paralleling film caps with electrolytic caps

[mzzj]

http://omega.enstb.org/yannis/cours/s31/i-want-to-believe.jpg

 

[Conrad Hoffman]

Well, the truth is out there. Somewhere. Isn't it?

 

[Conrad Hoffman]

Ack! It's all worthless pontification. I installed a switch that flips 24 ohms in and out of both supply rails on my preamp. Can't hear one iota of difference other than my imagination playing tricks on me. Filter with whatever caps you find on the floor under the bench, or use big bucks audiophile parts, the results will be determined by what's in your head, not what's in the preamp. OTOH, I changed my cartridge alignment by less than a degree, and that makes what I consider a big difference.

 

[Eva]

Ack! It's all worthless pontification. I installed a switch that flips 24 ohms in and out of both supply rails on my preamp. Can't hear one iota of difference other than my imagination playing tricks on me. Filter with whatever caps you find on the floor under the bench, or use big bucks audiophile parts, the results will be determined by what's in your head, not what's in the preamp. OTOH, I changed my cartridge alignment by less than a degree, and that makes what I consider a big difference.

I fully agree. Audibility of supply and coupling capacitors is a myth. The advantages of parallel capacitors are a myth. Any capacitor is fine as long as the amplifier loops being powered don't oscillate and the resulting ripple voltage is low enough considering PSRR. Electrolytics alone are fine in 100Khz SMPS, placing anything else in parallel results in ringing and increased EMI. The increasingly resistive nature of electrolytics at high frequencies is almost always advantageous.

Our ear is plain junk, 90% of what we hear is what we have been told to hear by others. I get really bored with those placebo effect discussions. I usually expend my time tuning audible things like speakers and crossovers. Alter tweeter level by 0.5dB and you will get an audible change for sure.

 

[ChocoHolic]

Fascinating...
I just went for two days to see the terracotta warriors and when I come back, then suddenly a hardfact thread turned to subjective opinion thread...
I do not reject our subjective perception as Eva does, but up to now my experience with most myth-explanations was that my trial to correlate the stated sound differences with circuit mods and measurements did fail.

...
Our ear is plain junk, 90% of what we hear is what we have been told to hear by others. I get really bored with those placebo effect discussions. I usually expend my time tuning audible things like speakers and crossovers. Alter tweeter level by 0.5dB and you will get an audible change for sure.

I fully agree to look at the dominant obvious drawbacks in sound reproduction.
...you optimze about 0.5db in speakers? ..wow...

I am struggling with 20db errors of my living room...

But the good thing is: My ears told me during many other listening sessions at friends and shops, including myth-perfectionized systems, that they have similar issues
Usually only the systems, which are promoted as tight/fast bass (nice wording for no bass) do not suffer from that.

Back to topic:
In most of the models in this thread I am seriously missing the resistive part. mzzj is completely right.
High Q of a PSU is not desired. We need low Z combined with low Q.

 

[Conrad Hoffman]

Eva, I'm not bored yet. I'm willing to go after anything that holds out some hope of being real, rather than biases and imagination. Unfortunately, I've yet to find much in terms of wire types, cap types, or anything else that doesn't affect the basic frequency response and distortion products. I have heard differences in circuit topologies, but suspect the spectrum analyzer would quickly explain those. The speakers and room still overshadow everything else. Fortunately, most of my listening is done with headphones.

 

[rdf]

Source impedance is one aspect of power supply filtering, consider RF noise rejection. Back to technical, do single electros have a very high Q impedance peak where the effective series inductance goes off against the parallel leakage capacitance? LTSpice, which doesn't have parameters to add losses to parasitics, will return PS attenuation of 0dB at that point, typically in the TV band.

 

[mzzj]

Source impedance is one aspect of power supply filtering, consider RF noise rejection. Back to technical, do single electros have a very high Q impedance peak where the effective series inductance goes off against the parallel leakage capacitance? LTSpice, which doesn't have parameters to add losses to parasitics, will return PS attenuation of 0dB at that point, typically in the TV band.

