Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 05:40 AM, Andy I wrote:
There is some feedback from the audio signal into the heater voltage. Was that intentional?? Or just an undesirable side-effect?? I don't expect it would have very much effect on the heater's temperature (and from there to the triode's characteristics), but it looks undesirable to me. Should there be filtering?
Sorry, are you asking whether the audio signal feedback into the heater voltage comes from a design intentional choice ? Actually I don't know since I took it from the schematic of a commercial audio amplifier (Bravo Ocean).
|
Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 08:46 AM, Carlo wrote:
A different timestep employed by .TRAN card for transient analysis can't explain that weird (non physical/nonsensical) result for the ITS solution.
You're right about that.
?
Andy
?
?
?
|
Re: LTspice 24.1 Simulation Errors
On Thu, Feb 20, 2025 at 08:57 AM, Tony Casey wrote:
I don't believe that LTspice 24.1 shouldn't have complained, if VCC was assigned in the top-level schematic. It is not re-defined anywhere in the 74LVC1G library. That being so, it is perfectly legal syntax to use it anywhere.
Well, there may be one caveat.? If I remember correctly, Mike Engelhardt said that parameter values do not descend infinitely far down into their subcircuits, like you think they ought to.? I think he said it goes down only three(?) levels deep.
?
That was and is really disturbing.? I never took the time to verify it.
?
Andy
?
|
Re: Weird results DC operating point for Tube amplifier
It's been discussed and argued, and stated by Analog Devices's experts with the LTspice code, that LTspice should be entirely deterministic, with no randomness in simulations unless the user actually adds it.? One of the tools sometimes used to solve systems of equations, is adding a little randomness into the mix.? The randomness can steer the solver one way or the other, thus potentially avoiding difficult solutions.? But we are assured that LTspice does not do that.? As far as I am aware, SPICE itself (from Berkeley) did not either.? As far as I know, "numerical noise" also does not exist in the sense that repeated runs through the same code should be exactly the same, down to the very last bit.? Even "round-off errors" are exactly predictable and repeatable.
?
If I remember correctly, ADI also said that LTspice code did have some unintended non-determinism, and that these have been (or are being) cleaned up in recent LTspice releases.
?
Over the years I have seen cases where LTspice simulated differently on repeated runs.? We know it should not have done that.? My guess is that I was witnessing some of those unintended bugs that ADI has been fixing.
?
Maybe they are not all fixed yet.? (And as they say, you can't get rid of ALL bugs.)
?
Or maybe you (Jerry Lee Marcel) had certain settings set, the first time you tried this simulation, which caused your simulation to converge correctly right "out of the box" the first time, but not a day later when you fired up LTspice again and it had reverted back to your default settings.? Who knows?
?
Andy
?
|
Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 05:40 AM, Andy I wrote:
What I mean is, what do the steady-state DC voltages look like, and are they correct or incorrect for your circuit?? I was not referring to the INITIAL voltages at the start of the transient simulation. When the simulation is near 60 seconds and reached steady-state, do the bias voltages look right, or wrong?
Ok, by "bias voltages" you mean actually the mean value of the voltages averaged for instance over a time period of the source signal (e.g. averaged over a 1ms interval for a 1Khz source signal). Near 60 seconds from the beginning of .TRAN 60 UIC analysis, the heater's voltage and current looks good.
?
I meant the voltages in your circuit, at some or any or all circuit nodes. ?Were the FET's gate and source DC (bias) voltages about right, when near 60 seconds? ?Or were they wrong?
Ok yes, for instance the MOSFET's gate and source mean (DC bias) voltages (and current) near 60 seconds look good.
?
|
Re: LTspice 24.1 Simulation Errors
On 20/02/2025 14:57, Tony Casey wrote:
I
don't believe that LTspice 24.1 shouldn't have complained, if VCC
was assigned in the top-level schematic.
It should be obvious, but due to a typo, it might not be - it should
have been:
I don't believe that LTspice 24.1 should have complained, if VCC was
assigned in the top-level schematic.
--
Regards,
Tony
|
Re: LTspice 24.1 Simulation Errors
On 17/02/2025 09:22, herman.vos via
groups.io wrote:
The highlighted VCC should actually have been VCC3 and
after this correction, LTspice 24.1 will not complain (at least
not for the 2-input nand gate).
?
Do you know what previous LTspice versions have filled in?
Did it assume something like: "ah there's only one parameter
which comes close to VCC which is VCC3 so let's use that one?"
or did it fill in just some positive value (3V3 or 5V? or zero?
Were ALL simulations with this library just wrong??
