Layout review: Inverting buck converter

[strobot]

Hey Bertho, -8.2 V is actually the correct voltage since I'm using different feedback resistors than the schematic.  R2 = 10K and R1 = 1.02K should yield Vout = -8.265 V.

The diode is a Diodes Inc. B260A-13-F

L1 is a Taiyo Yuden NR6045T150M with max DCR of 77 mOhm.

I'll stack another 0.1uF on C1.

Going to check on the sine wave.  The load is a 144R resistor - will test with different loads.

Will repost more informative scope images.

[senso]

Thanks about the information about the top planes, didn't know that, and usually I base my designs from the eval boards gerbers(when given by the manufacturer) and they always use top and bottom ground pours, but I will follow your advice, thanks 

[Bertho]

As for the diode, I think you should use something like DB2W40200L. The reverse recovery time is very important and should be as short as possible. The B260 has not even specified it in the datasheet and it has a capacity of ~200pF. It may be good for low-frequency switchers, but for 1MHz+ it is not good enough.

Coil looks fine and has nice low DCR and saturation at ~2.3A. The self-resonant frequency is at ~10MHz. Can you blow up the switch-noise and see if it looks like a 10MHz signal? It may be the coil's resonance showing in the noise.

[strobot]

OK, thanks for the info on the recovery time of the diode.  I understand how reverse recovery time can be so important at 1 MHz+.

The sine wave must be coming from the circuit somehow.

This is the scope of the disconnected benchtop power supply.  Its a BK Precision 1610A.  Not sure where that burst noise is coming from.


I swapped in a 9V battery and there is no measurable noise (with my scope) on the outputs when its disconnected.


Scoped the input with the battery attached running the combined 144 ohm load.  (10K and 147R in parallel).


Switch timing images coming up...

[Bertho]

Ok, that could be from the input capacitors and wiring.

I read the frequency wrong the first time. It is ~1/(0.8*200ns) ~= 6.25MHz. I suggest you add one or two 0.1uF (X7R or the like) to the input capacitors to see if it comes from there. These high frequencies are very persistent and are a bit awkward to get pinned down.
Can you also float the probe, without touching the circuit, over the board and wiring? See if this signal is radiated. It may be picked up by the probe and you may be able to detect where it originates.

Your power feed exhibits a resistance of ~0.3Ohm (extrapolating from the ripple). You may want to add a 47..100uF low esr aluminium cap on the input. A much better input cap would be a 47uF aluminium organic polymer capacitor.

[strobot]

Hey Bertho - thanks for the guidance again!

I soldered a 0.1uF X7R across the input pins and also on top of the 10uF filter cap.

I tried floating the probe over the board and am able to pick up a square wave clearly near the switching node and inductor, but I didn't see any sign of our sine wave. 

I measured the switch node square wave ringing to be around 80 MHz.

I tried measuring the switch node and outputs simultaneously, but connecting the probe tip to the switch node copper caused switching noise at the output to increase dramatically.

VIN at battery terminals


VIN at circuit terminals - square wave is probably from radiated EM at switchnode.  Square wave amplitude was sensitive to scope probe orientation even using the pokey ground lead.


VO1


VO2

[Bertho]

Nice. Your images confirm that the sine originates from the input. I think it is generated from the battery leads ending up as a transmission line. The small capacitors clearly reduce the oscillation amplitude and, if I see it correctly, then the sine is now slightly damped over time.

I am convinced that you need a better input capacitor. The ceramics are not cutting it. An organic polymer with some smaller ceramics is the way to go. The input impedance should be low and the current spikes need to be dampened more effectively at the input.

The switch-node ringing will probably be reduced with a better diode. My guess here is that the diode allows for a resonant swing when it is turning off.

To get rid of the switch induced EMI, you need a HF shielded probe; not the easiest to get. Probes have the problem that the ground-connection (in the cable) is part of the current-loop to the scope connection, thereby sensitive to induction. FWIW; If you are really in for some hackery... You can reduce the induction by wrapping the probe and probe-cable in alu-foil (not touching gnd/live pins) and then adding a wire from that shield to the GND plug on the scope. It is important that the shield in not carrying any current. This is a bad hack and influences the probe's characteristic, but can help to reduce externally induced noise.

But then, you are are at ~20mV p-p noise and ~2mV ripple at the second output. That is a very good result for a switching power supply.

[Bertho]

I tried measuring the switch node and outputs simultaneously, but connecting the probe tip to the switch node copper caused switching noise at the output to increase dramatically.

You probably caused a ground-loop while connecting two probes' grounds. It is a real pain to connect multiple probes in these designs; a really bad pain.