LTSpice's own capacitor model seems bit strange:
If I set 10000uF cap with 30nH series inductance and 30mohm series resistance it shows insane resonance peak at 6Mhz and again dropping impedance beyond this point. It appears that LTspice assumes that Cpar is 0.1% of the actual capacitor value and uses model descibed on manual page 108
http://www.google.com/url?sa=t&ct=r...rTqcwyqnPoP_CqhKg&sig2=WuDPcG8h9TjKJWFW4JYi4g

For large electrolytics this model leads to completely insane results and I think its better use exteral Rs+Ls added to cap.

 

[rdf]

That caught me out too. Set it explicitly to zero to disable Cpar. The insane peak is, of course, due to Cpar and Ipar being modeled completely lossless. Any idea what realistic values for loss would be?

 

[Conrad Hoffman]

Hurrah! People smarter than me are finally looking at the cap model, which I've always been a bit unhappy with for audio purposes. Now, how do you do losses that are frequency dependent, so the results of a sweep are accurate? A fixed value Rs or Rp is worthless for that. (Should we move it over to a Spice thread?)

 

[gootee]

I hope that somebody does come up with a decent way to improve frequency-dependent modelling of capacitors, in LT-Spice.

There are some LT-Spice "demos" having to do with capacitors with frequency-dependent losses, at:

http://tech.groups.yahoo.com/group/LTspice/files/ Tut/Laplace Sources/

You would probably need to be a member of the LT-SPICE group, to download the files. Here is the homepage, in case anyone wants to register: http://tech.groups.yahoo.com/group/LTspice/ .

I looked into modelling frequency-dependent ESR for AC analysis in LT-SPice, but haven't gotten too far, yet: For frequency-dependent ESR, we would need a frequency-dependent resistor, to place in series with a capacitor. That CAN be done in LT-Spice, for AC Analysis, by using a G-source (a voltage-dependent current source), with a Laplace equation in the source's "Value" field.

For example, if we somehow knew that, for a particular cap, ESR=.08+8000/freq, we could put a G-source in series with the cap (connecting the "voltage control" lines of the G source to the ends of the series assembly of cap and G-source, presumably) and, in the G-source's "Value" field, enter:

Laplace=(1/(.08+8000*2*3.14/(1+abs(s))))

I tried this, and it DOES seem to more-or-less work. But I haven't gotten too far into it, yet. When I tried it with an ideal 22uF cap with a 10K resistor, in a low-pass filter configuration, it at least made a low-pass frequency response curve with the 3 dB point at the correct frequency, and then leveled out to constant gain again at some higher-frequency breakpoint. But, the phase stayed at zero degrees. (If I changed the polarity of the voltage control inputs for the G-source, I also got a peak at the 3 dB frequency, plus the phase was 0 deg until the 3 dB point, and then flipped to 180 deg.)

There is also a way to use a table, instead of an equation, to specify frequency-dependent data points, IIRC.

- Tom Gootee

 

[Eva]

Electrolytic capacitors become more resistive and less capacitive at high frequencies due to the distributed nature of ESR and capacitance. How about modelling this by splitting capacitance and ESR in, say, 10 equal parts and connecting them in series/parallel in a pi fashion?

 

[gootee]

Electrolytic capacitors become more resistive and less capacitive at high frequencies due to the distributed nature of ESR and capacitance. How about modelling this by splitting capacitance and ESR in, say, 10 equal parts and connecting them in series/parallel in a pi fashion?

Hi Eva,

That sounds like it might be a reasonable type of approach to look at.

Importantly, it (or something like it) might be a way to be able to use resistors that DON'T vary with frequency, to get a capacitor model with resistance and capacitance (and impedance in general) that DO vary with frequency, which would be a very nice way to be able to do it, with Spice, since Spice's Laplace sources often are not practical to use in the time domain.

