Noise Reduction

I have a PCB which utilizes a switching reg to charge two large caps to

350VDC. Unregulated battery power (6.4V-8.4V) is supplied to this board through a two pin connector. There is also another 4 pin connector through which the board gets a regulated source of power (3.3V) as well as 3 other signals of which one is a charge done signal.

I am having issues with noise on the signal lines when the charge cycle initiates. The noise is at its worst at the beginning of the cycle which seems to indicate it's related to di/dt (current tapers off as caps charge). The noise on the charge done signal occasionally triggers the interrupt prematurely (on another PCB to which the 4 pin connector is attached via 12" 24AWG conductor). Switching frequency is between 100kHz and 300kHz.

The board is 2 layers with the bottom layer serving mostly as a ground plane (a few signals running around). I believe I have a decent layout as far as the high current paths in the switching circuit. Everything is kept as tight as possible (given the large transformer required) and tied with large copper polygons (reducing inductance of traces).

I am revising the board and want to improve the noise situation. First thing I did was I added a RC network to the form a low pass filter right at the 4 pin connector. I suppose I could also use a LC combination. Is there a reason to choose one over the other? Second, and I am not sure this is actually beneficial, I made an L shaped slot to route the high currents in the ground plane back to the 2 pin connector. The thought was to keep those currents out from underneath the signals going back in the 4 pin connector.

Here is a rough image of the PCB layout

formatting link
I've marked up the signals in RED and the high current paths in YELLOW.

Any suggestions?

--------------------------------------- Posted through

formatting link

Reply to
eeboy
Loading thread data ...

This looks like a classic in-rush current problem. I'm guessing you have a boost mode regulator, so when the output caps are discharged (actually they'd be at your un-regulated input voltage) they'd be seen as a low impedance path. You probably need some kind of soft-start circuit to limit the current through the inductor until the output voltage has increased sufficiently. Do you have a schematic to post?

Mark.

Reply to
markp

In article , eeboy writes

LC's will give a sharper filtering effect against high freqs, however, I've noticed that the L's can couple magnetically to switching transformers so you end up with them actually introducing noise (at

100-300kHz in your case) if too near the switcher's transformer. Using a shielded L helps. Exactly what "too near" is depends on Stuff, but I'd try to keep them a couple of cm away at least. Looking at your board, next to the 4 pin filter sounds like a good position. I guess I'd go for an RC filter with a long time constant like 100 millisecs, if the processor at the far end can take such slow edges. To get that cutoff would need very large LC's so again, RC looks the way to go. Cheaper too.

I don't think the L slot is a good idea. The high currents will find their own optimised route and magnetic forces will herd the electrons along the most direct route home. But the L means your red tracks are no longer shielded by the ground plane over much of their length.

Assuming T2 is the transformer, I would not run the red tracks parallel to it but instead have them head radially away from it as soon as possible. This will reduce the energy that can be coupled into them by the magnetic flux changing across them.

From your yellow line it appears the high current switching IC is that

14 pin thing up near the top. Can you move it south to reduce the high current loop area?

The tracks to the pins of T2 (round thing in top right) look remarkably thin. You want big fat tracks to it.

It may be, that you need to reduce the noise coming out of the 2 pin connector. These days I tend to put common mode chokes on such inputs so they cannot conduct / radiate noise back along the incoming cable, which generally results in an EMC fail. Are the wires to the 2 pin connector twisted? That would reduce radiated mush a lot. Keep the signal and power wires apart if possible.

Does the 4 pin connector have its own 0V or does the signal rely on the

0V supply from the unregulated 2 pin supply? You might be getting ground bounce on a shared ground due to the high currents. This kind of problem can sometimes be solved simply by using thicker wire for the connectors.

Check the input reservoir capacitor for your switcher. It needs low impedance. Aluminium electrolytics are good these days (OSCONs are best unless you expect a large temperature swing).

--
Nemo
Reply to
Nemo

Ok, this has already been mentioned but it can really help: If you can afford the longer charge time do a current limit, or soft-start if this only happens upon turn-on or charge from zero.

That is not a surprise because one of the lines (highlighted red) is running really close to T2.

Suggestions: Get rid of the wide GND plane slit. Add GND pour under T2. Run the "red" lines straight back and not as a loop. If you must use a

2-layer do as much as possible on the other plane and only notch out small slits in the GND plane where you can jumper over with two vias and a trace snippet.

RC is great and cheaper but that depends on 3.3V power draw. On that line you may need an inductor. On signal lines you can use RC but always make sure that the digital input where they go to has hysteresis, IOW that it is an input with Schmitt behavior.

Well, other than the above it's all hard to tell sans schematic. You might want to hold a loop probe near T2 and see if it lets off any high-frequency ringout. If it does you could try a snubber but that'll need space because those dissipate.

A 4-layer would be really great to clean this up nicely. But I understand that this ain't always in the cards.

Interesting. I see they offer free membership. So where's the catch?

