Re: 12AU7 tube heater model
Indeed, but I think it is a dangerous option,
to be used only with great care. Parallel V sources can create
infinite loop current, and non-physical transformers are not
easy to detect, which being liable to produce credible but wrong
results.
On 2025-02-21 14:44, Andy I via
groups.io wrote:
There is another option to disable the topology check that
caused this error.
.options topologycheck=0
The description is: "Set to zero to skip check for floating
nodes, loops of voltage sources, and non-physical
transformer winding topology".
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: 3 Phase Voltage Sense model
Andy, your right thought I had those matching, will correct and give it a try.
?
Larry
|
Re: 12AU7 tube heater model
vOn Fri, Feb 21, 2025 at 09:35 AM, Carlo wrote:
BTW, on LTspice Control Panel->Hacks! tab there is a checkbox named "Add GMIN across current sources". Is it supposed to "address" such a problem/error related to the current source's infinite impedance ?
I do not think it was designed for that purpose.
?
It does not eliminate the error message.? The error message comes about because of a topology check.? When LTspice is checking the topology, it likely does not include things such as GMIN as if they were separate elements.
?
There is another option to disable the topology check that caused this error.
.options topologycheck=0
The description is: "Set to zero to skip check for floating nodes, loops of voltage sources, and non-physical transformer winding topology".
?
Andy
?
|
Re: PWM Timing Causing Shoot-thru
Ahhh thank you guys for explaining the distinction. It seems obvious now the difference between the .sub and the .asy.
?
I have re-uploaded my zip with the .asy.
?
?
Thanks!
-May
|
Re: 12AU7 tube heater model
On Fri, Feb 21, 2025 at 06:01 AM, Andy I wrote:
The spike around 160 mA is the "singularity" I mentioned earlier.
?
This shows how the Duncan Amps heater model fails, when the heater's temperature becomes too great.? The resistance hits the singularity, then goes negative, causing the heater to generate energy instead of dissipating it.
Very good. By using Gmin stepping iteration, the spike is at 166 mA. Starting from 167 mA the heater resistance becomes negative and, as you highlighted, the Duncan Amps heater model begins to fail.
?
By the way, you can eliminate that error message, by adding a 1T resistor across the heater. ?That stops LTspice from thinking the nodes are floating.
?
BTW, on LTspice Control Panel->Hacks! tab there is a checkbox named "Add GMIN across current sources".?Is it supposed to "address" such a problem/error related to the current source's infinite impedance ?
?
?
|
Re: PWM Timing Causing Shoot-thru
It's not the model that's missing, it the symbol: IR2110.asy.
--
Regards,
Tony
On 21/02/2025 15:18, May via groups.io
wrote:
toggle quoted message
Show quoted text
I am still checking this thread.
?
I did include IR2110.sub in the zip file. I
just downloaded my zip, extracted it to a folder and was able to
run the simulation without any issues.
?
You are most likely absolutely correct about the "C" signals;
I have not yet touched those. Was focused on "A" and "B".
|
Re: PWM Timing Causing Shoot-thru
On Fri, Feb 21, 2025 at 09:18 AM, May wrote:
I did include IR2110.sub in the zip file. I just downloaded my zip, extracted it to a folder and was able to run the simulation without any issues.
Please read carefully.? You did not upload the SYMBOL file, which is IR2110.asy.? That file is missing from the .zip that you uploaded.? Having the model file does no good when the symbol file isn't there.
?
Of course it works fine on YOUR computer, because you have that symbol file already, somewhere in YOUR computer.? But we don't.? When I open your schematic, there is an error message, and there are "holes" on your schematic where the IR2110 symbol was supposed to be.? And I can't run the simulation without it and get meaningful results.
?
Andy
?
|
Re: using LTSPICE symbols for representation of spice netlist of OPAMP
On Fri, Feb 21, 2025 at 09:03 AM, john23 wrote:
Is there a way to plug somehow the attached CIR file to standart LTSPICE symbol.
