Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
BTW, .option Noopiter in LTspice skips Direct Newton-Raphson (NR) iterations to calculate the ITS/DC operating point. Using default settings, LTspice will try Direct NR to calculate the ITS/DC operating point.
?
How many "Direct NR" iterations are allowed to run before giving up (no convergence achieved) and start using homotopies (i.e. gmin stepping, source stepping etc..) ?
?
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
On Wed, Mar 5, 2025 at 01:22 AM, Andy I wrote:
NGSPICE has had a VDMOS model since release 32 (current is 44.2).
That is what I heard.? BUT -- Is it the same as LTspice's VDMOS?? ?That is,
did ngspice try to copy LTspice's VDMOS?? How successfully did they copy
LTspice's VDMOS?
We know exactly what ngspice is doing: (reading the source of the intrinsic model implementation, it is the standard DMOS and discrete SPICE diode model but has a thermal output node). According to the help, the LTspice model has a nonstandard Cgd(V) characteristic, and the anti-parallel diode is (of course) not like the substrate diode of a monolithic device. I don't think ngspice tries to copy LTspice, both try to approximate the same datasheet from the same parameters supplied by a .model line. Neither implementation is likely to produce nVs where Volts are expected. -marcel
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
On Wed, Mar 5, 2025 at 04:27 AM, Andy I wrote:
I am uncertain what you suggested.? Why would either simulator use a "small signal linear equivalent circuit" for the transient simulation of something which is or might? be nonlinear?? Shouldn't it always solve the non-linear equations at each timestep?? That is how it is supposed to work, isn't it?
Ok yes, for transient analysis it is supposed to work that way. Therefore, at the end of transient analysis, there will be a total number of iterations done (some associated with ITS calculation and others to solve non-linear equations at successive timesteps until the end).
?
Using a small-signal linear equivalent circuit makes sense only for .AC analysis.
Ok, the above is made explicit in ngspice manual's section for .AC analysis. However, in the case at hand, even .AC analysis for both simulators doesn't provide a reasonable/good result (since the calculated DC operating point isn't reasonable).
?
Carlo
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
On Wed, Mar 5, 2025 at 05:48 AM, Carlo wrote:
Btw, as far as I understood, transient simulation doesn't use the same "small signal linear equivalent circuit" for non-linear devices (i.e. diodes, bjt, mos etc..). Instead at each timestep it leverages on the solver (possibly iterating to solve non-linear equations) to work out circuit's voltages and currents.
I am uncertain what you suggested.? Why would either simulator use a "small signal linear equivalent circuit" for the transient simulation of something which is or might? be nonlinear?? Shouldn't it always solve the non-linear equations at each timestep?? That is how it is supposed to work, isn't it?
?
Using a small-signal linear equivalent circuit makes sense only for .AC analysis.
?
Andy
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
On Wed, Mar 5, 2025 at 03:23 AM, <mhx@...> wrote:
NGSPICE has had a VDMOS model since release 32 (current is 44.2).
That is what I heard.? BUT -- Is it the same as LTspice's VDMOS?? ?That is, did ngspice try to copy LTspice's VDMOS?? How successfully did they copy LTspice's VDMOS?
?
Or does ngspice do a completely different VDMOS model?? Does this fall under the "VDMOS means different things to different people" which I suggested?
?
Andy
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
On Tue, Mar 4, 2025 at 05:06 PM, Andy I wrote:
It looks like you used LTspice's schematic and transistor models (standard.???) in both simulations.? That MIGHT be a problem.? LTspice's discrete MOS models in standard.mos all use LTspice's proprietary "VDMOS" (Vertical Double-Diffused power MOSfet) model, which is a little different than SPICE's ordinary MOS models.? I don't know what ngspice does with the VDMOS model definition.
?
There is a chance that ngspice handles the IRF510 model incorrectly.
?
Thanks Andy, that's the point indeed ! I downloaded the following IRF510 model from
?
.MODEL IRF510 NMOS LEVEL=3 VTO=3.699 KP=20.82U RD=21.08M
+ RS=450.8M IS=202.7F CBD=366.6P
+ CGSO=604.9P CGDO=62.62P
?
LTspice and ngspice return exactly the same answer for ITS. However it isn't good enough since the amplifier's output signal isn't there (only some nV oscillating around 0V).
?
I let the simulation continue for 20 seconds (.tran 0 20 19) with no luck (with or without UIC to skip the ITS step). The output signal V(out1) isn't good at all both for LTspice and ngspice.
?
Btw, as far as I understood, transient simulation doesn't use the same "small signal linear equivalent circuit" for non-linear devices (i.e. diodes, bjt, mos etc..). Instead at each timestep it leverages on the solver (possibly iterating to solve non-linear equations) to work out circuit's voltages and currents.
?
Carlo.
?
?
?
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
On Tue, Mar 4, 2025 at 02:06 PM, Andy I wrote:
I don't know what ngspice does with the VDMOS model definition.
NGSPICE has had a VDMOS model since release 32 (current is 44.2). -marcel
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
Carlo, did you have succcess finding the ngspice user group?? (Not the brand new "AllSpice" group.)
