EEVblog #859 - Bypass Capacitor Tutorial

[uncle_bob]

How about using a 50 Ohm to 0.1 Ohm RF transformer connected to a test point on the board and use a directional coupler to look at the return loss in a frequency sweep?

Hi

Ok so now we need a broadband 50 ohm to 0.1 ohm transformer ... hmm ... check Mini Circuits .. .not so much.

Assuming you built such a beast, you would find that it is surprisingly narrowband. Getting a couple decades of "good response" only happens if you have a fairly liberal interpretation of "good". If you want to check over as many decades as a modern board is likely to need, you will have to do a *lot* of transformers.

Next step is to calibrate both the transformer and the directional coupler. That involves "known good" standards at least for short / open / and load. Open always has issues on any calibration setup. Maybe a bit less so here. Short needs to be a short to << 0.1 ohms. That is true both in terms of absolute impedance and phase (non reactive). Your 0.1 ohm standard ... lots of fun.

Now we need to connect those standards to the output of our test rig. Each standard needs to be connected in turn. Each needs to have the same "reference plane" as the others. APC-7 connectors take care of part of this at 50 ohms. Grab the catalog .. no 0.1 ohm connectors listed at DigiKey. Same thing with 0.1 ohm cable. Connector and cable impedance is a function of a few things, one is inner conductor diameter as a percentage of the inside of the outer sheath. For 0.1 ohms ... errr ...  So we parallel a few cables we can get.... gee that's a lot of cables ...

No that's not the whole story, but you probably get where this is leading off to.

It's far more common to measure at a few spot frequencies and maybe over the top decade / octave than to sweep the entire board accurately. It's even more common to "try it and hope (maybe based on modeling)" than to measure a board before there is a problem.

Bob

[Ampere]

Great bypass cap tutorial. I learned a lot.

[T3sl4co1l]

Er, well, you don't need to be taking 0.1 ohm out for a walk... just put it right there on the fixture.  It'll all be hand made, and the transformer secondary will be a short 'C=' section of copper foil, the '=' being a wide, thin parallel plate transmission line.  Primary (and core) fits inside the 'C', maybe using a pot core?

What's more, 0.1 ohms is pretty arbitrary; 1 or even 10 ohms would still improve sensitivity without making things so aggressive.

I've used matching transformers in this range for induction heating applications; you get bandwidth to a few MHz, which is more than enough for typical purposes.  An optimized design might struggle to achieve under 1 ohm beyond 100MHz, but I suppose that would still be good enough here.

Tim

[jnissen]

Most of the comments to date have been accurate and on target. I did do quite a bit of system level analysis in a past life with various IBIS modeling packages to predict resultant signal integrity. One of the better ones was Sigrity's tool flow. Used real package parasitics in addtion to the board file and localized decoupling. Could get you fairly close to real on die power droop and resultant signal integrity effects. Was insightful and provided fairly good results.

Now that I do on die work I have always kept those analysis limitations in the back of my mind. The fundamental take away is that you have to have a local on die source of decap in high di/dt loading environments to overcome the limitations in the power delivery network of the package and board.  I do significant sims to ensure that our package model parasitics can be overcome with on die decoupling. Sometimes the loads are just too fast and large that is nearly impossible to achieve enough on-die decoupling and in those cases you can attack the problem at the source. Perhaps re-architect your drivers and limit edge rates where appropriate.

[T3sl4co1l]

Now that I do on die work I have always kept those analysis limitations in the back of my mind. The fundamental take away is that you have to have a local on die source of decap in high di/dt loading environments to overcome the limitations in the power delivery network of the package and board.  I do significant sims to ensure that our package model parasitics can be overcome with on die decoupling. Sometimes the loads are just too fast and large that is nearly impossible to achieve enough on-die decoupling and in those cases you can attack the problem at the source. Perhaps re-architect your drivers and limit edge rates where appropriate.

Hello,

Do you work with digital / logic, or PMIC as well?  I have a question about integrated switching regulators, if you've worked on 'em.

Tim

[uncle_bob]

Er, well, you don't need to be taking 0.1 ohm out for a walk... just put it right there on the fixture.  It'll all be hand made, and the transformer secondary will be a short 'C=' section of copper foil, the '=' being a wide, thin parallel plate transmission line.  Primary (and core) fits inside the 'C', maybe using a pot core?

What's more, 0.1 ohms is pretty arbitrary; 1 or even 10 ohms would still improve sensitivity without making things so aggressive.

I've used matching transformers in this range for induction heating applications; you get bandwidth to a few MHz, which is more than enough for typical purposes.  An optimized design might struggle to achieve under 1 ohm beyond 100MHz, but I suppose that would still be good enough here.