I don't believe that LTspice 24.1 shouldn't have complained, if VCC
was assigned in the top-level schematic. It is not re-defined
anywhere in the 74LVC1G library. That being so, it is perfectly
legal syntax to use it anywhere. It may well be that it was intended
that the highlighted VCC should have been VCC3, but in actual fact,
it makes no difference as VCC → VCC1 → VCC2 → VCC3 as you descend
the hierarchy. This feature of the library was inherited from the
74HC and 74HCT libraries, originally written by Helmut Sennewald. I
suspect this was deliberately done as an aid to debugging as the
design of the library hierarchy evolved, and was never changed. So I
saw no reason to change it either. The CD4000 libraries were
similar, except that the base parameter used was VDD, instead of
VCC.
It can cause problems, particularly if users either deliberately, or
by accident, don't use the accompanying symbol library with the VCC
parameter named in each symbol, with users then trying to figure out
what parameters should be specified in the top level schematic. If
they would use the example schematic as a template, it would never
arise.
This is a fuss over nothing.
--
Regards,
Tony
|
Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 05:44 AM, Jerry Lee Marcel wrote:
I thought I suggested small differences in (a) settings or (b) algorithms.? I do not suggest gremlins in the computer!? :-)
?
Andy
?
|
Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 03:54 AM, Jerry Lee Marcel wrote:
However, just right now, running the simulation gave the same erroneous results as mentioned by many, with 26V on the heaters (weird from a 24V source).
Do you mean your .TRAN ITS solution (i.e. DC operating point) step returns 26V @ -166mA on the heater's pins ?
I'm no expert, but I suspect the different timesteps explain the different results.
A different timestep employed by .TRAN card for transient analysis can't explain that weird (non physical/nonsensical) result for the ITS solution.
|
Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 05:22 AM, Carlo wrote:
BTW, as far as I can tell, below is the part of the tube's SUBCKT from dmtriodep.inc library modeling the heater:
(netlist code deleted for brevity)
?
Yes, that is the heater's model.? But there is also a "connection" from inside that netlist code, to the triode.? Presumably, that connection brings the heater's temperature to the triode, where it affects the triode's electrical characteristics.? I think many of the node voltages inside the heater model represent temperature, and there are thermal time-constants.
?
Andy
?
|
Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 05:22 AM, Carlo wrote:
What do you really mean with "DC voltages look wrong" ? .TRAN 60 UIC skips the ITS step, hence there is not a DC solution at all.
What I mean is, what do the steady-state DC voltages look like, and are they correct or incorrect for your circuit?? I was not referring to the INITIAL voltages at the start of the transient simulation.? When the simulation is near 60 seconds and reached steady-state, do the bias voltages look right, or wrong?
?
Do you actually mean the average of the voltages on some circuit's nodes ? In this sense, yes, starting from about 50 sec, the (averaged) voltage on heater's pin looks good like the (averaged) current entering it (its sign looks good either !)
I meant the voltages in your circuit, at some or any or all circuit nodes.? Were the FET's gate and source DC (bias) voltages about right, when near 60 seconds?? Or were they wrong?
?
There is some feedback from the audio signal into the heater voltage.? Was that intentional?? Or just an undesirable side-effect?? I don't expect it would have very much effect on the heater's temperature (and from there to the triode's characteristics), but it looks undesirable to me.? Should there be filtering?
?
.TRAN 60 Startup analysis looks good either.
So, if .TRAN 60 UIC looks bad, but .TRAN 60 Startup looks good, then it should be obvious which one to use and which one to avoid.
?
But you added the word "either"!? I don't understand.? Did I misunderstand you?
AFAIK "Start external DC supply voltages at 0V" (Startup) does apply to DC voltage power supply and does not to SINE, PWL, PULSE, EXP sources including subcircuit (SUBCKT) sources. Does it apply to DC current power sources as well ?
Yes, "Startup" applies only to the DC value of independent sources.? I believe "sources" means both voltage and current sources.? (You can try it and see what it does.)
?
Note that it does not apply to independent sources inside of subcircuits.? That's why it has the word "external".? I believe LTspice does that because sources inside subcircuits are likely parts of models and how they work, and not the sources that supply power to the circuit.? LTspice wants to start only the main power sources at 0 and then ramp them up, but not modify what's inside the models.
?
Andy
?
|
Re: LTspice 24.1 Simulation Errors
On Thu, Feb 20, 2025 at 12:26 PM, Tony Casey wrote:
If a top level parameter is not re-defined beneath the top level, its value will cascade down the hierarchy. Perhaps, it is this behaviour that has changed in 24.1? I haven't had the chance to investigate this further yet. This would represent a significant change in the assumed architecture.
--
Regards,
Tony
That's exactly what happens. Nothing was changed.
|
Re: Weird results DC operating point for Tube amplifier
Well, I have not much to tell.
The simulation worked right from day one, with 5.8V on the
heater.
However, just right now, running the simulation gave the same
erroneous results as mentioned by many, with 26V on the heaters
(weird from a 24V source).
BUT, running the sim for 60 seconds shows the voltage
oscillating, to more or less stabilize at about 5.8V. The peaks
never go above 15V.