?
Andy
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
Carlo,
?
I'm sorry that I am not currently able to give you direct help with the ngspice part of your question.? But here is another thing to consider.
?
It looks like you used LTspice's schematic and transistor models (standard.???) in both simulations.? That MIGHT be a problem.? LTspice's discrete MOS models in standard.mos all use LTspice's proprietary "VDMOS" (Vertical Double-Diffused power MOSfet) model, which is a little different than SPICE's ordinary MOS models.? I don't know what ngspice does with the VDMOS model definition.
?
There is a chance that ngspice handles the IRF510 model incorrectly.
?
(I'm also aware that "VDMOS" can mean different things to different people and their tools.)
?
To put both simulators on equal footing, try downloading an IRF510 model from the internet and plug it into both simulators.
?
Andy
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
On Tue, Mar 4, 2025 at 01:36 PM, Carlo wrote:
As you can check, .tran 100n 10m analysis gives quite different answers for ITS/DC operating point. Btw, as convergence aid, option noopiter gminsteps=0 is used in LTspice to skip direct NR and gmin stepping to get a "reasonable" ITS solution.
FYI, LTspice ignores the first parameter of the .TRAN command.? Therefore, ".tran 100n 10m" is identical to ".tran 0 10m" or ".tran 10m 10m".? In the old days of SPICE, the first parameter was the print step interval for SPICE's line-printer output.? ".tran 100n 10m" would have given you about 100,001 lines of waveform data, which might have spanned about two thousand pages (four reams) of paper in your line-printer.? LTspice never prints waveforms like that, so the first parameter is always ignored in LTspice.? Maybe ngspice still uses it for something; I don't know.? But that's off-topic anyway.
?
I have not used ngspice in years, so I can't try that simulation, but someone else here might.? Since ngspice's input is a SPICE Netlist, and since LTspice can simulate SPICE Netlists, did you also try simulating the ngspice netlist in LTspice?? It is a "sanity check", if nothing else.
?
Because your simulation uses the troublesome 12AU7 model which we already know has issues with multiple convergent operating points, it would not surprise me if differences were seen.? We saw that already, even from people using just one simulator (LTspice).? It's a flip of the coin whether it finds one initial operating point, or another, especially when they are both valid, mathematically.
For instance 12AU7's plate voltage is 12.8V for LTspice vs 22.6V for ngspice.
DC currents are also quite different and, in the end, output signal for ngspice isn't good at all even for a 1Khz amplifier's input signal.
Did you let the ngspice simulation continue for several more seconds, to see if it drifted towards a more appropriate operating point?? This might be just another case like the ones we had earlier with LTspice.? If the 12AU7 model, or any of the other models, do not handle out-of-bound conditions properly, then any simulator might find a mathematically valid but physically incorrect initial operating point.? That is really a problem with the model, not the simulator which is just doing its job.
?
I don't want to say that this IS the difference you saw, but it might be.
?
Andy
?
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
Carlo,
?
Remember that uploaded files should be uploaded to the "Temp" directory only.? As it says, "Do not upload your files here" where 'here' is the top-level directory -- and "Click 'Temp' first, before uploading."
?
Please re-read the group's guidelines on the group's main webpage.? It reminds you about this:
To upload:? First navigate to the?Temp?folder, then click the "New/Upload" button.
?
Andy
?
|
Re: opamp BW slew rate search engine sorting
On Tue, Mar 4, 2025 at 03:31 PM, john23 wrote:
Hello , The analog devices website is not aloowing to filter OPAMPs exactly by the BW slew rate etc parmater.
For example as you can see here.Its not allowing me to sort OPAMP models.
Why do you say that it does not allow you to sort bandwidth or slew rate columns?? It works for me.? Did you click on the up- and down-arrows at the top of the columns?? Was there something wrong about the sort orders you saw after doing that?
?
If it did not work the way you desired, did you send feedback to Analog Devices?? Most of their webpages have a link in the lower right corner for "Site Feedback".? And there is another one near the lower right corner for "How would you describe your experience with this page?"? I can't say if web features such as that are available in all parts of the world, but there PROBABLY is a way in your country for telling ADI how their webpage did not meet your expectations.
?
The group you are in is about LTspice.? It's not a forum to complain about someone's website, even if that 'someone' is the same company that releases LTspice.? Their part selector pages have nothing to do with LTspice.? The group you are in is not run by Analog Devices, and complaining here has no assurance of reaching anyone at Analog Devices..
?
Andy
?
|
Re: Model of TDA2822, Dual Low-Voltage Audio Amplifier
I have tested it, and it seems to work quite
well. But read the data sheet with care.
On 2025-03-04 20:36, Kerim via
groups.io wrote:
On Tue, Mar 4, 2025 at 10:56 PM, John Woodgate wrote:
Have you asked ST Micro if they have a SPICE model
(not an 'LTspice model')?
During the search, I heard someone in a forum who did and didn't
get a reply.
I think I will likely have to test it in real if no one here
heard of it.
Thank you.
?
