Amplifier DC Offset won't budge from ~40mV

[Nate_P]

It looks to me like changing the resistor on the feedback side will muck up the gain of the amp. The tone control on this amp is rolled into the power amp feedback loop and it'd be a major science project to modify. I'm actually working to model in the tone control circuit now as without it the voltage gain is all over the place.

I've found suitable models for the sc1845 and sa992, and I found a sub for the driver transistors as well. If I can find a sub for the power transistors I should be able to model the behavior of the entire circuit minus the protection relays etc.


Here's the new sim so far. I haven't gotten around to properly naming everything yet.

 

[Nate_P]

Alright! Finally finished the sim. I gave up on renumbering everything, I'll remember to start with correct numbers next time. It's too tedious to go back and do it after the fact.

Here's the circuit with the tone control. I manually tweaked the pot values to get a flat response as I didn't want to figure out the exact details of the pot contours. I mirrored the amp section so that I could directly compare the effects of any tweaks.

Closer pic of the amp section:

And of my final transient analysis setup:

I added the line:

.option numdgt=7

to force ltspice to use double precision math. Computation time is still quite reasonable using max timestep 1uS.

Here's the THD plot.

The .FOUR results are as follows:

Channel 1 (modified channel): 0.005794%(0.153639%)
Channel 2 (Stock channel): 0.005482%(0.140632%)

To be honest, at this point I can't decide whether to leave well enough alone or zero the offset out of principle because it obviously has negligible negative side effects.

It does seem as if lowering the input impedance is driving the tone control transistor a bit harder, though I can't see any meaningful difference in the FFT picked up at that node either.

EDIT-Forgot to mention that I tweaked the volume control to level match the channels. It does seem like the 100k vs 68k input impedance shifts the volume curve a bit.

Cheers,
Nathan

 

[Nate_P]

Forgot to post the frequency response.

Green=modified, blue=unmodified.

 

[sgrossklass]

Good work. The scaling on the THD plot is pretty nuts though, I would cut off at like -120 dB and < 100 kHz so you can actually see some detail. It does look like 2nd @ -85 dB, 3rd @ -95dB or thereabouts.

What sort of idle current are you getting through the 0.47 ohm resistors? (Including an .op line might prove helpful.) Given this value I imagine the real deal isn't running more than about 20 mA or so - tweak the trimpor value accordingly.

Mind plotting things at the preamp output as well, just to get a clearer picture? Just to avoid having power amp distortion mask the difference.

I would also have a look at freq=10k. I'd guess it wouldn't make much of a difference for the follower but very much may for the power amp when loaded.

Do note that SPICE simulation has a tendency to underestimate BJT distortion since modeling of parasitic capacitance variation is only a linear approximation. The reverse is true for MOSFETs, and FET models also seem to vary a great deal.

BTW, you can always zip your .asc files and upload that... free remote backup.

 

[Nate_P]

The real deal is idle voltage across the 0.47 ohm resistor of 40mV, which corresponds to 42mA idle current. (40mV/(0.47*2))

I set the sim to roughly the resistance I set the adjusters to in real life but it's probably better to match the currents up. I just checked and it's running WAY hot in the sim as I have it. Oops. I'll fix that and report back with adjusted plots. In the meantime, here's the output from the volume control emitter followers:

I did get my BJT files from a library posted randomly here or on another forum so hopefully they're setup reasonably. The voltage drivers and output current drivers are also modeled after modern transistors that have been recommended on various forums as replacements for burnt out examples of the original parts in this amp, as finding a spice file for a 30 year old out of date transistor seemed like an exercise in futility.

Cheers!
Nathan

 

[Nate_P]

I had to turn the bias resistance way way down compared to real life. Any idea why that would be? I'm guessing that my triple diode string is biasing it way harder than whatever the single device triple diode does in real life.

New THD Results:
Modified Channel: Total Harmonic Distortion: 0.005819%(0.153779%
Unmodified: Total Harmonic Distortion: 0.005479%(0.140761%)

 

[Nate_P]

Alright! Here are the 10k results

Output with 8 Ohm purely resistive load:

THD Results:
Modified:Total Harmonic Distortion: 0.013734%(0.019241%)
Unmodified:Total Harmonic Distortion: 0.013785%(0.019280%)

And the input at the diff pair:

THD Results:
Modified: Total Harmonic Distortion: 0.010322%(0.016971%)
Unmodified: Total Harmonic Distortion: 0.010232%(0.016911%)

 

[sgrossklass]

Ideally impedance on inverting and noninverting inputs would be matched, allowing much of the distortion related to input bias current to cancel. Not easy here though.

