ESD and EMI protection - How to?

It would be helpful to know the failure mode.

It may not be the inputs that need protecting.

Yes, the power and ground on your board need protection against any ESD. Your power supply alone may not be sufficient.

As mentioned by @n.a.moseley the schematic would be necessary to give you any specific advise, but in general, no resistors alone won’t help much. You may need some series resistance depending on your circuit but I would look into some combination of TVS diodes, zener diodes, and clamping/steering diodes.

Resistor noise is going to be the least of your concerns. Given the low resistances and low bandwidth, resistor noise will be in the nV (nano-volt) range.

IEC 61000-4-2

1 Like

Hi All,

Thank you for your responses. I went to the client Yesterday and reviewed what had happened during tests.
They performed 2 tests. The first being EMI testing where they send a lot of radio signals close to the device.
For this test the device unfortunately failed also. Every 100Mhz it picked up the signal and messed with the opamp or the dac. Anyways the resulting measurements from the loadcells were completely off.

The second test was the ESD test where according to european regulations (IEC 61000-4-2) they test with 2, 4, 8 and even 15kV. For the USA apparently these regulations go up to 8kV and are voluntary.

Something in the opamp region got fried with the 15kV

Which is weird because the product is inside a aluminium housing and the opamp circuit is no way near the side of the housing where there is plastic (for the button and the BLE antenna).

But we found out that during assembly, the cables from the loadcells (which are about 120mm) were about 60mm too long and were folded above the pcb and reached the plastic side (near the power button).
The 15kV fried the circuit when touching near this button.
So we speculate that actually the spark entered these wires and directly fried the opamps (or mosfet which powers off the sensor ground).

Also we think these same wires might be the reason for the EMI pickup of radio waves.

Does this sound (very) plausible to you guys?

This brings me to a second question.
The housing is made of aluminium and should function as a shield. But we did not ground it…
Should we ground it to the pcb ground? (or battery ground) ?

Find attached the schematic and a picture of the device.

In 2 weeks time I will get a lecture from the testing guys on how to design a PCB for EMI and ESD.
But I would like to understand more about this beforehand.

And I think it is a nice real world learning case :wink:

Firstly I would shorten any wires so that they were no longer than absolutely necessary. It would also be a good idea for your loadcell wires to be twisted in pairs. It wouldn’t hurt to do the same with the battery wires. Also try adding a small capacitor (10n) between +IN and -IN of your opamps. If possible add ferrite inductors to all four loadcell wires were they connect to the PCB.

2, 4, 6, 8 kV is used for contact discharge testing where the tip of the ESD gun is placed in direct contact with any exposed metal surfaces or external connections.
2, 4, 8,15 kV is used for air discharge testing when there are no exposed metal surfaces or external connections.
Each level consists of 3 discharges of each polarity.

Again, you need to more accurately determine the failure mode. In other words, exactly what failed? This would help identify where you need to add more protection.

The AD8226 has ESD protection on it’s inputs but it is only 1.5kV HBM which doesn’t even meet level 1 of IEC61000-4-2. The ESD protection it does have works by dumping the excess current into your power rail. Since you are using a charge pump regulator with a relatively small capacitor it is very unlikely your power rail can absorb this excess current (see below). Therefore your 3v3 rail will spike and this is probably what has caused the damage.

I would consider adding something like a 3V3 unidirectional TVS diode between the battery input and ground. More importantly I would add a 3V6 zener diode between the 3V3 power rail and ground.

Good luck!

Note: The current from a level 4 discharge, 8kV contact or 15kV air discharge, has a rise time of 1ns and a peak current of 30 amps, 15 amps after 30ns.

Edit: The capacitor mentioned above to be added to the opamp inputs must be a good quality C0G/NP0 or film capacitor.


@1.21Gigawatts A very informative post, Rob!

1 Like

@1.21Gigawatts Thank you (and all others) for your reply. Very informative indeed.

I had a crazy busy week with other projects so sorry for my late reply and thank you.

Lets dig some deeper :wink:


I tested te pcb and everything works except for the opamps. They just output a fixed value. One is at 3.3v and the other at 1.6 or something.
All other components seem fine.

Normally the wires from the loadcells would not be close to the plastic housing and inside an aluminium shell away from prodding fingers. So therefore I did not think to protect these inputs.
Would you agree with that (in other words, if the wires are stashed awaydo you think I still need to protect these inputs?)

If you still recommend protecting the inputs what are my options. I see you suggest a tvs diode and zener. I also have read about resistors in line with the inputs (to eat up the current I assume).
And for these parts, what are the variables I should consider (speed, max voltage, …)
What will / might be the influence on the input?

The loadcells are polled around 10x second. So not extremely fast.



