Noisy PSU?

[pftrvlr]

Originally posted by astouffer
Is the filament supply floating? Connect a 1.uf cap from one side to ground.

The heater supply is grounded through two 100 ohm resistors. I do want to try DC-float AC-ground config later.

[pftrvlr]

Did some more SPICE sim, and here is what I found:

For
Rectifier->45uf ASC Cap->10H-125ma Hammond 159P Choke->45uf ASC Cap
There is 32mv p-p ripple in the PSU output

For
Rectifier->470uf electrolytic Cap->10H-125ma Hammond 159P Choke->470uf electrolytic Cap
The ripple is about 0.5mv.

I will measure the ripple using cap->DMM method see if the numbers match.

Sounds like that a headphone (95db sensitivity) amp requires a much lower ripple PSU.

[pftrvlr]

Originally posted by refference
First of all , your headphone amp is drawing less than
60 mA , from the power supply , your choke is rated for
10 H @ 125 mA , so it is not developing the total self-in-
ductance , then the SPICE sim , does not reflect the actual
situation .

The Hammond web site (http://www.hammondmfg.com/153.htm) states:


Units will exhibit less inductance at slightly higher currents or more at lower currents.


I am bit confused. Can someone explain?

[refference]

Hi pftrvlr ,

Hammond’ s staff gives that information , because they
probably are giving the AVERAGE self-inductance value .

If the current rises , the nucleus will saturate sooner
and then the self-inductance will obviously be a bit lower
than the average value .

If the current is low , the nucleus is working more
“ relaxed “ , and then the self-inductance will be a bit
higher than the average value .

At this point I apologize , and agree with EC8010 , when
he said :

“Carlos: The choke's inductance might be a little low from
drawing 60mA rather than 125mA, but nothing much
to worry about “
...... and vice-versa .

So , forget about my first suggestion , but I sustain my
second and third suggestions , obviously if you are using
tube rectifier , you must to pay attention to the tube datasheet
about the input capacitor max. value . ( see my post # 4 )
The 2200 uf / Ampere rule of thumb , has worked very fine ,
for me , many years , for both , tubes and solid state PSUs .

After all , I think that you only need a better filter , like you
said in your post # 12 :

“Sounds like that a headphone (95db sensitivity) amp requires
a much lower ripple PSU.”

Conclusion ( at least for me )
You have a very good headphone amp. and an excellent head-
phone , and the “ set “ is very sensible to ripple .

Best Regards for all ,

Carlos

[gootee]

Originally posted by pftrvlr
Did some more SPICE sim, and here is what I found:

For
Rectifier->45uf ASC Cap->10H-125ma Hammond 159P Choke->45uf ASC Cap
There is 32mv p-p ripple in the PSU output

For
Rectifier->470uf electrolytic Cap->10H-125ma Hammond 159P Choke->470uf electrolytic Cap
The ripple is about 0.5mv.

I will measure the ripple using cap->DMM method see if the numbers match.

Sounds like that a headphone (95db sensitivity) amp requires a much lower ripple PSU.

In your spice simulations, you probably do need to at least include the capacitors' ESR (Equivalent Series Resistance), AT the ripple frequency.

If your caps' datasheets don't give the ESR at 120 Hz (or 100 Hz), they should at least provide a figure for max tan(delta), or maybe for dissipation factor (which is just a percent = 100*tan(delta)).

Then use tan(delta) @ f = 2 * Pi * f * C *ESR(f)

i.e. ESR(f) = tan(delta)/(2 * Pi * f * C)

e.g. If tan(delta) = 0.1, then, for 45uF,

ESR45(120Hz) = 0.1/(2 * 3.14 * 120 * .000045) = 2.95 Ohms

and for 470uF,

ESR470(120Hz) = 0.1/(2 * 3.14 * 120 * .00047) = 0.282 Ohms

So you put those resistances in series with each capacitor. Then your spice simulation should match reality a little better.

If you want to make it better still, you can also include the parasitic inductance and resistance of your wires or PCB traces. You can look up the typical values of each of those, for different wire gauges, or calculate them for PCB trace geometries. But, to start with, you can just try using 25nH and .001 Ohm per inch of wire or PCB trace. So you just put an inductor and resistor in series, in place of each conductor, in your simulation.

Using the wire or trace impedance in simulations is especially important when you want to make sure that ground-return currents aren't ruining an otherwise-good power supply and amplifier design, with the voltages they induce at the non-ground ends of shared conductors!

I have some ready-made LTspice simulation files that might be helpful, and also GIF drawings of same, downloadable at:

http://www.fullnet.com/~tomg/gooteesp.htm

They include a couple of power supply schematics, which already have a convenient setup for including grounds' impedances. NOT shown are the parasitics included in each component, since they are not shown on the LTspice schematics (because LTspice allows entering them directly for some components).

Also included is a power transformer model, with simple instructions for measuring the parameters yourself, from which it then calculates other parameters automatically.

- Tom Gootee

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

[pftrvlr]

Thanks Tom. I will check it out. I am using point-to-point wiring, is there any difference in the parameters from the PCB?

[gootee]

Yes. Every wire size and material, etc, has its own figures for inductance and resistance per unit of length. PCB traces' impedances, similarly, vary with trace length, width, thickness, and material type.

You can find auto-calculators for all of those things, on the web, if it becomes important to do them more-accurately. But, at first, you can just use the 25nH per inch and 0.001 Ohm per inch (which are probably close to #20 wire). Later, if you find out that your circuit happens to be sensitive to a particular wire's impedance, then you might want to worry about getting it more exact.

While we're on the subject of parasitics: I usually also stick a 0.3pF cap in parallel with each resistor, to see if the circuit is sensitive to it. Resistors do have capacitance. (Actually, everything has capacitance, and inductance, and resistance.)

If you want to get fancy, you can also model the leakage current of the capacitors. Many of them say it's something like ".01CV or 3uA, whichever is greater", although some common "low leakage" types say .002CV.

So, assuming they say I = .01CV, that gives V/I = 1/(.01C) = parallel R for the model.

e.g. For 470 uF: 1/(.01 * .000470) = 213k in parallel. And for 45 uF: 1/(.01 * .000045) = 2.22 Meg in parallel.

By the way, for any ceramic and film caps, you can use an ESR of something like .03 Ohms, just to get in the ballpark, to see if the circuit is sensitive to it. It might help when you're looking for high-frequency resonances, if everything else is modeled well.

And, of course, always include the spec'd series R for inductors, if you don't have an even better model for them.

Note, too, that if you're doing AC Analysis (bode plots), then it gets "a little more difficult" to model some of the frequency-dependent things, like ESR of caps. In that case, you have to create a resistor for each one that uses a Laplace source. It gets somewhat messy. And those Laplace sources usually don't like simulating in the time domain, very well at all, unfortunately.

- Tom Gootee

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