--
Regards, Joerg

http://www.analogconsultants.com/
 Click to see the full signature
Reply to
Joerg

through

other

which

I suppose I could PWM the 'CHARGE ENABLE' pin in the beginning to see if that helps. However, as you mention, obviously the charge time would suffer.

100kHz

as

kept

with

I posted a revised picture of the layout which shows top and bottom layers along with the top silk. Might be a bit more helpful. See..

formatting link

I removed the L slit from the ground plane. The reason I don't have a plane under T2 is I was afraid I would capacitively couple the high voltage spike. T2 is actually a trigger transformer with an output pulse of nearly

10kV for the triggering a xenon flash tube. With this information do you still recommend extending the ground plane underneath T2?

T1 is the flyback transformer. The high current path is J2+ to T1 primary to Q2 to R10 to GND. The physical size of the components prevents me from maintaining a tighter loop. I am also constrained in a few other areas... the two connectors are fixed, the large electrolytics are fixed due to their height, and the board outline is fixed.

right

this

currents

keep

R9 and C11 now provide a low pass on the 'CHARGE DONE' int signal returning. The

3.3V line is now really only used to pull up the 'CHARGE DONE' signal as the output of the IC is open collector. I suppose I can experiment with LC and RC combinations as they are both available in 0805 form.

the

I haven't experienced any 'catch'. It's certainly an inconvenience over having access to a news server. Unfortunately that is something my ISP doesn't provide.

--------------------------------------- Posted through

formatting link

Reply to
eeboy

through

other

as

kept

with

right

currents

Good point. Unfortunately no... and I kick myself because I had a chance to add a 5 pin connector and provide a reference from the board this connector goes back to.

I have a 100uF electrolytic and a 4.7uF ceramic hanging off this node at the input to the transformer.

--------------------------------------- Posted through

formatting link

Reply to
eeboy

Well, you could PWM it, then step on it and see how far you can push it until the tires start sqealing :-)

However, that's like taking pain pills all the time instead of finding out what really causes the pain.

Yes, but maintain enough isolation so nothing arcs. Since you have traces underneath C2 it seems there must be enough potting or other insulation on the transformer.

Not really. You would have a clear shot on the red layer, right through and underneath R3 -> R2 -> Q2. You might have to adapt the footprints a little but I've done stuff like that. Since they look like 0805 and a DPAK it should be easy. The large loop you have now is prone to pick up stuff.

If that's too spooky for you there is another more northern route: Over the top of R4 and C6, then through the middle of TP6 and on towards the west through the middle of R10 which is a big resistor with tons of center clearance.

With both routes you don't have to cut into the GND plane at all.

There's also two traces in red north of R10 which I'd tuck through the center of R10. Plenty of space.

That would be no problem. If you don't want to go underneath the parts can you make this a 4-layer? But I'd try the "tunnel" first.

But make sure the uC or whatever is connected has Schmitt inputs.

Probably they live off of the revenue from the advertising links on the top of the pages.

My ISP (AT&T) ditched all of Usenet last year. So I signed up with an independent newsserver in Germany (news.individual.net). It costs 10 Euros (about $14) per year and so far it works great.

--
Regards, Joerg

http://www.analogconsultants.com/
 Click to see the full signature
Reply to
Joerg

P.S.: When you route sensitive traces think about magnetic coupling. For example, R10 looks like a current sense resistor so it will probably carry serious current spikes. Lines parallel to it pick that up to some extent. IOW, parallel = not good, perpendicular traces = better.

Same with T2. The line that comes from R11 parallels it on the west side. If T2 is wound around a core that's standing up this will couple, big time. If you shoot off perpendicular like I suggested in my previous post you should see a nice improvement.

--
Regards, Joerg

http://www.analogconsultants.com/
 Click to see the full signature
Reply to
Joerg

...

eternal-september.org access is free, but no binaries.

My ISP still offers nntp but it's unreliable.

Grant.

--
http://bugs.id.au/
Reply to
Grant

You can get free abse here.

formatting link

Reply to
Hammy

Assuming there is no other connection between bulk power and signal lines, cut the plane between the two connectors, and rejoin the 4pin signal ground at a power ground point nearer the signal source.

RL

Reply to
legg

There are several free ones but I've heard that some have become spam sources and are thus often blocked by others, and some aren't too reliable. I don't know about eternal-september though. The newsserver I am using right now is very reliable, has pretty stiff restrictions that make spamming difficult yet doesn't interfere with normal newsgroup usage, and at 15 bucks a year I won't complain about the cost :-)

--
Regards, Joerg

http://www.analogconsultants.com/
 Click to see the full signature
Reply to
Joerg

Thanks for that link!

Mark.

Reply to
markp

to

board

cycle

which

100kHz

Is

a=20

for=20

keep

the

no=20

=20

=20

=20

so=20

which=20

=20

ground=20

problem=20

connectors.

to

connector

=20

Try adding about 20 to 50 nF, low ESR in parallel with those two and pay=20 attention to placement.

Reply to
JosephKK

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.