[strobot]

Alright, cool.  I've tried to take all your suggestions into account. 

I made the LC filter with the same 15uH that was used in the converter with a 10uF after it.  The resonant frequency should be about 18.4 KHz taking into account the 50% derating of the 10uF capacitor.

Schematic:


BOM:  Any suggestions for lowering the BOM cost?  I am going to try replacing the 47uF X5R 10V 1210 caps with several 10uF X5R 25V 1206 caps, since the 47uF ceramics are pretty expensive (about $1.50 in single quantities vs $0.35 for the 10uF 25V)

https://docs.google.com/spreadsheet/ccc?key=0AlUlVoMq1FqldDZLMEo2U3FPSzdDckxWZjVLMWdpbXc#gid=0

[Bertho]

I made the LC filter with the same 15uH that was used in the converter with a 10uF after it.  The resonant frequency should be about 18.4 KHz taking into account the 50% derating of the 10uF capacitor.

That should be fine.

I do suggest that you add at least a 0.1uF at the first filter stage. You only have 3x10uF at the moment and you really want to take part of the HF out at that stage.

BOM:  Any suggestions for lowering the BOM cost?  I am going to try replacing the 47uF X5R 10V 1210 caps with several 10uF X5R 25V 1206 caps, since the 47uF ceramics are pretty expensive (about $1.50 in single quantities vs $0.35 for the 10uF 25V)

Organic polymer caps are expensive, especially for 1MHz+ switchers as most of them have an ESL that makes them inductive at those frequencies. So, as output capacitor it is not always a good choice. As input capacitor they are a good choice if properly decoupled with ceramics (f.x. 47uF/10V polymer with a 10uF/25V+0.1uF/50V ceramic).

Replacing the 47uF ceramic with 5x10uF is fine and should not give you any problem. Mouser 963-TMK316BJ106KLHT is ~$0.15 @10 pcs. so you can replace them all with the same ceramic and get advantage of the larger quantity.

[strobot]

Roger on the additional 0.1uF. 

How does this look?

[Bertho]

Roger on the additional 0.1uF. 
How does this look?

Well, it looks very stylish 

You may want to extend the access to the +9V input on the right a bit. The input should hit the big cap first and it seems to me you have a problem attaching right now.

The only thing I see is that you changed the grounding plan a bit. I do not know if that has any influence. The ground-impedance should be low enough as not to have any significant effect.

The question will be if you see a difference when you are using both +V and -V supplies further on in the design. The advantage of the big grounding (as you have now) is that it creates a better global reference. It still matters where you reference it from later on. In that respect, I think you may want to add a lower trace (at the bottom) to extend the V+ input to the left (taken from C2) and add the same secondary and tertiary filters in the space on the lower left for V+. It would create a perfect symmetry and you have filtered output of both plus and minus supply nicely together with a perfectly center ground reference.

[Paul Price]

You have the input battery negative terminal connected to the positive output.  This is wrong. It should connect to the ground pin of the switcher IC. This means that the 9V battery will float, but you are not using the 9V battery to power anything else..correct?

You really have been led down a primrose path with all this layout trimming when your basic power input connections to the LMR14206 IC are wrong.


To correctly view the output of a switcher like this, make a tight twisted pair of insulated wire and connect to the output, then connect the scope leads to the twisted pair ends several inches away from the board using symmetrical ground and probe point lead lengths. This will eliminate any magnetically coupled pulse from being picked up from the switching inductor while giving you a clean view of the output voltage.

[Paul Price]

You would do much better in eliminating most of all those ceramic filter caps and use a low ESR, low-profile standard aluminum electrolytic cap shunted by a single ceramic cap. on the input power and output power points.  Adding a small (20 to 150uH) choke bypassed by a small low-profile electrolytic will further decouple the neg. output and would lower any remaining noise to almost nothing visible. If you add a filtering choke inductor take care to place it so it does not magnetically couple with the power switching inductor.  This looks very easy since the picture of your board show the switching inductor is well magnetically shielded.

Your board is bloated by all these excess ceramic caps.

There are many types of ceramic caps and you can get ceramic cap types  that do not have a high negative coeff. of voltage.

[lgbeno]

Loop inductance of the feedback node is the most sensitive part of any power supply.  I think it would be better to shift the c6-c9 down to be inline with r1 and r2.  Also I assume that there is a via terminating r1 to gnd.  You need to consider the length of the current path of this net back to the IC pin including the vias. 

All of the filters in the world cannot fix a feedback inductance problem...