(in AD797 they also have extra decompensation pin)
What could be done ??
No you can't use the normal op-amp symbol directly, because of that extra pin.? The normal op-amp symbol is "opamp2", and it works for the majority of op-amps.? But not this one.
?
Here is something to consider doing.? Make a copy of the opamp2 symbol.? Then edit that symbol (in LTspice's symbol editor) to add the extra decompensation pin, and save the symbol with a new name, in your own symbol library.
?
Alternatively, start searching through the vast numbers of Analog Devices op-amps that come with LTspice, until you find another one that has an extra pin but still looks like an op-amp.? Make yourself a copy of that one.
?
If you know that you will never use the decompensation pin, there is another alternative:? Wrap a 5-pin subcircuit around the Analog Devices AD797 model, and don't bring that extra pin out to the outer subcircuit.? Now you have a 5-pin subcircuit, which CAN be used with the built-in "opamp2" symbol.
?
.SUBCKT MyAD797 In+ In- V+ V- Out
X? In+ In- V+ V- Out Decomp? AD797
.LIB AD797.cir
.ENDS MyAD797
?
Andy
?
|
Re: using LTSPICE symbols for representation of spice netlist of OPAMP
Yes, you can take a standard symbol, edit the attributes, and save it as a "new" *.asy file. Easy peasy.
|
Re: 12AU7 tube heater model
The model is obviously seriously wrong. I?
really can't see why a simple formula Rhot = Rcold*(1 +aT +
bT^2)? could not be used. That can't possibly 'blow up'. T =
Thot - Tcold.
On 2025-02-21 14:01, Andy I via
groups.io wrote:
Carlo,
?
In your latest uploaded file (12AU7heater.zip), try this:?
Plot V(n001)/I(I1), which shows the effective resistance of the
Heater.? Change the .DC sweep past 160m, to 200m.? (.dc I1 120m
200m 1m)
?
It will be difficult to see what happens, because the
resistance goes "through the roof" around 168 ma.? But above
that spike, the resistance becomes negative.? Click on the
plotted formula at the top of the plot to enable the waveform
"cursors", then drag the vertical cursor to the right, while
noting the resistance values in the pop-up window.? To the right
of the spike, they are negative.
?
The spike around 160 mA is the "singularity" I mentioned
earlier.
?
This shows how the Duncan Amps heater model fails, when the
heater's temperature becomes too great.? The resistance hits the
singularity, then goes negative, causing the heater to generate
energy instead of dissipating it.
?
By the way, you can eliminate that error message, by adding a
1T resistor across the heater.? That stops LTspice from thinking
the nodes are floating.? Adding the 1T resistor changes the
location of the singularity where the heater model "blows up",
but it still has negative resistance when it gets too hot.
?
Andy
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: PWM Timing Causing Shoot-thru
Hi Andy!
?
I am still checking this thread.
?
I did include IR2110.sub in the zip file. I just downloaded my zip, extracted it to a folder and was able to run the simulation without any issues.
?
You are most likely absolutely correct about the "C" signals; I have not yet touched those. Was focused on "A" and "B".
?
Thanks!
-May
|
Re: 12AU7 tube heater model
On Fri, Feb 21, 2025 at 09:06 AM, John Woodgate wrote:
I see; the notation is confusing. But is the synthetic resistor then allowed to be zero ohms?
Hmm.? Define "zero ohms".? :-)
?
The current through the G-source can become zero, which it does when the voltage across it is zero.? It isn't zero ohms in that case.
?
I suppose it could become zero ohms too, but I am not sure if LTspice can handle the math for that, as a G-source.? Maybe an E-source would be better for that.
?
?
?
|
Re: 12AU7 tube heater model
I see; the notation is confusing. But is the
synthetic resistor then allowed to be zero ohms?
On 2025-02-21 13:42, Andy I via
groups.io wrote:
On Fri, Feb 21, 2025 at 08:20 AM, John Woodgate wrote:
The term v(u1:hb,0)
is in the denominator of the function and I think it is zero
at startup.