The housing is made of aluminium. This should act as some protection.
However. I did not connect it to the pcb ground in any way.
Should or shouldn’t I do this and how?
Is it ok to connect it to ground at the battery compartment? Or is this too far away from the pcb?

Analog ground

I did not bother with making a separate analog and digital ground on this pcb since it is sooo small and in my eyes the traces are short. Was this a mistake?
(Maybe this is something @ChrisGammell would know)

Pickup of radio

So it picks up radio waves. Whenever it does that the measurement of the data is off scale. So does that imply that this is before the opamps (aka the loadcell wires) or after the opamp in the traces of 2cm to the ble module (on both sides fairly ‘shielded’ by groundplanes)


Unfortunately it would be very difficult to twistpair the wires after the fact. Next batch of loadcells I could ask the factory. Same for ferrite beads since there is no space for in the housing.
So my hopes are on shielding from the housing.
And maybe extra shielding by metallic mesh tape? Would that be an option? But should I then ground this mesh and how?
(Or would more affordable aluminium or copper tape also work?)


And/or a solution like a capacitor/filter between the inputs. Would this 10n capacitor work, and how? And what influence will it have (RC ?)
Which specs for the capacitor should I consider?

Well a lot of questions again. Hope to make this post more informative :wink:

1 Like

Hi Frits jan,

Sorry, but this is no longer a small design problem. You’re basically asking us to re-design/ruggedize a commercial product for free.

Als je wilt, ben ik tegen een redelijk uurtarief in te huren.


Haha Niels,

Thanks for the feedback. It was absolutely not my intention to do this. I, like many people on this forum are just interested in electronics and might sooner or later experience things like this. It is a thing you will learn from either an education background or from experience.

So I thought this fits the CE forums well.
And it is a real live example which makes this interesting.

Also because I think there are many ways to rome, it might be interesting to see different reactions. And also might this post act as a warning for others to at least give this a thought.

As for your offer, when I am still completely lost I might take you up on it :wink:
I can always use some experts on my side. Will send you a pm.

Best regards
Frits Jan

Hi Frits Jan,

I agree real-world examples, like you show here, are excellent show-cases on what people will run into when making a product. I see where you’re coming from. On the other hand, there is a fine line between helping people grow by providing knowledge or feedback, and providing specific knowledge that, under other circumstances, would result in a consulting job.

My personal view is that, when it comes to highly-specific questions/help on a commercial product, this line is crossed.
I am curious what @ChrisGammell 's position on this is.

I’m sorry if all this comes across as confrontational, that’s not my intention at all.


Sure I understand. On the other hand. This type of problems you will likely only encounter in real live (commercial) products because why test hobby projects on emc and esd :wink:
And since part of my background is in CE, I thought this might be a nice thing to post here and get deeper into.

On the other end, I might ask @ChrisGammell to remove this post because it is a real live product… Don’t know if the forums are searchable by google…

I will get a lecture on this topic tomorrow from the test expert and am planning to share the things I learned HERE. But would love to get into the knowledge beforehand because I would like to have some second opinions.To see things more in perspective.

share HERE not THERE :wink:

Most of your questions have been answered. You may not like the answers because they are all difficult to do at this stage. As for band aid solutions like copper foil tape etc, it may help with EMI but make the ESD worse.

While you may not test your hobby projects a commercial product should have been tested long before the production stage. If EMI/ESD certifications are important for your product it may be wise to halt production until you resolve the issue.

1 Like

Honestly, I think this comes down to what each person is comfortable sharing. If it doesn’t violate any of their company rules, I think it’s fine to ask for assistance here. Each forum member has the choice to participate in a thread or not, and stop participating at any time. You should be able to mute notifications in the bottom left of the post if it becomes bothersome. I don’t condone anyone insisting on help, so if someone continually bugged someone for assistance, we would deal with that individually. I don’t think that’s the case here though.

Personally, I’m a big fan of seeing the rough parts of the design process, as this is so often hidden behind companies. So yeah, I think this is a great topic, especially if @fritsjan continues to update the things he is trying and what is working, even without input from the community. The important thing about seeing the “rough parts” of the design process is also seeing some kind of resolution.


If there are measurement output issues, the radio waves are getting rectified at some point I’m guessing.

Have you selectively desoldered different parts of the device to see if that helps to eliminate the signal? Mostly I’m wondering if this happens when the load cells are desoldered?

Hi Chris,

Thanks for your feedback. Unfortunately I am not able to replicate the EMI since it only occurred during the testing at the special test institute. But I am going there tomorrow and this is good input. Now I can ask them to have a go without the loadcells attached and with. See if the problem lies there. Thanks!!

As for testing in proto stage. I totally agree. This is not how I normally would work. But unfortunately the whole project is not going as how I normally would have done it. The thing is that other parties are in play and changed timelines and even features. Which brings us here.