Tim

Hi

We obviously work on different things. The stuff I work on barely starts at 1 MHz and the planes need to be low impedance to well past a few GHz to be useful.  Is that 0.1 ohms or something else? The 0.1 came from an earlier set of posts.

Bob

[apis]

It's funny how often a lot of theory in practice boils down to "try and see what works". It's like when you take a statistics course with a lot of calculus and algebra and in the end the most important result is that the arithmetic mean is a good estimate of most things. But anyway, a great video and lots of great comments.

[nctnico]

Er, well, you don't need to be taking 0.1 ohm out for a walk... just put it right there on the fixture.  It'll all be hand made, and the transformer secondary will be a short 'C=' section of copper foil, the '=' being a wide, thin parallel plate transmission line.  Primary (and core) fits inside the 'C', maybe using a pot core?

What's more, 0.1 ohms is pretty arbitrary; 1 or even 10 ohms would still improve sensitivity without making things so aggressive.

I've used matching transformers in this range for induction heating applications; you get bandwidth to a few MHz, which is more than enough for typical purposes.  An optimized design might struggle to achieve under 1 ohm beyond 100MHz, but I suppose that would still be good enough here.

Tim

We obviously work on different things. The stuff I work on barely starts at 1 MHz and the planes need to be low impedance to well past a few GHz to be useful.  Is that 0.1 ohms or something else? The 0.1 came from an earlier set of posts.

The 0.1 Ohm is just a number to get some meaningfull results by injecting enough current into the DUT and perhaps there are better ways of making some kind of probe. Ofcourse it isn't going to be as easy as putting some wire on a core and attach a bunch of long wires/cables to it. Anyway you need to keep in mind that checking the behaviour of a power decoupling system isn't going to be exact science anyway so if you want to determine whether there is excessive peaking or not over a certain frequency range you could use a crude tool for a ball-park estimate. Ideally you'd need to have all the power rails at their operating voltages to include the effect of voltage dependant capacitance changes.

[uncle_bob]

Er, well, you don't need to be taking 0.1 ohm out for a walk... just put it right there on the fixture.  It'll all be hand made, and the transformer secondary will be a short 'C=' section of copper foil, the '=' being a wide, thin parallel plate transmission line.  Primary (and core) fits inside the 'C', maybe using a pot core?

What's more, 0.1 ohms is pretty arbitrary; 1 or even 10 ohms would still improve sensitivity without making things so aggressive.

I've used matching transformers in this range for induction heating applications; you get bandwidth to a few MHz, which is more than enough for typical purposes.  An optimized design might struggle to achieve under 1 ohm beyond 100MHz, but I suppose that would still be good enough here.

Tim

We obviously work on different things. The stuff I work on barely starts at 1 MHz and the planes need to be low impedance to well past a few GHz to be useful.  Is that 0.1 ohms or something else? The 0.1 came from an earlier set of posts.

The 0.1 Ohm is just a number to get some meaningfull results by injecting enough current into the DUT and perhaps there are better ways of making some kind of probe. Ofcourse it isn't going to be as easy as putting some wire on a core and attach a bunch of long wires/cables to it. Anyway you need to keep in mind that checking the behaviour of a power decoupling system isn't going to be exact science anyway so if you want to determine whether there is excessive peaking or not over a certain frequency range you could use a crude tool for a ball-park estimate. Ideally you'd need to have all the power rails at their operating voltages to include the effect of voltage dependant capacitance changes.

Hi

Ok, we do (on average) a board a week. Doing a full blown measurement of that board (with all the calibration) is about six months per board. Yes, both are man hours. So off we go to the finance barons and say "we need to increase our board design costs by 24X". We then go to sales and say "we need to do a board / measure a board / redo a board" for each design. That will take the design process (and our delivery) out by ??X. Neither group is exactly what I'd call "happy".

Bottom line, the money you save with a fancy / validated design (it needs 3 less caps) is a bit tough to sell up front. Overkill is a lot cheaper / faster / easier / more normal and it works.

Bob

[nctnico]

I'm not quite sure where you are getting at. Do you expect to need 6 months to measure a board or are you currently needing 6 months to test a board?

[uncle_bob]

I'm not quite sure where you are getting at. Do you expect to need 6 months to measure a board or are you currently needing 6 months to test a board?

Hi

If you are going to do all that is involved in testing a board over a wide range of frequencies, it will take a long time. The last time I went down this road, 6 months was an overly optimistic time span for doing it. If you did it full time and already had some setups, you probably could do a full (measured) characterization of a board in 6 months.  That's an un-acceptable amount of time when compared to the design process that I'm familiar with.

Again, this is on fair sized boards that are running multiple rails, some at voltages like 1.2 or 0.9. Currents in the couple amps to tens of amps are not unusual. They have significant energy running around well into the 10's of GHz range. There's noting terribly crazy about them. They are running fairly normal FPGA's and DSP stuff. The internal edge rates of this stuff (and thus the current spike widths) can be amazingly fast. The current all comes from the power plane ...(not quite correct, but close).