It is in the numerator.
?
There are no parentheses around "(42
- 6.2)*v(u1:hb,0)".? Only "(42
- 6.2)" is in the denominator.
?
Andy
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
using LTSPICE symbols for representation of spice netlist of OPAMP
Hello, In ltspice there are many modles and I like to use the standart symbols to represent the model.
When I create model from a netlist at worst I use a recrangle with pins? and at best I try to draw opamp by myselse and? the result genrally is not looking good.
Is there a way to plug somehow the attached CIR file to standart LTSPICE symbol.
(in AD797 they also have extra decompensation pin)
What could be done ??
Thanks.
?
/g/LTspice/files/Temp/ad797.cir
|
Re: 12AU7 tube heater model
Carlo,
?
In your latest uploaded file (12AU7heater.zip), try this:? Plot V(n001)/I(I1), which shows the effective resistance of the Heater.? Change the .DC sweep past 160m, to 200m.? (.dc I1 120m 200m 1m)
?
It will be difficult to see what happens, because the resistance goes "through the roof" around 168 ma.? But above that spike, the resistance becomes negative.? Click on the plotted formula at the top of the plot to enable the waveform "cursors", then drag the vertical cursor to the right, while noting the resistance values in the pop-up window.? To the right of the spike, they are negative.
?
The spike around 160 mA is the "singularity" I mentioned earlier.
?
This shows how the Duncan Amps heater model fails, when the heater's temperature becomes too great.? The resistance hits the singularity, then goes negative, causing the heater to generate energy instead of dissipating it.
?
By the way, you can eliminate that error message, by adding a 1T resistor across the heater.? That stops LTspice from thinking the nodes are floating.? Adding the 1T resistor changes the location of the singularity where the heater model "blows up", but it still has negative resistance when it gets too hot.
?
Andy
?
|
Re: 12AU7 tube heater model
On Fri, Feb 21, 2025 at 05:37 AM, Andy I wrote:
In the expanded netlist, Ghot connects to nodes U1:HB and 0.? U1:HB connects to the 1 milohm sense resistor, whose other end goes to U1:HA, which then connects through 6.2 ohms to node N001.? N001 is the one driven by the independent current source.? So the whole string of nodes N001, U1:HA, and U1:HB appear to be "floating" in the topology check.
Ah ok. The point is that, by removing both the independent current source I1 and the G-source Ghot from the overall topology, the topology check realizes that there is the series/string of R:U1:cool and R:U1:load resistors (connecting node N001 with U1:HB passing through the intermediate node U1:HA) that are actually disconnected from the rest of the circuit. Therefore the topology check complains that U1:HB node is floating and connected to the (controlled) current source G:U1:HOT.
?
?
|
Re: Looking for advice on TRAN timing
#FFT
If you're interested, I have a new tool, which is somewhat faster
than the Analyser you mentioned and just as accurate.
I don't know for sure whether using (maximum) timesteps of binary
fractions of the period are better, or not, but it is convenient.
You might also find THD_Measurement_Test_Results.pdf
useful. It shows the THD measurement floor as you increment the
exponent, "n", in the expression Tmax = Period/2**n. There's no
point in making Tmax shorter than necessary as it just makes the
simulation slower for no benefit.
--
Regards,
Tony
On 21/02/2025 13:34, Ryu via groups.io
wrote:
toggle quoted message
Show quoted text
I'm looking for help concerning the timing parameters of a
TRAN simulation
to evaluate the distortion of an amplified sine wave.
?
I've been reading through lots of messages of this group
concerning "distortion" and "tran timing"
recently but could not find an answer to what I was looking
for.
[I came across the audio distortion analyser contributed by Tony
Casey,
for which I am thankful and it is indeed a fine tool.]
?
Hitherto I've used 1 or 2 per mille of the sine wave period,
so the time step would be 1 usec or 2 usec
when testing with 1 kHz. From my tests I decided for myself
that values exceeding 1% of the period
should best be avoided.