The real deal is idle voltage across the 0.47 ohm resistor of 40mV, which corresponds to 42mA idle current. (40mV/(0.47*2))

Right in the middle of the optimum 0.13-0.26 mA per resistor range, interesting.

I had to turn the bias resistance way way down compared to real life. Any idea why that would be? I'm guessing that my triple diode string is biasing it way harder than whatever the single device triple diode does in real life.

You should find substantial variation with different diode models. 1N4148s happen to be very small diodes with correspondingly high voltage drop. (I think Bob Cordell has a better model for them, too.) This biasing setup thus is very parts-specific.

Diode string biasing all but disappeared after the 1970s. It's not very flexible and getting tempco right is tricky, not to mention that some series of varistor diodes had a less than stellar reliability track record (an intermittent bias diode is about the last thing you want).

Incidentally, the 47n capacitor in parallel (C111/112) is a good start, but is only being used to tame HF distortion here. Soldering in a little electrolytic of 10+ µF in parallel would substantially extend its effect downwards.

 

[mjona]

One reason that true dc amplifiers are not the norm is that dc offset drifts with the temperature which will vary on the environment.

There is a proportional increase transistor conduction directly proportionate to temperature differences on the Kelvin scale.

It would be mistake to set the output Iq when the amplifier is cold and put the cover back on and not to pay attention to where this is sited - perhaps with other equipment stacked directly above or below.

It is not clear that the simple things like this have been attended to first up.

Semiconductors should hold their specifications for a lifetime. Some power transistors can hang on even although a pcb shows burn marks.

 

[Nate_P]

Ideally impedance on inverting and noninverting inputs would be matched, allowing much of the distortion related to input bias current to cancel. Not easy here though.

What is preventing this in this case?

Right in the middle of the optimum 0.13-0.26 mA per resistor range, interesting.

I believe it's more like 42mA per, as the 40mV is measured across both legs of the dual resistor making up the 0.47 ohm pair. So ~20mV per side/0.47 Ohms = a little over 40mA.

You should find substantial variation with different diode models. 1N4148s happen to be very small diodes with correspondingly high voltage drop. (I think Bob Cordell has a better model for them, too.) This biasing setup thus is very parts-specific.

Diode string biasing all but disappeared after the 1970s. It's not very flexible and getting tempco right is tricky, not to mention that some series of varistor diodes had a less than stellar reliability track record (an intermittent bias diode is about the last thing you want).

Do you know of any good articles written on biasing techniques? I'm now curious what more modern amps use in place of the diodes.

Incidentally, the 47n capacitor in parallel (C111/112) is a good start, but is only being used to tame HF distortion here. Soldering in a little electrolytic of 10+ µF in parallel would substantially extend its effect downwards.

I'll try modelling this up.

 

[Nate_P]

One reason that true dc amplifiers are not the norm is that dc offset drifts with the temperature which will vary on the environment.

There is a proportional increase transistor conduction directly proportionate to temperature differences on the Kelvin scale.

It would be mistake to set the output Iq when the amplifier is cold and put the cover back on and not to pay attention to where this is sited - perhaps with other equipment stacked directly above or below.

It is not clear that the simple things like this have been attended to first up.

Semiconductors should hold their specifications for a lifetime. Some power transistors can hang on even although a pcb shows burn marks.

I took several measurements over time of the DC offset. At initial startup (settles to under 50mV very quickly) and then at various times after the receiver had been running both at idle and after extended playback at relatively high volumes. Obviously the temperature may change with it's case reinstalled, but the sim shows that the design has roughly 35mV of DC offset "baked in" to the input stage so 40mV is actually pretty good for a pair of hand matched input transistors.

That said, I would not expect massive drift on the dc offset simply because it's set only by the small signal side of things. The amount of heat being produced in that section of the circuit is very small and nothing is heatsinked so it shouldn't drift a ton after initial warm up, unless a ton of heat is being trapped in the case from the output transistor heat sink.

I pulled the original 2SA798 pair both because I wanted to measure their matching (not so hot) and because I'd read several accounts of that particular transistor causing troubles so I wanted to do some preventative maintenance. Similar to replacing 2SC458s that go bad and cause noise and leak current.