Also wrt to mr price's comment, I'm also having trouble mapping the layout to the schematic.

A word on ground pours and "ground loops". A ground pour is a way to ensure that current finds the lowest path of impedance.  If you force current to flow down a path it might not be to lowest impedance.  I think a best practice is to pour the top and bottom and stitch them together with ample vias.  You can look at you pours afterwards and look for little peninsulas and islands that may exist in the pour and selectively eliminate them as they can become radiating structures.  With all things EMI, "it depends". But in my opinion there is such a focus on adding impedance with series filters and ferrite beads, better to focus on lowering the impedance of return currents to the source.

[Paul Price]

http://www.digikey.com/product-detail/en/UMA1A330MDD/493-5944-ND/2598615

cost each small quan:  22 cents US

[strobot]

Thanks for the commments, Paul and lgbeno, but the converter IC is not wired incorrectly.

Using a buck converter in an inverting buck-boost topology
http://www.ti.com/lit/an/slyt286/slyt286.pdf

To implement the buck-boost topology of Figure 2, the buck-converter ground pin is connected to VOUT, and the positive lead of the output capacitor is connected to ground.

The converter's feedback is positive with respect to the converter's ground, so it has to be this way.

Designing an Inverting Buck Boost Using the ADP2300 and ADP2301 Switching Regulator
http://www.analog.com/static/imported-files/application_notes/AN-1083.pdf

This means that the 9V battery will float, but you are not using the 9V battery to power anything else..correct?

The positive terminal of the battery is the positive rail for the opamps.

To correctly view the output of a switcher like this, make a tight twisted pair of insulated wire and connect to the output, then connect the scope leads to the twisted pair ends several inches away from the board using symmetrical ground and probe point lead lengths. This will eliminate any magnetically coupled pulse from being picked up from the switching inductor while giving you a clean view of the output voltage.

Awesome! Thanks for the tip, I'll have to try this.

You would do much better in eliminating most of all those ceramic filter caps and use a low ESR, low-profile standard aluminum electrolytic cap shunted by a single ceramic cap. on the input power and output power points.  Adding a small (20 to 150uH) choke bypassed by a small low-profile electrolytic will further decouple the neg. output and would lower any remaining noise to almost nothing visible. If you add a filtering choke inductor take care to place it so it does not magnetically couple with the power switching inductor.  This looks very easy since the picture of your board show the switching inductor is well magnetically shielded.

I was worried about ripple current in the electrolytics, which is why I shied away from them initially.  If the ripple current is handled by the ceramics, that makes sense.  Would the higher ESR of the electrolytics dampen the transmission line effects I was seeing?

[Paul Price]

The input power connections are wired wrong. You are not implementing an AD2300 IC. I have some doubt that the LMRxxxx IC would operate  the same as the AD2300. You can easily verify this by changing the battery connections as I recommend(op-amp circuits disconnected.)

 Of course, the output positive lead must be the ground, but the negative for the battery must be at the ground pin of this switcher IC you are using. This is why you are seeing odd voltages and ripple.

It is obvious you need another battery here or a different converter configuration/chip if you want to also power the positive rail for the op-amps.

A low ESR aluminum electrolytic capacitor will have no problem dealing with these rather low currents and offers low ESR at low to high frequencies. Adding a single additional ceramic cap (.1uF, for example) will take care of any higher frequency noise (>1 MHz).  I urge you to try the low-ESR aluminum cap. in your circuit and you will see that you do get the results I mention.

[Bertho]

You would do much better in eliminating most of all those ceramic filter caps and use a low ESR, low-profile standard aluminum electrolytic cap shunted by a single ceramic cap. on the input power and output power points.  Adding a small (20 to 150uH) choke bypassed by a small low-profile electrolytic will further decouple the neg. output and would lower any remaining noise to almost nothing visible. If you add a filtering choke inductor take care to place it so it does not magnetically couple with the power switching inductor.  This looks very easy since the picture of your board show the switching inductor is well magnetically shielded.

I was worried about ripple current in the electrolytics, which is why I shied away from them initially.  If the ripple current is handled by the ceramics, that makes sense.  Would the higher ESR of the electrolytics dampen the transmission line effects I was seeing?

The use of aluminium caps at 1MHz+ switchers have the problem that their ESL will get in your way, making them less effective. Even most polymer caps will become inductive at 1MHz+ frequencies and therefore less suited as output capacitor. The point in this design, as far as I am aware of, is to create V+/V- suitable for analog electronics. That means to ensure proper switch dampening. For that, ceramics are better suited than aluminium caps with this particular switcher.