Maybe all we would need would be a way to use published or measured ESR and DF numbers, probably at two or more different frequencies, to get the R and C values for the model.

I realize that you suggested just dividing the C and R equally. I will try that, in LT-Spice, with some caps for which I have ESR at two different frequencies, and see what kind of match-up I can get, for varying numbers of RC sections. Oops: I'm not sure how the Pi-type topology would work, in this case. That might be more like modeling equivalent _parallel_ resistance. (Or, maybe/probably I don't understand how you meant for them to be connected.) But see the next paragraph.

Another proposed model that I have seen, at http://groups.google.com/group/sci....5b44b149a4aaee?q=spice+capacitor+esr&lnk=ol&# (about halfway down the page), uses a main series L, R, and C, and then has multiple RC-in-series sections, all in parallel with the "main" C. More parallel RC sections increases the accuracy, apparently (maybe in much the same way that adding terms to a Taylor series does). But I have no idea, yet, how the R and C values would be calculated, for that type of model. (Or maybe we could use Eva's suggestion and just divide the main C and R (i.e. ESR), maybe even equally, into some number of parallel series-RC sections. Or maybe we'd need to use some geometrically decreasing values, or something. I can't quite see it, off the top of my head, yet.

From what I have read recently, ESL (Equivalent Series Inductance) apparently does not vary with frequency (edit: it actually does). And DF (Dissipation Factor, where DF = ESR/Zc, Zc=w.C.ESR, so ESR=DF/(w.C) = DF/(2.Pi.f.C)) is apparently very roughly constant with frequency. So that should mean that if we have a published ESR spec for one frequency, and a published DF spec, then we can calculate ESR at some other frequency, subject to "DF is _very roughly_ constant with frequency". So, at least there might be a way for those of us without network analyzers to try to verify any model that we do try.

OK. I did a little research, after writing but before posting the above. I did a Google search for "spice capacitor esr distributed model frequency". The stuff below is all from the first three pages of the search results.

Here are some pretty-good papers I found (but only skimmed, so far), that are about the use of ladder networks for modelling capacitors:

http://www.aeng.com/articles/Capacitor.pdf (see Page 8)

http://www.intusoft.com/nlpdf/nl45.pdf (see Page 11)

http://www.kemet.com/kemet/web/home...CD004EBC04/$file/TechTopics Vol4No5 Sep94.PDF

http://thayer.dartmouth.edu/inductor/papers/CAP2IAS.pdf

http://www.cde.com/tech/impedance.pdf

And this might be interesting:

http://www.intusoft.com/models/caps.lib

There's also some very-interesting-looking stuff here:

http://home.att.net/~istvan.novak/papers.html

In particular, from that site, THIS GUY seem to have gotten extremely serious about it: http://home.att.net/~istvan.novak/papers/DCE05_Black-box-model_SUN-Novak_v1.pdf

These are also from that Istvan Novak site:

http://home.att.net/~istvan.novak/papers/EPEP2003_cap_models.PDF
http://home.att.net/~istvan.novak/papers/EPEP2003_cap_models_poster.PDF

Enjoy.

P.S. INTUSOFT'S Newsletters appear to be a GOLDMINE of spice simulation tips, etc! They're all here:

http://www.intusoft.com/newsletters.htm

- Tom Gootee

 

[gootee]

Here's a page with a technique for measuring capacitor parasitics, WITHOUT a network analyzer:

http://emcesd.com/tt020100.htm

- Tom Gootee

 

[gootee]

OK. I tried it. And this "frequency-dependent spice capacitor model" stuff looks promising.

The main "problem" is going to be the fact that the needed datapoints are going to have to come from somewhere, which, in many cases, might mean actually measuring them ourselves, unless someone can point out an easier way.