Bob

[T3sl4co1l]

Er, well, all that nastiness is handled on the die, even. Large power planes occupy at least a few metal layers; some transistor junctions also serve to bypass those nearby.  In the GHz, caps on the interposer handle transients that the PCB couldn't possibly handle directly.  PDN bandwidths are only in the 100MHz range.

Tim

[uncle_bob]

Er, well, all that nastiness is handled on the die, even. Large power planes occupy at least a few metal layers; some transistor junctions also serve to bypass those nearby.  In the GHz, caps on the interposer handle transients that the PCB couldn't possibly handle directly.  PDN bandwidths are only in the 100MHz range.

Tim

Hi

Wish that was true .... If it's a chip scale part, your are straight into the die.

Bob

[Fungus]

I'm not quite sure where you are getting at. Do you expect to need 6 months to measure a board or are you currently needing 6 months to test a board?

If you are going to do all that is involved in testing a board over a wide range of frequencies, it will take a long time. The last time I went down this road, 6 months was an overly optimistic time span for doing it. If you did it full time and already had some setups, you probably could do a full (measured) characterization of a board in 6 months.

What would it achieve, exactly? What would be the benefit over the quick-and-dirty techniques?

[uncle_bob]

I'm not quite sure where you are getting at. Do you expect to need 6 months to measure a board or are you currently needing 6 months to test a board?

If you are going to do all that is involved in testing a board over a wide range of frequencies, it will take a long time. The last time I went down this road, 6 months was an overly optimistic time span for doing it. If you did it full time and already had some setups, you probably could do a full (measured) characterization of a board in 6 months.

What would it achieve, exactly? What would be the benefit over the quick-and-dirty techniques?

Hi

You *would* know what the board actually did.

It's expensive / complex enough that there really is little call to do it. With low voltage / high currents the impedances are indeed pretty low. The frequency ranges are quite wide .... it's a royal pain.

Bob

[T3sl4co1l]

Ew, unit typoes...

But yeah, your clues are here: "General Purpose", so you know they're going to be shitty, and "Dissipation Factor" (~0.2).  If that's measured at 120Hz (typically the case), then a 100uF capacitor has a reactance of 13 ohms and ESR of 2.6 ohms.

And no electrolytic in history has ever been rated for kiloamperes.

Tim

[David Hess]

I've even read about people demanding from manufacturers high ESR caps, or trying to spoil the resonances with series resistors.

I've seen series resistors added. You must be pretty desperate to have to do that.

I have seen some designs go a step beyond adding series resistance to increase the ESR.  Instead they selected a value of decoupling capacitance and adjusted the length of the traces so that the low impedance series resonate frequency was located on top of a troublesome switching harmonic.  In this way they could notch out various harmonics generated by the clocking of the digital logic or switching power supply.

[David Hess]

If making ceramic capacitors "sideways" makes them less inductive, why aren't all low voltage, high value ceramics made that way?

The greater force from the surface tension of the solder and the lower force from gravity makes the part more likely to suffer a failure.

[David Hess]

I've even read about people demanding from manufacturers high ESR caps, or trying to spoil the resonances with series resistors.

I've seen series resistors added. You must be pretty desperate to have to do that.

Not really. Linear regulators dont like low ESR, or some voltage reference noise reduction pins dont like low ESR. slyt339 from TI for example explains this.

Agreed, decidedly not desperate. I've done it quite a lot when I wanted something in the form factor of a MLCC but with high DF. That's not a bad thing, it's something that's quite often desirable. Hence why we even have a name for it in certain applications: "snubber"

Audio amplifiers commonly require a series RC network for stability which illustrates what is going on in a more visible manner.  Some comparators can be used as operational amplifiers if a suitable RC snubber is added to their output.  Some seemingly intractable operational amplifier oscillation problems can be solved by adding a large high ESR output shunt capacitance.

The RC network whether the R is part of the ESR or provided as a separate component is part of the frequency compensation network.  Lower performance "high dropout regulators" with their emitter or source follower outputs have a low impedance so they are more tolerant of low ESR output capacitors than high performance "low dropout regulators" with their common emitter or source follower outputs which have a relatively high output impedance.  You can still make a high dropout voltage regulator oscillate under the proper conditions though; the common old 7805 and 7905 linear regulator application notes show a low ESR decoupling capacitor at the input and *only* a small high ESR bulk capacitance at the output.

Switching regulators have all of the same problems and can also be made to oscillate if the output ESR is too low.  There is a trade off between output ripple and feedback loop stability.

