at 58:09 you accidentally do exactly what you want and even more, but you do not recognize it because you are talking too much and distracted by commenting to the others.

Another reason you did not recognize it is because the design rules are set much smaller than what they were originally routed on. So KiCad does not only straighten 3 traces with one mouse swoop, adjusts the trace spacing to the current design rules. It has also placed those traces off grit. Design rules take precedence over grit settings, as you are explaining @51:30. I appreaciate you want to give constructive feedback to the KiCad team, but it will not be necassary for this feature.

I even managed to capture a screenshot of the straightened & off grid routed traces.

This works so well that I only use a grid for placing components and holes and such, and ignore the grid for routing traces. Trace widhts should be defined by DRC rules, not by some grid. You say Altium users keep changing the Grid all the time. I just ignore it (or set to < 1mils).

Note 1: If you do not want the traces hugged so closely you should edit the design rules for those traces, and not use the grid.
Note 2: Traces can also be locked.

[Doctorandus_P]

I've also used many different PCB programs in the last 30 years. Mostly for hobby projects, I'm not a "professional designer" (whatever that means).
And they all have their quircks.

I've also read and seen many reviews, and the common thing is that reviewers tend to like and appreciate the programs they are familiar with, and have difficulty with adjusting to the idiosyncracies of software they do not know wel. A classical example of this is the mouse rant in the beginning of the video.
I found that a nice way  to pan is to zoom out on one section of a board, and then zoom in on another section, both with the scroll wheel, not even a need to laboriously push a button. But as everything, it takes some time to get used to it.

[nctnico]

I've also read and seen many reviews, and the common thing is that reviewers tend to like and appreciate the programs they are familiar with, and have difficulty with adjusting to the idiosyncracies of software they do not know wel.

I agree with that. Every PCB package has a certain work flow and idea behind it. I'm currently learning a new PCB package and even though the old one is from the same vendor (Cadence) it works completely different. Not so different compared to other packages I have used but nevertheless it is going to take time to get to the level of productivity I could achieve with the old package. Fortunately the new package has a very easy way to create shortcuts so I re-created the most used short cuts from the old program.

[German_EE]

I can think of only one advantage of two layer boards over four, removing devices during repair is a lot easier.

If whilst replacing a chip on a two layer PCB you remove a plated through hole then the repair can be easily done, even on a power pin. Sure, you might need to drill a 1mm hole and pass a wire through to link a couple of traces but it can still look good.

Now switch to a four layer PCB and pull out a plated hole by accident. It's impossible to remake the connection without a jumper wire to the nearest power or ground pin, thereby destroying your EMC work.

Yes, I know that it's possible to remove any part using professional equipment without damaging the PCB, but not all of us have that professional equipment and after using braid or a manual solder sucker on the same pin for the fifth or sixth time you may hit problems.

[mrpackethead]

Are through hole parts even a thing still