Then, I'm hoping that someone knows where to get, or how to design, an algoritm that will synthesize the RLC network to fit to the data.

The only thing I've actually tried, in LT-Spice, so far, is the "RLC ladder network" type of model, similar to what is shown on Page 8 of this paper:

http://www.aeng.com/articles/Capacitor.pdf

And I only had two "half" data points, i.e. the ESR at two frequencies. So I just manually tweaked the R coefficients, until the real part of the response to a 1 Amp sine wave matched the ESR at those frequencies.

I guess I'll have to haul out one of my old phase-angle voltmeters and get some real (no pun intended) datapoints (OR, what WOULD be a good way to get the needed data?). And then, as I said, I hope that someone knows where to get an algorithm that will fit an RLC ladder network to such a dataset. (I don't really want to become a programmer, again.) [It would be awfully nice, too, if the data for, say, one series of models from a manufacturer had some scalable commonality, or something like that, that would make coming up with the spice models easier, once one was done.]

One good thing about this type of model (as opposed to using Laplace sources, etc) is that it also works well for Transient simulations.

Below is a JPEG of (and downloadable LTSpice files for) a schematic of what I tried, in case anyone is interested. It was done for a Nichicon UHE-series 220 uF 50 Volt electrolytic capacitor. I modeled it with one spice capacitor as well as with the RLC ladder-network, for easy comparisons. There are quire a few problems with it, still, mostly because of my extremely-limited data, and poor model parameter selection. But you'll see that it has great potential.

http://www.fullnet.com/~tomg/capmod1.jpg

And here is a plot of the real part of the voltage divided by current (i.e. resistance), in the frequency domain:

http://www.fullnet.com/~tomg/capmod1p.jpg

And here are the LTSpice files for the schematic above:

http://www.fullnet.com/~tomg/capmodel.zip


It's just a start. I hope that someone has some ideas that can make it much easier to model real capacitors with somewhat-accurate frequency-dependent characteristics. So far, as I have said, the main two problems seem to be a) getting the data for a capacitor, and b) synthesizing the model-network based on the data.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

 

[Eva]

Uhm...

I like the ESR plot that you got, it looks realistic.

Doesn't the distributed R, L and C look like a lossy transmission line (like a coaxial cable)? Couldn't it be modelled that way?

 

[gootee]

Doesn't the distributed R, L and C look like a lossy transmission line (like a coaxial cable)? Couldn't it be modelled that way?

Yes! Good observation. In fact, I have been seeing mentions of using lossy transmission line models for this, depending on which version of spice, or whatever, that the people were using.

I've never actually tried any of the lossy line models in Spice. But we still would need the parameters for particular capacitors, right? Or is there something I'm missing, that would make it all much easier?

 

[gootee]

In case anyone is feeling ambitious, the paper at the link below might have some good clues about an algorithm for synthesizing a ladder network, given a curve-fitted transfer function (See pages 11 to 22):

http://www.ee.ucl.ac.uk/~yyang/E713/E713_Notes_1.pdf

And this one looks very interesting, too (done back in 1964!):

http://ntrs.nasa.gov/archive/nasa/casi.ntrs.nasa.gov/19660030427_1966030427.pdf

(Wow those people did some work!)


I'm hoping there's some major simplification that can be taken advantage of.

 

[gootee]

Speaking of transmission lines, the paper below has probably everything one might need to know about the mathematics and modeling of wires, pcb traces, and transmission lines:

http://bwrc.eecs.berkeley.edu/Classes/ICDesign/EE141_f99/Notes/chapter4.pdf


More material from that course:

http://bwrc.eecs.berkeley.edu/Classes/ICDesign/EE141_f99/notes.html

 

[Conrad Hoffman]

Here's a spreadsheet with my measurments of various capacitors at different frequencies. Possibly that can confirm the model.

Conrads Caps

This is great stuff, and should either prove revealing, or put a lot of capacitor myths to bed.

edit- typo