Cheers
Nathan

 

[mjona]

I took several measurements over time of the DC offset. At initial startup (settles to under 50mV very quickly) and then at various times after the receiver had been running both at idle and after extended playback at relatively high volumes. Obviously the temperature may change with it's case reinstalled, but the sim shows that the design has roughly 35mV of DC offset "baked in" to the input stage so 40mV is actually pretty good for a pair of hand matched input transistors.

That said, I would not expect massive drift on the dc offset simply because it's set only by the small signal side of things. The amount of heat being produced in that section of the circuit is very small and nothing is heatsinked so it shouldn't drift a ton after initial warm up, unless a ton of heat is being trapped in the case from the output transistor heat sink.

I pulled the original 2SA798 pair both because I wanted to measure their matching (not so hot) and because I'd read several accounts of that particular transistor causing troubles so I wanted to do some preventative maintenance. Similar to replacing 2SC458s that go bad and cause noise and leak current.

Cheers
Nathan

Before pulling 2SA798 pairs you would have to consider the applications in which these were being used were like for like - but fair enough replacing these got rid of your bogey.

One thing that does affect the dc balance of an LTP is the tail current which might not be quite right.

The junction of the emitters for the paired transistors is a pivot point for the amount of current drawn by each and if this is not quite enough one will draw more than the other.

R24 in your simulation is part of the Constant Current supply in the LTP tail. The value of 390R sets Q3 current. Further back down the track a 3.9k voltage dropper resistor R3 3.9k feeds a 8.2V zener diode D1 and the bias diodes D2,D3 to Q3 base.

In these areas small variations can make a difference so this is an area of interest.

In the schematic and in your simulation the supply rails of +/-42.9 Volts look odd and one wonders if your electricity supply produces these figures when you measure the hardware.

If your supply voltages are a bit lower than specification, trimming R3 value to change the bias currents slightly in D1-D3 is the first of one of two possible options.

 

[Nate_P]

Thanks for the info! I do remember when I measured the replacement bias diodes (2x 1n4148 to replace a vd1212 which is another amp killer part from the 70s) that one set measured a little lower voltage drop than the other. I can pull those and see if the lower drop pair ended up on the channel with slightly more DC offset.

I'll check the actual voltages. I just started out with the voltage specced in the SM at the supply rails. If I remember right, I think at one point I measured very close to +-40v even.

I've learned a ton since starting this project, replacing the 798s was what I was told to try before I had the schematic so it was one of the first things I did. In hindsight taking more measurements before swapping parts around would have been prudent.

 

[mjona]

It can be helpful to run of a paper copy of the schematic and measure the actual voltages in the areas effected and write them in pencil on the paper copy so you can look at these and think about them later.

 

[sgrossklass]

What is preventing this in this case?

You've got the tone control in there, and its impedance is no doubt going to vary depending on settings. That said, in flat it ought to simplify to something purely resistive between output, inverting input and ground. Well, either that or R||C with equivalent ratios. Having optimum performance in flat seems like a sensible compromise to me.

All you are interested in at the end of the day is the impedance seen by the inverting input. If in doubt, you could always take all of your feedback components, connect the output node to ground and feed the inverting input node via an AC voltage source with very high but known output impedance (maybe 1000 megohms). An AC analysis and some multiplication later, you should have a pretty decent representation of impedance over frequency.

Do you know of any good articles written on biasing techniques? I'm now curious what more modern amps use in place of the diodes.

A Vbe multiplier, usually. It's got the right kind of tempco for BJTs, you can mount its transistor to the heatsink (plastic package TO-126s are often being used for simplicity), and you can dial in just about any voltage regardless of VAS current. The position of the trimpot is somewhat critical - you always have to think about what happens if it ever fails open or develops bad wiper contact; configurations with pot in B-E tend to be failsafe, while those with it in B-C or wiper at base tend to blow things up.

As thermal tracking of bias is invariably delayed by the time it takes for heat to travel through the heatsink and warm up the bias spreader transistor die, some manufacturers have come up with parts featuring integrated sensing diodes. These haven't been quite the hit you might expect them to be, in part due things not working quite as well as expected (tempco matching etc.). That said, the basic idea is good.

As far as literature goes, Douglas Self's Power Amplifier Design Handbook has a chapter on thermal compensation, so that may be worth looking up.

 

[mjona]

Thanks for the info! I do remember when I measured the replacement bias diodes (2x 1n4148 to replace a vd1212 which is another amp killer part from the 70s) that one set measured a little lower voltage drop than the other. I can pull those and see if the lower drop pair ended up on the channel with slightly more DC offset.