I also tested time steps adjusted to the power of 2, e.g. 2**14
(interval / 16384).?
?
For the interval (t_stop - t_start) I usually take 16msec
when testing with 1kHz
but I have also used values from 10msec to 48msec.
It is this parameter which I personally find most difficult
to decide upon.
?
So, to sum it all up, I wonder if there is a guideline which
values to use for the time step
and the interval for a certain test frequency when testing
audio related circuits with sine waves.
(I'm still using LTspice XVII.)
|
Re: 12AU7 tube heater model
On Fri, Feb 21, 2025 at 08:20 AM, John Woodgate wrote:
The term v(u1:hb,0) is in the denominator of the function and I think it is zero at startup.
It is in the numerator.
?
There are no parentheses around "(42 - 6.2)*v(u1:hb,0)".? Only "(42 - 6.2)" is in the denominator.
?
Andy
?
|
Re: 12AU7 tube heater model
On Fri, Feb 21, 2025 at 08:07 AM, Carlo wrote:
Looking at the complete circuit topology, U1:H2 node is the node where the subckt G-source Ghot joins the external DC independent current source (I1). In the overall circuit this U1:H2 node is connected to GND (0). However U1:HB isn't the node where the two current sources (internal and external) actually join.
I think you are confused about nodenames.
?
There is no U1:H2 node.
?
U1:H2 is a portion of the names of elements R:U1:H2 and C:U1:H2.? There is nothing named U1:H2, neither a node nor an element.
?
In the expanded netlist, Ghot connects to nodes U1:HB and 0.? U1:HB connects to the 1 milohm sense resistor, whose other end goes to U1:HA, which then connects through 6.2 ohms to node N001.? N001 is the one driven by the independent current source.? So the whole string of nodes N001, U1:HA, and U1:HB appear to be "floating" in the topology check.
?
Andy
?
|
Re: 12AU7 tube heater model
The term v(u1:hb,0) is in the
denominator of the function and I think it is zero at startup.
On 2025-02-21 13:07, Carlo wrote:
On Fri, Feb 21, 2025 at 04:31 AM, Andy I wrote:
But LTspice doesn't know this.? It sees the circuit
topology as a current source connected to another current
source, and it thinks the node where they join is "floating".?
So it generates the error message, but it continues to process
the netlist anyway, and everything works!
Looking at the complete circuit topology, U1:H2 node is the node
where the subckt G-source Ghot joins the external DC independent
current source (I1). In the overall circuit this U1:H2 node is
connected to GND (0). However U1:HB isn't the node where the two
current sources (internal and external) actually join.
?
Here the expanded netlist:
? ? --- Expanded Netlist ---
*
C:\Users\carlo\Documents\LTspice\Bravo_Ocean_ampli\12AU7heater.asc
r:u1:cool n001 u1:ha 6.2?
r:u1:load u1:ha u1:hb 1m
b:u1:§esens u1:hd 0 v=v(u1:ha,u1:hb)*1000?
b:u1:§epwr u1:he 0 v=v(n001,0)*v(u1:hd)/(pwr(6.3 ,2)/ 42)
r:u1:h1 u1:he u1:hf 91k
c:u1:h1 u1:hf 0 1.05e-05?
b:u1:§eh2 u1:hg 0 v=v(u1:hf)?
r:u1:h2 u1:hg u1:hh 270k
c:u1:h2 u1:hh 0 1.05e-05?
b:u1:§eh3 u1:hj 0 v=limit(v(u1:hh)-0.75,0,1e6)*4?
r:u1:h3 u1:hj u1:hk 91k
c:u1:h3 u1:hk 0 1.05e-05?
b:u1:§ghot u1:hb 0 i=(1/(v(u1:hg)+0.001))/(42 -
6.2)*v(u1:hb,0)
i1 0 n001 150m
.dc i1 120m 160m 1m
.end
?
ERROR: Node U1:HB is floating and connected to
current source G:U1:HOT
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
John Woodgate
Carlo
Tony Casey