I'm no expert, but I suspect the different timesteps explain the
different results.
Le 20/02/2025 à 12:19, Carlo a écrit?:
toggle quoted message
Show quoted text
On Thu, Feb 20, 2025 at 02:44 AM, Jerry Lee Marcel wrote:
I have no problem understanding the possible
multiple equilibrium possibilities.
My question was why does my installation succeeds everytime in
finding a viable solution when it seems all others have
problems.
Is my computer jinxed?
Sorry, could you be more specific about your viable solution of
.TRAN analysis (without UIC or Startup flag) ? I'm referring in
particular to the ITS (aka DC operating point) solution (e.g.
the DC current entering the heater's pins). Thanks.
|
Re: LTspice 24.1 Simulation Errors
On 17/02/2025 17:28, Andy I via
groups.io wrote:
These are good
questions.? I can't answer them without examining the models more
closely.? But if it's true that there was no parameter named
"VCC", then all versions of LTspice should have / would have
complained bitterly about that and refused to run.? LTspice would
not ever have substituted a different parameter, whether or not it
had a similar name.
This was never the case. "VCC" is the required top level parameter
in 74LVC1G, just as with 74HC and 74HCT etc.. If it is not set,
LTspice (all versions) will set an error. If a top level parameter
is not re-defined beneath the top level, its value will cascade down
the hierarchy. Perhaps, it is this behaviour that has changed in
24.1? I haven't had the chance to investigate this further yet. This
would represent a significant change in the assumed architecture.
--
Regards,
Tony
|
Re: Weird results DC operating point for Tube amplifier
On Thu, Feb 20, 2025 at 02:44 AM, Jerry Lee Marcel wrote:
I have no problem understanding the possible multiple equilibrium possibilities.
My question was why does my installation succeeds everytime in finding a viable solution when it seems all others have problems.
Is my computer jinxed?
Sorry, could you be more specific about your viable solution of .TRAN analysis (without UIC or Startup flag) ? I'm referring in particular to the ITS (aka DC operating point) solution (e.g. the DC current entering the heater's pins). Thanks.
|
Re: LTspice 24.1 Simulation Errors
On 17/02/2025 09:22, herman.vos via
groups.io wrote:
I'll be happy to
upload later this week an updated version of the 74LVC1G library
with the abovementioned faults repaired.?
If you do this, could you ensure that all the changes are logged in
the header of the library, so I can keep track of everything.
Thanks.
--
Regards,
Tony
|
Re: Has anyone tried 24.1.3?
On 19/02/2025 10:25, Ian McCrum MI5AFL
via groups.io wrote:
.meas ac V3dBnf when
mag(S21(V1))=Vmax/sqrt(2) rise=1
This has always worked. The keyword "WHEN" is always associated with
the x-axis value. In .AC it is Hertz. In .TRAN it is time.
"FIND <something>" should only really be used when
<something> is explicitly not the x-axis, although it does
also work when referring to the x-axis. Why make the .MEAS more
complicated than it needs to be?
--
Regards,
Tony
|
Re: Weird results DC operating point for Tube amplifier
I have no problem understanding the possible multiple equilibrium
possibilities.
My question was why does my installation succeeds everytime in
finding a viable solution when it seems all others have problems.
Is my computer jinxed?
Le 19/02/2025 à 16:22, Andy I via
groups.io a écrit?:
toggle quoted message
Show quoted text
On Tue, Feb 18, 2025 at 11:18 AM, Jerry Lee Marcel wrote:
How come that I can run the simulation, which gives
credible results?
A good question.
?
This model can fail because it has more than one stable
operating point.? Think about flip-flops.? They have two stable
states, and neither is guaranteed to happen initially.? A simple
flip-flop might come up in either state (and maybe one of three
states when simulated).
?
The heater's model is likely to always simulate coming up in
the same state because SPICE is deterministic, when used with
the same settings and algorithms.? But differences in simulator
settings or algorithmic details might change that.? I'm guessing
that is why you had better luck than others did.
?
Andy
?
|
Re: Weird results DC operating point for Tube amplifier
On 19/02/2025 20:32, Carlo wrote:
TRAN 60 UIC or
"start external DC supply voltage at 0V" actually skip the ITS
step, hence even after 60 sec of simulation the time constant of
heater's model is such that that singularity is not reached.
This is not what "UIC" means or does. If you just want to start the
DC sources at zero, use the "startup" switch instead.
--
Regards,
Tony
|
Re: Weird results DC operating point for Tube amplifier
On 19/02/2025 13:58, eewiz via
groups.io wrote:
I wish I would have stumbled upon this feature long ago.
?
This causes me to wonder about this wire probing
feature versus placing 0V sources in wires to measure currents?
The advantage of the 0V voltage source method is that it can easily
be used in the argument of B-sources.
--
Regards,
Tony
|
Carlo
Tony Casey