I think you are missing the point of simulations. It is not to have something totally accurate, it’s to debug your ideas, find there limitations, weaknesses and requirements before prototyping.
Simulation and prototyping are complimentary tools for getting the job done.
I’m really grateful to people that enjoy simulation and are willing to share their work and face public constructive criticism. But being critical because you don’t like completely accurate simulation tools is not a fair critique.
Simulation and prototyping are complimentary tools for getting the job done.
I’m really grateful to people that enjoy simulation and are willing to share their work and face public constructive criticism. But being critical because you don’t like completely accurate simulation tools is not a fair critique.
On this subject, I built my amp first, and only after I started playing with LTspice. I have to say that the simulation was quite good, even instability when increasing gNF on the real amp was accurately shown. Is not perfect, by any means, but it is an excellent complementary tool.
Nothing beats prototyping with the real hardware though, at least for me.
Nothing beats prototyping with the real hardware though, at least for me.
A bit late…
Change the inductance until you approximate your -3dB point in low-frequency and then change the coupling coefficient (K) until you get the -3dB point at high-frequency.
I don’t know what to suggest for inductance, Mullard values might be close enough.
Change the inductance until you approximate your -3dB point in low-frequency and then change the coupling coefficient (K) until you get the -3dB point at high-frequency.
I don’t know what to suggest for inductance, Mullard values might be close enough.
HAMMOND 125A universal PUSH-PULL Output Transformer
For diyaudio fellow JoeAlders I made a hierarchical model of the Hammond 125A.
He was working on the Lingwendil flea amplifier project
https://www.diyaudio.com/community/threads/6sn7-push-pull-flea-amplifier-project.303846/
Based on the datasheet (and a 125A that Joe kindly sent me to take some measurements) I created this model. Measuring a transformer with simple equipment is not a trivial task, as we both experienced. The transformer K calculated from my L measurements was too high when looking at the frequency response. To correct this discrepancy, I cheated and adjusted K to match the LTspice results with my 3k-8 frequency response measurements. So there is certainly room for improvement.
The LTspice simulation of the ampfifier is made by Joe.
happy diy,
Ite
NOTE:
By adjusting a few parameters you can easily convert this 125A model to another type from the 125A..E series. Start with changing Lpp, R-brown/blue, and Rs-total, and go from there.
For diyaudio fellow JoeAlders I made a hierarchical model of the Hammond 125A.
He was working on the Lingwendil flea amplifier project
https://www.diyaudio.com/community/threads/6sn7-push-pull-flea-amplifier-project.303846/
Based on the datasheet (and a 125A that Joe kindly sent me to take some measurements) I created this model. Measuring a transformer with simple equipment is not a trivial task, as we both experienced. The transformer K calculated from my L measurements was too high when looking at the frequency response. To correct this discrepancy, I cheated and adjusted K to match the LTspice results with my 3k-8 frequency response measurements. So there is certainly room for improvement.
The LTspice simulation of the ampfifier is made by Joe.
happy diy,
Ite
NOTE:
By adjusting a few parameters you can easily convert this 125A model to another type from the 125A..E series. Start with changing Lpp, R-brown/blue, and Rs-total, and go from there.
The HF -3dB point is a good start, but lurking behind is the ugly resonance caused by the series cap (prim. to sec.).
This is what I found when modifying my Leak ST60: -3dB@55KHz, dip@70KHz, and peak@90KHz
@Ite: thanks for your model; it allows the parasitic caps to be specified. However, in order to approximate the actual response above, I need to use around 10nF between prim. and sec., but the actual measured value is about 2nF. Any thoughts?
This is what I found when modifying my Leak ST60: -3dB@55KHz, dip@70KHz, and peak@90KHz
@Ite: thanks for your model; it allows the parasitic caps to be specified. However, in order to approximate the actual response above, I need to use around 10nF between prim. and sec., but the actual measured value is about 2nF. Any thoughts?
LEAK-8615 transformer model
@Zung,
I am not a transformer expert, more an LTspice WYSIWYG transformer model promoter.
In your Leak-enstein thread I saw the Ray Whitcombe info on how the transformer is constructed internally.
I made a model that follows that recipe and got some promising results!
happy diy,
Ite
@Zung,
I am not a transformer expert, more an LTspice WYSIWYG transformer model promoter.
In your Leak-enstein thread I saw the Ray Whitcombe info on how the transformer is constructed internally.
I made a model that follows that recipe and got some promising results!
happy diy,
Ite
Hi Mo,
The asymmetry is caused by the distortion in the "out" signal. (use control-L to show it in the error log)
When you re-run the simulation with a lower input signal, the signal will have lower distortion and the symmetry will be better.
The distortion is not caused by the transformer model. It is only a simple lumped model, that doesn't incorporate core-saturation.
Press Right Mouse Button on the transformer, and click [Open Schematic] to view the model used.
The example circuit with the EL34 is only to show how to use the transformer model. It is by no means a perfect circuit.
happy diy,
Ite
The asymmetry is caused by the distortion in the "out" signal. (use control-L to show it in the error log)
When you re-run the simulation with a lower input signal, the signal will have lower distortion and the symmetry will be better.
The distortion is not caused by the transformer model. It is only a simple lumped model, that doesn't incorporate core-saturation.
Press Right Mouse Button on the transformer, and click [Open Schematic] to view the model used.
The example circuit with the EL34 is only to show how to use the transformer model. It is by no means a perfect circuit.
happy diy,
Ite
Hi, inhave been interested in this topic recently, and wondering what to measure on the output transformers to be able to judge their merit before trying to use them.