We now have a ‘small’ production going on of 250pc and only 50pc are build up yet. Mainly used for promotion and testing now. So we might fix the others with some quick fixes, learn from it and build the next batch with emi and esd in mind.

The only thing is that we all did not expect this to happen and maybe it is just bad luck with the wires being in the wrong place and acting as an antenna for both emi and esd.
This is also why I posted the question here to see if people with knowledge about this would potentially agree with this theory.

Anyways. Late now here, big day tomorrow. Hope to learn a bunch.
I will post my learnings asap.

It would be interesting to hear about your progress.

1 Like

Hi all,

You are absolutely right Rob. It has been some busy days for me.

I went to the testing expert and got a compact lecture about EMI and ESD.
It was very very informative. I got an insight in things which I always thought were the right thing to do to discover they were actually not.
I am thinking of a way to share all this information with you and how. Because to explain it well I probably should write a blog post about it or something and make some drawings to be really clear.

But let me try to make a summary here…

Please correct me if I am wrong or use the wrong technical terms :wink:


Electromagnetic interferance. It all has to do with magnetism.
Radio waves create a magnetic field and when a wire is placed in this field a current (I1) can run trough this wire.
There is always a return wire and also in this wire a current (I2) will be present, but in opposite direction.
Depending on how far apart both wires are, they lay in different strengths of the magnetic field. The one closest to the radio waves will have a higher current than the one further away. So you will end up with a remaining current I1-I2.

So one solution is placing the wires very close to each other so that I1 and I2 are almost identical.
Better is to twist the wires, so each wire lies in the opposite magnetic field for every twist.
This makes I1 and I2 exactly the same so you will have a result of 0

So one thing I had to do as @1.21Gigawatts pointed out was twisting the wires from the sensors.
This reduces a lot of interference on its own and actually was not really new to me.

But from here on this theory can also be applied to the PCB and this is interesting. Let me try to explain:


Lets say we have a double sided PCB. On the top we have 2 chips and a signal track between the 2.
Both chips are connected to GND and decoupled. The ground plane is on the bottom side.

Now how would the return signal go back to the first chip?

My guess was, the fastest way like this (via the GND plane of on the bottom of course)

Ehm wrong…
Apparently it takes the route of less flux resistance (or something like that, please correct me on the terminology)
It follows the upper track EXACTLY but on the bottom GND plane like this:

What? So directly I got this question on why we were thought to make separate analog and digital planes and stuff like star grounds…
Maybe this might be neccesary for very high frequency signals, but for ‘normal’ signals it appears that the ground return can handle itself :wink:


So why is this important? Remember the previous post about the twisted wires? The traces on a pcb are also wires.
In this case a pair of wires is the trace on top and the return is the path the return current flows through the GND plane.
In order to have a minimal effect of interferance, you want both ‘wires’ to be placed in the same magnetic field.
So if the return current follows the exact same path as the trace above it, this is (almost) the case. Just the distance to the GND plane difference (1.6mm or if the GND plane is in the middle of the PCB 0.8mm)
If this is not the case we create a loop and therefore a difference of the wires in the magnetic field and it becomes a receptor for interferance (read antenna).

In my next post there I explain how this can happen…


Now we put some more components on the PCB and of course we need to cross a track.
We go down to the ground plane make a track there and go up again:

Now we made an antenna! This is a drawing of an PCB antenna which can send a signal to a sattelite:

It just consists of a track and a cut out of the ground plane. With the size of the cut you can set the frequency…
The signal gets picked up in the track crossing the open ground plane. (in the previous picture, the track from top left to bottom right)

So this is very bad and also very very common!!

Now how to fix this?

Lets make a 4 layer PCB… We were thought we can use the inner layers for GND and V+ right?
Now lets put a component on the top and one on the bottom and connect both with a signal track:

Now how would the return signal go?
Following the tracks exactly?


The first part right bottom part of the track ‘sees’ the GND plane and the return signal follows the exact path of this track.
But the other part of the track is blocked by the V+ plane !! So it takes the other shortest route.

And now we are back to the theory of the wires and picking up magnetism. As you see the signal and return form a loop, the space between is big and therefore both paths will lay in a different magnetic field, different sizes of current will be picked up and not cancelled out. So noise will appear on this signal path…

So how to make a PCB which follows the rules:

  1. Make a GND plane in one of the inner layers.
  2. Do not interrupt this plane (near tracks)
  3. Trace all V+ as traces

To take the previous example and add a GND layer:

This eliminates the need for removing copper from the GND plane and therefore no antenna is formed, signals can just follow the tracks back on the GND plane.

So far for EMI now, I hope to find time for ESD later on


Hi to everyone, I have a question related to what yoiu Jan actually prepared here. The return signal can not go back in the V+ plane?, only in the ground plane? Thank you for you reply :"D