A bode plot which includes the output RC network can be very informative.  I have occasionally varied the output capacitance and ESR while measuring their effect in order to derive unknown aspects of the of the feedback network using a bode plot.  A network analyzer could always be used to measure it directly but one is not always convenient.

I usually try to put at least one chunky, lossy capacitor on every rail, it can go a long way to damp resonances.

This is a common brute force solution.  It becomes fun when you want to determine how little capacitance you can get away with or how much design margin is present.

[VanitarNordic]

What types of bypass capacitors must be used?

All should be ceramic?

[Fungus]

What types of bypass capacitors must be used?

All should be ceramic?

For TTL circuits? Yes. Speed is essential.

Electrolytic are much too slow, ceramic are in a good place on the fast/cheap graph.

[VanitarNordic]

What types of bypass capacitors must be used?

All should be ceramic?

For TTL circuits? Yes. Speed is essential.

Electrolytic are much too slow, ceramic are in a good place on the fast/cheap graph.

Not just TTL, for any digital or MCU based circuit which might accompany analog parts or analog ICs such as Opamp. If we gonna use 3 capacitors, I was thinking to use tantalum for the biggest one (1uF). what do you think?

10nF and 100nF => ceramic
1uF => tantalum

[T3sl4co1l]

What types of bypass capacitors must be used?

All should be ceramic?

For TTL circuits? Yes. Speed is essential.

Electrolytic are much too slow, ceramic are in a good place on the fast/cheap graph.

Slow in what sense?  Is an electrolytic with approx. equivalents C = 100uF, ESR = 0.5Ω and ESL = 3nH "slow"?  (Hint: it'll probably outperform most recommended combinations of ceramics!)

The RC time constant is a small part of the story.  Typically, the layout is a bigger part!

Tim

[T3sl4co1l]

Not just TTL, for any digital or MCU based circuit which might accompany analog parts or analog ICs such as Opamp. If we gonna use 3 capacitors, I was thinking to use tantalum for the biggest one (1uF). what do you think?

10nF and 100nF => ceramic
1uF => tantalum

Stacking up different value ceramic caps is foolhardy.  Normally, it makes things worse.  No one realizes this, because no one tests this!

Tantalum are generally safe from an impedance standpoint, but 1uF may be too small, in that its ESR will be too high to be beneficial.  Tantalum are also unsafe on high current power supplies -- they tend to catch fire.

Tim

[David Hess]

What types of bypass capacitors must be used?

All should be ceramic?

Electrolytic are much too slow, ceramic are in a good place on the fast/cheap graph.

Slow in what sense?  Is an electrolytic with approx. equivalents C = 100uF, ESR = 0.5Ω and ESL = 3nH "slow"?  (Hint: it'll probably outperform most recommended combinations of ceramics!)

But it will be unlikely to outperform a combination of an electrolytic and ceramic capacitor.

Usually a single larger electrolytic capacitor is use for bulk decoupling of many packages and to swamp out resonances of the higher Q ceramic capacitors. (1)

The RC time constant is a small part of the story.  Typically, the layout is a bigger part!

Which points to why one larger electrolytic capacitor can serve for bulk decoupling of several individually decoupled packages.  The small capacitors do not have enough capacitance to work at low frequencies and at low frequencies, the relatively remote electrolytic capacitor is not that far away.

Not just TTL, for any digital or MCU based circuit which might accompany analog parts or analog ICs such as Opamp. If we gonna use 3 capacitors, I was thinking to use tantalum for the biggest one (1uF). what do you think?

10nF and 100nF => ceramic
1uF => tantalum

Stacking up different value ceramic caps is foolhardy.  Normally, it makes things worse.  No one realizes this, because no one tests this!

Some application notes recommend this for specific parts like wideband operational amplifiers and converters.  I wonder though if these date from the time when through hole layouts were parasitic inductance was greater. (1)

It is not quite the same situation but one project I did involved a 50 ohm high power capacitive ground isolator which operated from 50 MHz to 1.2 GHz.  It ended up with 4 x 1000pF, 4 x 0.01uF, and 4 x 0.1uF surface mount ceramic capacitors in parallel using a symmetrical coaxial transmission line layout.  Just using 4 x 0.1uF capacitors did not work at all.

Tantalum are generally safe from an impedance standpoint, but 1uF may be too small, in that its ESR will be too high to be beneficial.  Tantalum are also unsafe on high current power supplies -- they tend to catch fire.

This sort of thing has always bothered me.  Why isn't the output from the power supply better controlled to limit surge current or dv/dt?

(1) At some point it pays off to model the power distribution circuit and if you have the proper equipment, test it.  I suspect this is either foreign or infeasible for many engineers leading to a mix and mash of various rules of thumb for decoupling which usually work but not always.  Jim Williams had something to say about decoupling in Linear Technology application note 47 but unfortunately did not test any polymer electrolytic capacitors.