I'll check the actual voltages. I just started out with the voltage specced in the SM at the supply rails. If I remember right, I think at one point I measured very close to +-40v even.

I've learned a ton since starting this project, replacing the 798s was what I was told to try before I had the schematic so it was one of the first things I did. In hindsight taking more measurements before swapping parts around would have been prudent.

As pointed out in post 6 there are quite a few twists in the schematic and I can see some things that have not made it across to your simulation - which is a good reason to print out a copy and if this spreads over more than one page to match up the joins and tape them together. You should then do a more thorough check.

Anyway the positive rail voltages in your simulation are given as 42.9V while those on TR114, TR108, and TR110 are slightly lower. On the negative supply you have -42.9V but the feed for some of your transistors comes via R173 from an off the page source.

It seems there was an aim to set the diode bias in transistors and diodes to 0.6V to accommodate the selection of devices.

If you replace the LTP component complement odds are you will not achieve the same level of matching. There was a comment to this effect at the end of post 10.

Re the idea in post 6, of a 40 mV offset being by design a possible reason is to prevent build up of oxidation on relay contacts etc. Do the resistors have shiny leads or are they more a shade of grey in appearance?

 

[billbo]

Check the resistor values of the feedback path and also the input path to see if they haven't drifted from their perspective values. If they check O.K. I would replace TR103 TR104 with simple discrete transistors but make sure you match the beta of each pair as close as possible.Try using BC559C. If this does not work remove the current mirror setup and replace with simple 1k to 1.5k resistor on the left collector of the diff pair and the right collector straight to the negative rail. Simplify the circuit. There is too much bloat in that stage and the amount of distortion added will be next to nothing. C105 and C106 can be implemented on TR105 and TR106 collector to base only iF needed and adjusted appropriately. I did this mod on an amplifier which I could not get the offset down under 100mV. once I did this it came down to 4mV on one side and about 7mV on the other.
Regards
Billy D...
***************************
P.S. replaced emitter resistors and put discrete 0.47 5 watt resistors...

 

[Nate_P]

Interesting suggestions. It does seem that they went for the "everything and the kitchen sink" approach with this input stage. I was reviewing another NEC amplifier schematic and they had a much more basic tail resistor + emitter resistor setup as you suggest. I was surprised by this as it was actually a higher end product.

For now I'd like to get it operating as good as possible in the "stock" topology with minor tweaks and move forward from there. My main purpose here is to learn about amp designs and I'll do that best via an incremental approach.

 

[Nate_P]

If anyone would like to toy with this spice model and make further suggestions, I've made a portable version of it as it stands now and it can be downloaded here:

Dropbox - SchematicBackup.zip

This amp is finally back on the healing bench and I hope to get the last bits of work done on it in the next couple of weeks. I have a pair of vintage KLH's that are looking for something to drive them.

 

[Nate_P]

Check the resistor values of the feedback path and also the input path to see if they haven't drifted from their perspective values. If they check O.K. I would replace TR103 TR104 with simple discrete transistors but make sure you match the beta of each pair as close as possible.Try using BC559C. If this does not work remove the current mirror setup and replace with simple 1k to 1.5k resistor on the left collector of the diff pair and the right collector straight to the negative rail. Simplify the circuit. There is too much bloat in that stage and the amount of distortion added will be next to nothing. C105 and C106 can be implemented on TR105 and TR106 collector to base only iF needed and adjusted appropriately. I did this mod on an amplifier which I could not get the offset down under 100mV. once I did this it came down to 4mV on one side and about 7mV on the other.
Regards
Billy D...
***************************
P.S. replaced emitter resistors and put discrete 0.47 5 watt resistors...

Hadn't thought to check the feedback path resistors. I'll do that.

Using the schematic numbering scheme:

I've already replaced the diff pairs with hand matched 2SC1845s. Replacing the current mirror transistors had no effect so I'm planning to put the originals back in. I also replaced R109, R111, R113 with tight tolerance metal films to no effect. It was at that point that I decided to do the spice model as the shotgun approach obviously wasn't working.

The spice model showed 35mV DC offset even with all perfectly matched theoretical transistors. If I tweak R105 to 68k the DC Offset goes away. I believe it's because 68k is approximately the correct value to match the feedback path DC resistance through R117 and R115, as has been discussed previously.

The question that remains there is - are there any negative effects to doing this? The distortion predictions in LTSpice say no (to my eye) but am I missing anything?