LTSpice model for output transformer

[hkc]

I'm trying to do a SPICE model for the amp I'm building but I have run into a difficulty around the transformers.
I have a Hyeboer 18W HT-6135 output transformer. I know the turns ratios an nominal impedance in ohms but SPICE wants the impedance in Henrys.

I have tried measuring the impedances but although I have a decent oscilloscope I don't have an even half way decent signal generator so I didn't get very far with that.

The primary to secondary turns ratios and impedences in ohms are

Yellow 48:1 3 ohm
Green 27:1 7 ohm
Orange 22:1 15 ohm

When I get this working I'm going to try modeling the power supply and then I'll need to do it again with a much more complex transformer.

Thanks for any pointers.

Hank

[jazbo8]

18W OPT SPICE Model

Try this one, it should be pretty close...

.SUBCKT 18W_OPT P1 B P2 O16 O8 O4 Com
* Push Pull Transformer
* 10800 to 16 Ohms, -3db 80 to 15000 Hz
* Taps at 4 and 8 Ohms
* Heyboer_HT-6135
*   
LP1 1 B 2.71099224897965
LP2 2 P2 2.71099224897965
LA1 5 O8 0.00263122532543707
LA2 6 O4 0.00131561266271854
LA3 7 Com 0.00766795252904828
KALL LP1 LP2 LA1 LA2 LA3 0.975660566768592
RP1 P1 1 80
RP2 B 2 80
RS1 O16 5 8
RS2 O8 6 4
RS3 O4 7 3
.ENDS 18W_OPT

[hkc]

Many thanks!
What should I do about the floating secondaries?
I have connected a dummy load to the 8 Ohm outputs but the others were left unconnected as they would be in reality.
SPICE doesn't seem to like the fact that only one tap is used but I fear that putting dummy loads on the other taps might change the dynamics of the circuit.

Do I need to mention that I am a total newbie to amps and to spice?

Best regards,
Hank

[jazbo8]

You can leave the un-used pins open, as long as you ground the "Com" pin. Try it, if you still have problems, let me know.

[hkc]

Strange simulation results

Strange simulation results. [I have attached the LTSpice netlist file. Extension is changed from .asc to .txt following the rules of this forum. You will probably need to change it back to .asc to get LTSpice to run it.]

I have made this LTSpice model of an amp (Mostly copied from Doug Hoffman's Stout design. I have tweaked it a bit to get a better balance in the phase inverter and added a speaker model from the Fender amp model on the LTSpice yahoo group site.

I'm finding some strange simulation results. Actually I'm such a newbie that any simulation results are likely to be strange.
Anyway the design is extremely sensitive to the volume control. Using a plog taper pot for volume things work fine up to a wiper position of about 86%. Even slightly over that and the simulation doesn't converge. I'm wondering if this is a problem with the design or a problem with some part of the spice model. When things fail it looks like the inverted output of the phase inverter has started clipping and some kind of noise or oscillation appears in the simulation. Also the power tube plate circuit shows extremely high voltages with noisy peaks over 1KV.

Any insights or hints would be greatly appreciated.

Hank

[jazbo8]

I think C6 isn't connected correctly, the clue is the large difference in the plate load resistors for the LTP... also I am not sure about the SPICE models that you used for the tubes, so I modified the file and it seems to run better now.

[hkc]

Thanks!!!

I think C6 isn't connected correctly, the clue is the large difference in the plate load resistors for the LTP... also I am not sure about the SPICE models that you used for the tubes, so I modified the file and it seems to run better now.

Jazbo8,
Thanks so much. Connecting C8 directly to ground definitely fixes the balance problem.
I haven't tried your tube models yet. I'll do that next.
The models I used were the Rydel models available from eurexcem.com website
Your models are newer and look significantly more complex.

I have now also found your blog on the subject. Looks like I will be busy reading for a while

Hank

[jazbo8]

I found the Ayumi models are usually better than the other variants, so these days I don't even bother with the Rydel, Koren, Duncan or Bench, etc. SPICE models anymore, it just takes the guess-work out of the equation.

[MarkusBass]

None of the posted simulations work. LTSpice complains about missing symbols: 18W_OPT, OPT_PP_TAPS, potentiometer_standard. When you ask someone for help with your simulation, it would be nice to include all files not included in standard installation of LTSpice.

Mark

[überfuzz]

I'm not sure you get a "better" simulation just by swapping tube models. I tested different tube models a while back. My conclusion was that it's impossible to hear any significant difference between the models. Even if the models behave quite different, see attached png for clipping behaviour. In addition to this, a complex tube model is the heavier to calculate.

[hkc]

Jazbo8,
I visited Nakabayashi's site and found his treatise on modeling triodes and pentodes.
I don't know which is more daunting, the Japanese or the partial differential equations.
Probably the diffeq's since I can read Japanese given some time and a dictionary.
I saw some listings in his paper and also a bunch of parameter tables for different tubes but
I did not find the files in a spice readable form. Does a spice.lib file exist somewhere or is that
left as an exercise for the reader?

Thanks,
Hank

[überfuzz]

Jazbo8,
I visited Nakabayashi's site and found his treatise on modeling triodes and pentodes.
I don't know which is more daunting, the Japanese or the partial differential equations.
Probably the diffeq's since I can read Japanese given some time and a dictionary.
I saw some listings in his paper and also a bunch of parameter tables for different tubes but
I did not find the files in a spice readable form. Does a spice.lib file exist somewhere or is that
left as an exercise for the reader?

Thanks,
Hank

Like I wrote, don't get all exited about different tube models. You'll never see or hear the difference. ;-)

[hkc]

Everything has been posted. Please read the thread.

[hkc]

Found the Nakabayashi models on diyaudio.com.

Can't comment on whether or not one model sounds better than another but converging or not converging seems significant even if there isn't a perfect match to reality.

Hank

[überfuzz]

I'm pretty sure your calculation, i.e. simulation, won't diverge no matter what tube model you use. If your model won't converge, something else is wonky... Can you post your simulation.asc file here so that we can correct it.