Actually, you can buy aluminium and polymer caps for the higher frequencies, but they are more expensive. There is no need for high capacity values and therefore, again, ceramics are a better choice, even if you need a couple more of them.

The input capacitor has some slightly different use in this design. With a battery fed system, your input power supply has rather high impedance. The switch noise will be taken by the ceramics, but the bulk-impedance depends on the polymer cap, such that your battery is loaded quite evenly at a rather constant DC current level. A "good" aluminium cap has an ESR in the range of 150..300mOhm; your battery is in the order of 100..500mOhm and a polymer cap is in the order of 30..80mOhm. Ceramics have the very steep V*C product problem whereas  polymer caps are less dependent on it, so it is the better choice.

Loop inductance of the feedback node is the most sensitive part of any power supply.  I think it would be better to shift the c6-c9 down to be inline with r1 and r2.  Also I assume that there is a via terminating r1 to gnd.

The high-current path is mainly perpendicular to the feedback node so the problem is rather small. I do agree that the feedback connection can be pulled back a bit farther from under the first cap to reduce the potential coupling there.

[Paul Price]

Using analog circuits does not mandate that the main power supply be absolutely clean in output. Op-amps suitable for low-noise application have high power supply noise rejection.

In my years of design experience, low ESR aluminum caps bypassed by a ceramic cap do an excellent job in almost all analog circuits. Low enough ESR aluminum caps are neither hard to find nor expensive.

Of course, testing a circuit prior to designing a PCB and testing using a prototype PCB will verify that these assumptions are correct.

[strobot]

The input power connections are wired wrong. You are not implementing an AD2300 IC. I have some doubt that the LMRxxxx IC would operate  the same as the AD2300. You can easily verify this by changing the battery connections as I recommend(op-amp circuits disconnected.)

 Of course, the output positive lead must be the ground, but the negative for the battery must be at the ground pin of this switcher IC you are using. This is why you are seeing odd voltages and ripple.

This makes no sense to me.  The entire purpose of an inverting buck/boost configuration is to generate a negative supply from a positive voltage source, i.e. the battery.  The Texas Instruments app. note describes generally how to implement the inverting buck/boost topology using normal buck converter ICs.  There isn't some special feature that the AD2300 has that makes it work in the inverting buck/boost topology.

It is obvious you need another battery here or a different converter configuration/chip if you want to also power the positive rail for the op-amps.

I don't really know what to say.  I think you're missing the point of this circuit.  My application needs to run off a single battery and generate a bipolar supply.

Here is yet another Texas Instruments app. note that describes how to use a run-of-the-mill buck converter to generate a negative voltage from a positive input voltage source.  VIN is positive, the converter GND-pin is connected to the negative output, and the positive end of the output capacitor connects to the system GND.
http://www.ti.com/lit/an/slva257a/slva257a.pdf


I've built the inverting supply and it works.  I'm able to power op-amps with V+ coming from the positive terminal of the battery, GND referenced to the battery's negative terminal, and V- coming from the inverting supply output.

In my years of design experience, low ESR aluminum caps bypassed by a ceramic cap do an excellent job in almost all analog circuits. Low enough ESR aluminum caps are neither hard to find nor expensive.

I am more than willing to try out aluminum caps shunted with ceramics on the input/output, though, and appreciate your suggestions concerning them.

[Paul Price]

I would confidently guess that C3 in figure 3 of the TI circuit could be a low-ESR aluminum electrolytic, and this cap is sufficient to create a low-noise filtered output even without further HF bypassing with a ceramic cap. I also see that the C1 and C4 10uF input caps effectively further bypass power input to the IC ground pin.

Every IC can have its own personality, but If you find that the grounded positive output works with the LMRxxx device as well as with a direct connection to the negative term. of the battery, no one can argue with success.

Notice that the large uF value of  C3 functions to keep the battery ground closely connected with a low reactive impedance to the device ground return pin of the IC.

[strobot]

I have some spare Nichicon UCD1E221MNL1GS 220uF 25V low Z caps that I could try.  Will post results.

Just for reference, here is the noise from the TPS5430 as an inverting buck/boost converter in the TI app. note.  It uses a single 10uF 25V X7R on the input, another 10uF across VIN & VOUT, and a single 220uF 10V POSCAP (tantalum with conductive polymer) on the output.  The circuit Bertho has helped me design has performance at VO1 (before LC filter) that surpasses the TI EVM in terms of ripple and noise (see post 23).

http://www.ti.com/lit/ug/slvu243/slvu243.pdf
http://www.ti.com/lit/an/slva257a/slva257a.pdf


VO1


VO2 (after LC filter)