DC resistance of primaries and seconaries
primary inductance (at what frequency?)
secondary inductance
capacitance
overall weight
turns ratios
i have a de-5000 LCR meter that measures at 100, 120, 1000, 10000, and 100000hz, and it can within some limitations measure resitance, inductance, capacitance, both series and parallel. Also gives Q, and ø (not sure how to make a proper theta on this iPad). I have a bunch of other test equipment too if needed.
I’m Going to look closer at the models people have made and see if I can make sense of any of this…
DC resistance of primaries and seconaries
primary inductance (at what frequency?)
secondary inductance
capacitance
overall weight
turns ratios
i have a de-5000 LCR meter that measures at 100, 120, 1000, 10000, and 100000hz, and it can within some limitations measure resitance, inductance, capacitance, both series and parallel. Also gives Q, and ø (not sure how to make a proper theta on this iPad). I have a bunch of other test equipment too if needed.
I’m Going to look closer at the models people have made and see if I can make sense of any of this…
When using a iron core transformer Spice can be close at 1Khz in my experience.
However due to the lack of modeling of eddy current losses, magnetic hysteresis, magnetic saturation, non-linear permeability with current, very limited modeling of stray inductance and capacitance I find the results far less accurate than I would like at 20KHz or 20Hz.
Bench proto type amplifiers using iron core transformer normally perform significant different than in spice at 20Hz and 20KHz due to the above in my experience.
In the case of amplifiers that do NOT include iron core transformers the spice and the bench version will normally match very well from sub 1Hz to out into the 100s of KHz. Not so when iron core transformer are part of the spice models used.
The iron core transformer models I have seen so far (and created myself) fail to properly capture amplifier performance at the 100KHz or more needed to accurately model the feedback loops high frequency stability.
There is a long history of limited spice models for transformers and I see this as a weak point in spice modelling tube amplifiers.
Some of the transformer models devised to simulate switch mode power supplies capture more of the magnetic and high frequency issues I mention above with better fidelity. It is however difficult to characterize many of these parameters from measured samples in the first place let alone accurately model them.
Modeling a single inductor let alone a full transformer with many taps at high frequencies can be very complex.
I confess to lacking the mathematical chops to create improved transformer models but certainly yearn for them.
Here is a example that adds a bit more high frequency detail to the model but still leaves out much of the important stuff.
Getting the needed parameters for the model is unfortunately not easy and then there is the tolerance of each real transformer sample measured.
https://www.coilcraft.com/en-us/models/howto/simulation-model-considerations-part-ii-(1)/
This is a large complex subject.
But sadly I find some people use these simulations as an online weapon to argue that a certain actually built amplifier can't perform as reported "because in my sim of it doesn't perform well", when the actual amp works well and sounds great! Then they start making suggestions on how to improve it based on their changes to make it sim better, rather than deferring to the person who actually built and measured a real example. My fear is when these folks start posting let's say the transformer impedance is wrong, other viewers will believe their info based on a sim of the circuit and waste money building the amplifier wrong.
In the past I've personally tried their "mods" to the actual amp and most of the time it either hurts the performance or sounded much worse. And when I report this, these same folks will argue I either am incompetent and did it wrong, or that I don't know how to measure an amp. IMHO these sims could be helpful in seeing if the voltages and some minor design details work, but that same info can be calculated with ohms law and a tube data sheet. As far as amp performance, the models for the parts used in tube amps just aren't close enough.
There is nothing wrong with using LTSpice for simulation, provided one does not take it as a gospel of truth. I have had both "bad" and "good" advice from LTSpice on enhancements, some resulted in worse performance, others improved things. It is a useful tool, but nothing more than that. One can have the latest greatest Tektronix oscilloscope and still design a crappy sounding amp 🙂.
Oh yes.
But it seems that with sim lot of engineers come out publishing some diagrams that, honestly, sometimes are difficult to understand; in most case there is a mix of sand and vacuum!!!!!!!!!
Simply because the sim tells the something good comes out from them.
Different is to stay on desk, spending money, make a lot of solder point, having a real generator and a real test set up.
My ego is very proud to see that hardware I built is running an sounding good!
(my pocket something was crying!!!)
Walter
Actually simulation is very good for telling you something does not work. The tube models are usually very good. The transformer models really only exist for linear simulation. You can approximate the frequency and phase response by duplicating the measurement setup and curve fitting. This is normally good enough for getting the feedback right. It will tell you if your amp has a bulge at 1Hz or is likely to go off at 100KHz. Most models don't include max ratings. All LTP's will be perfectly balanced. Really its as good as the models are - but you have to ask the right questions.
This hierarchical SE transformer model is different from the previous one.
This model has a non-linear Chan core that takes into account the transformer size and magnetic properties of the laminated core.
The LTspice implementation of a multi winding Chan-core transformer is based on the work of the late analogspiceman.
Calculation of the core geometry A, Lm, and Lg for an EI transformer is based on the 'Peter Blanken' transform.
happy diy,
Ite
This model has a non-linear Chan core that takes into account the transformer size and magnetic properties of the laminated core.
The LTspice implementation of a multi winding Chan-core transformer is based on the work of the late analogspiceman.
Calculation of the core geometry A, Lm, and Lg for an EI transformer is based on the 'Peter Blanken' transform.
happy diy,
Ite
Last edited:
It would be great to understand more about how the model works, do you have the reference you can post?
Here are some files from analogspiceman, and the 1991 IEEE paper "Nonlinear transformer model for circuit simulation"
https://ltwiki.org/files/adventures_with_analog/magnetics/
further information on the LTwiki site:
https://ltwiki.org/index.php?title=Transformers
https://ltwiki.org/index.php?title=The_Chan_model
https://ltwiki.org/files/adventures_with_analog/magnetics/
further information on the LTwiki site:
https://ltwiki.org/index.php?title=Transformers
https://ltwiki.org/index.php?title=The_Chan_model