I am building a 6dj8-6as7 headphone amp, and it all working fine. This is my first scratch build project. So I have been doing a lot of SPICE sim and experimenting different things. Ragarding the PSU, I observed something interesting. The current draw is less than 60ma, power transformer is toroidal. AC heater supply comes from a separate toroidal heater transformer.
With
Rectifier->45uf ASC Cap->10H-125ma Hammond 159P Choke->45uf ASC Cap
I hear loud hum noise.
With
Rectifier->470uf electrolyptic Cap->10H-125ma Hammond 159P Choke->470uf electrolyptic Cap
I hear no hum at low volume.
The SPICE sim result shows that 10H/45uf PI filter should give low enough ripple.
Not having an o-scope to do more test, I can only suspect the Hammond choke might be the cause of hum.
Anyone has similar experience?
With
Rectifier->45uf ASC Cap->10H-125ma Hammond 159P Choke->45uf ASC Cap
I hear loud hum noise.
With
Rectifier->470uf electrolyptic Cap->10H-125ma Hammond 159P Choke->470uf electrolyptic Cap
I hear no hum at low volume.
The SPICE sim result shows that 10H/45uf PI filter should give low enough ripple.
Not having an o-scope to do more test, I can only suspect the Hammond choke might be the cause of hum.
Anyone has similar experience?
When you exchange that last cap, I guess because of the different form factor, you also change the ground connection of that cap to a different one.
Very often these things are a result of ground loops.
If you indeed change the connection, try to connect the caps both (when changing) exactly to the same point, and see if it still makes a difference in hum. Possibly not, and then you know the correct connection.
Jan Didden
Very often these things are a result of ground loops.
If you indeed change the connection, try to connect the caps both (when changing) exactly to the same point, and see if it still makes a difference in hum. Possibly not, and then you know the correct connection.
Jan Didden
Hi pftrvlr ,
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 .
Second , as a rule of thumb , the capacitor value have to be
aprox. 2200 uf / Ampere , to give you a low ripple . In your
case , 2200 uf x 0.060 A = 150 uf .
Third , to give you a “perfect” capacitor behavior , you need
to connect in parallel with each electrolytic cap , a mylar
or a polypropilene cap , with 1 / 100 of its value . Say , if
you are using a 150 uf elec. cap , you have to use a 1.5
uf in parallel with it , and the best solution , another plastic
capacitor of 1.5 uf / 100 = 15 nf , in parallel with the others .
( total 3 capacitors in parallel , 150 uf + 1.5 uf + 15 nf )
The new filter will be :
150 uf + 1.5 uf + 15 nf --> Choke --> 150 uf + 1.5 uf + 15 nf
Obviously I am assuming that you are using solid state
rectifiers , so the input capacitor value will not be a problem .
Try this solution , and give us a feedback ,
Regards ,
Carlos
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 .
Second , as a rule of thumb , the capacitor value have to be
aprox. 2200 uf / Ampere , to give you a low ripple . In your
case , 2200 uf x 0.060 A = 150 uf .
Third , to give you a “perfect” capacitor behavior , you need
to connect in parallel with each electrolytic cap , a mylar
or a polypropilene cap , with 1 / 100 of its value . Say , if
you are using a 150 uf elec. cap , you have to use a 1.5
uf in parallel with it , and the best solution , another plastic
capacitor of 1.5 uf / 100 = 15 nf , in parallel with the others .
( total 3 capacitors in parallel , 150 uf + 1.5 uf + 15 nf )
The new filter will be :
150 uf + 1.5 uf + 15 nf --> Choke --> 150 uf + 1.5 uf + 15 nf
Obviously I am assuming that you are using solid state
rectifiers , so the input capacitor value will not be a problem .
Try this solution , and give us a feedback ,
Regards ,
Carlos
Carlos: The choke's inductance might be a little low from drawing 60mA rather than 125mA, but nothing much to worry about. I think you may be coming from a solid-state viewpoint with your capacitor rule of thumb - valve rectifiers won't tolerate much capacitance. Adding small values of capacitance in parallel with an electrolytic will tidy up HF behaviour, but not change hum.
Pftrvir: I think the problem is more likely to be that headphones are very sensitive transducers so the acceptable levels of hum are much lower. It could always be a wiring problem as Jan has suggested, in which case the hum is likely to have a buzzy sound, but it may simply be that you need to add another stage of filtering. If you're keen and competent with SPICE, then why not calculate the level of hum that would be 120dB down on the headphone's maximum output and see if your amplifier sims at that level?
Pftrvir: I think the problem is more likely to be that headphones are very sensitive transducers so the acceptable levels of hum are much lower. It could always be a wiring problem as Jan has suggested, in which case the hum is likely to have a buzzy sound, but it may simply be that you need to add another stage of filtering. If you're keen and competent with SPICE, then why not calculate the level of hum that would be 120dB down on the headphone's maximum output and see if your amplifier sims at that level?
Thanks everyone.
The PSU has both a solid FRED rectifier and a 5Y3 tube rectifier. I can swith between this two easily depending the output voltage I need. Immediately after the rectifier is a 50 ohm resistor. I'm too concern about the in-rush current of the 5Y3.
I do parrallel a 1.5uf MKP cap with the electrolyptic cap. Having too many of the 1.5uf MKP, I put them everywhere.
Wiil do more SPICE and DMM work and report what I find out. Also thinking to get a cheap o-scope from EBay.
The PSU has both a solid FRED rectifier and a 5Y3 tube rectifier. I can swith between this two easily depending the output voltage I need. Immediately after the rectifier is a 50 ohm resistor. I'm too concern about the in-rush current of the 5Y3.
I do parrallel a 1.5uf MKP cap with the electrolyptic cap. Having too many of the 1.5uf MKP, I put them everywhere.
Wiil do more SPICE and DMM work and report what I find out. Also thinking to get a cheap o-scope from EBay.
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.
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.
refference said:
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?
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
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
pftrvlr said:
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
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
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
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.