--
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: Model of TDA2822, Dual Low-Voltage Audio Amplifier
On Tue, Mar 4, 2025 at 10:56 PM, John Woodgate wrote:
Have you asked ST Micro if they have a SPICE model (not an 'LTspice model')?
During the search, I heard someone in a forum who did and didn't get a reply.
I think I will likely have to test it in real if no one here heard of it.
Thank you.
?
|
opamp BW slew rate search engine sorting
Hello , The analog devices website is not aloowing to filter OPAMPs exactly by the BW slew rate etc parmater.
For example as you can see here.Its not allowing me to sort OPAMP models.
Is there some catalog search engine you reccomend where I could sort OPAMPS by their properties?
https://www.analog.com/en/product-category/high-voltage-op-amps-greaterthanequalto-12v.html#products-in-category
?
Thanks.
|
Re: Model of TDA2822, Dual Low-Voltage Audio Amplifier
Have you asked ST Micro if they have a SPICE
model (not an 'LTspice model')?
On 2025-03-04 19:42, Kerim via
groups.io wrote:
Hello,
?
In vain, I
searched its model (TDA2822) in the group¡¯s archive and on the
internet.
?
It is suitable
for 32 Ohm headphone with an electret microphone and 2*1.5V
battery.
?
I have one ear
working and its sensitivity has been degraded because of age.
TDA2822 gain is
fixed (39 dB = 89 V/V). In the bridge configuration (mono),
its output voltage limit is doubled.
?
Is there any
chance to find its LTspice model?
?
Thank you.
Kerim
--
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
|
Model of TDA2822, Dual Low-Voltage Audio Amplifier
Hello,
?
In vain, I searched its model (TDA2822) in the group¡¯s archive and on the internet.
?
It is suitable for 32 Ohm headphone with an electret microphone and 2*1.5V battery.
?
I have one ear working and its sensitivity has been degraded because of age.
TDA2822 gain is fixed (39 dB = 89 V/V). In the bridge configuration (mono), its output voltage limit is doubled.
?
Is there any chance to find its LTspice model?
?
Thank you.
Kerim
|
Re: LTspice vs ngspice 12AU7 tube amplifier transient analysis
Ok, I'll try asking..
?
I uploaded both LTspice .asc schematic and ngspice .cir netlist including the libraries for subckts referenced.
?
As you can check, .tran 100n 10m analysis gives quite different answers for ITS/DC operating point. Btw, as convergence aid, option noopiter gminsteps=0 is used in LTspice to skip direct NR and gmin stepping to get a "reasonable" ITS solution.
?
ngspice .tran however converges to a quite different ITS solution. For instance 12AU7's plate voltage is 12.8V for LTspice vs 22.6V for ngspice. DC currents are also quite different and, in the end, output signal for ngspice isn't good at all even for a 1Khz amplifier's input signal.
?
I've no idea why their ITS solutions are so different though...
?
Carlo.
?
?
|
Re: More syntax issues with 24.1.x
On Tue, Mar 4, 2025 at 01:53 PM, Tony Casey wrote:
On 04/03/2025 13:14, Mathias Born via groups.io wrote:
Yes, this won't work anymore. Prior versions pre-process the input and replace the .include line with the contents of the included file and then parse everything all over again. 24.1 is very different, it doesn't accept a top-level directive in the middle of something.
But you don't actually need such general behavior, all you want is to load data from another file, and that's certainly useful. How about extending the table syntax:
?
B1 1 2 I=table(V(3,4), "BC848B_Ic_Vce_400u.inc")
No, that doesn't work, either, in any version.
Even if this did work, I have hundreds of instances like this. It's a lot less pain to stick with 24.0.12.
Sorry, that was a misunderstanding. The above syntax was a proposal for a future change. This is about a compromise. The old way can't come back. I'm open for suggestions.
And modifying all those netlists could be done in one go with grep. (Or much better, with
?
Best Regards,
Mathias
?
|
Re: More syntax issues with 24.1.x
On 04/03/2025 13:14, Mathias Born via
groups.io wrote:
Yes, this won't work anymore. Prior versions pre-process the
input and replace the .include line with the contents of the
included file and then parse everything all over again. 24.1 is
very different, it doesn't accept a top-level directive in the
middle of something.
But you don't actually need such general behavior, all you
want is to load data from another file, and that's certainly
useful. How about extending the table syntax:
?
B1 1 2
I=table(V(3,4), "BC848B_Ic_Vce_400u.inc")
No, that doesn't work, either, in any version.
U:\Simulations\LTspice\Modelling_Bipolar\BC847_BC857\OP_Characteristic_rounding.net(17):
Invalid number of arguments.
B1 1 2 I=table(V(3,4) "BC848B_Ic_Vce_400u.inc" )
?????????????? ^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
With or without a comma between "V(3,4)" &
"BC848B_Ic_Vce_400u.inc" the same error results. Doesn't look like
the file is being included.
Even if this did work, I have hundreds of instances like this. It's
a lot less pain to stick with 24.0.12.
--
Regards,
Tony
|
Carlo
John Woodgate
Tony Casey