My parallel stereo single ended triode is now ready :)

[Gabe001]

Kalee20, thank you. The 300pf is a new addition. I only did it in LT spice. The idea (in my head - could be wrong) is that it makes the gain block less effective at high frequencies by taking some of HF out of the local feedback loop, starting at 17k. Of course this could cause other issues.

Unfortunately Ltspice doesn't have an export all function, that I know of. I'll need to provide the lib and symbol files for the valves. Did you get the OPT up and running?

[Jez1234]

In hi fi amps I design I regard around 60KHz as a minimum figure for the -3dB point and often that would be due to an input 1st order filter. Full power bandwidth should be >50KHz ideally. I've designed mosfet amps which can give excellent square waves at full power and 100KHz... could be used as a MW transmitter no doubt

[G.Castle]

Originally Posted by kalee20

All the same, at the upper end I can't help feeling it should be better. I was really hoping to run the LTSpice sim and have a play, probing intermediate points - but without the valve models I can't do this, and I'm not sufficiently LTSpice fluent to find or create my own. (Plus, time's at a premium right now!)

Peter, possibly the op can confirm if he used self compiled .Inc models for the simulation, if I'm doing anything from scratch I have used Ayumi Nakabayashi INC files, they were originally assembled for TINA 7 but the attached are modified for LTSPICE

If Gabe could share what he used that would be a great help

[Jez1234]

I do wish there were more Ayumi Spice files for Multisim!

[HG MICKE]

Triode connected EL34 present a rather large input capacitance, including miller capacitance, it is in excess of 200pf for each Valve. This will, with the driving stage set up, give an early HF roll off.

Colin

[Gabe001]

I've got the ayumi valve set, alongside some others. I certainly didn't compile my own but I'll have a look and see which I've used. If it's easier I'll switch the models in my simulation to ayumi. Will post more this evening

[kalee20]

Originally Posted by HG MICKE

Triode connected EL34 present a rather large input capacitance, including miller capacitance, it is in excess of 200pf for each Valve. This will, with the driving stage set up, give an early HF roll off.

I estimated it at 98pF in Post #46, based on limited data in the data sheets... Post #48 put the HF roll-off at 61kHz therefore.

Your 200pF per valve is double this capacitance, so this would predict 30kHz, which is getting closer to Gabe's measured 20kHz.

(Where did you get the 200pF from, was this actual measurement on valves, capacitance and gain?)

[kalee20]

Originally Posted by HG MICKE

Triode connected EL34 present a rather large input capacitance, including miller capacitance, it is in excess of 200pf for each Valve. This will, with the driving stage set up, give an early HF roll off.

I estimated it at 98pF in Post #46, based on limited data in the data sheets... Post #48 put the HF roll-off at 61kHz therefore.

Your 200pF per valve is double this capacitance, so this would predict 30kHz, which is getting closer to Gabe's measured 20kHz.

(Where did you get the 200pF from, was this actual measurement on valves, capacitance and gain?)

[HG MICKE]

200+ pf is from Philips EL34 data, Grid 1 to all except anode 15.2pf. As G2 and Anode are now the same in Triode mode plus Grid 1 is is no longer shielded from the Anode. Gain in Triode mode is about 10.5.

Colin

[Gabe001]

here goes. I was using a mix of valves from different libraries. I've redone the circuits to use all "koren" valves

Everything in this zip file. I've never done this before so hopefully it works

The asy valve files go in \lib\sym\koren
The asy transformer file (ham1627se) go in \lib\sym\opt
All the lib files go in \lib\sub

You should be able to add these valves and transformer via the "add a new component" menu (f2). The symbols used for the valves are triode_new2 and xpentode4. Once they have been added select the spicemodels "ecc82" and "el34"

fingers crossed
Gabriel

[kalee20]

Originally Posted by HG MICKE

200+ pf is from Philips EL34 data, Grid 1 to all except anode 15.2pf. As G2 and Anode are now the same in Triode mode plus Grid 1 is is no longer shielded from the Anode. Gain in Triode mode is about 10.5.

Thanks!

Don't forget though, that a lot of the 15.2pF in 'Grid 1 to all except anode 15.2pF' will be Cgk, and that doesn't get multiplied-up by 11.5 (= 1 + your 10.5).

What we really need is Cg-k and Cg-(g2+a), however the anode is relatively remote and Cg-g2 is probably good enough. Unfortunately I don't have any EL34's so I can't measure them.

Although it's bringing us more in line with reality, I can't help thinking that 200pF per EL34 is a bit over-capacitive!

[GrimJosef]

Originally Posted by kalee20

... Don't forget though, that a lot of the 15.2pF in 'Grid 1 to all except anode 15.2pF' will be Cgk, and that doesn't get multiplied-up by 11.5 (= 1 + your 10.5) ...

In fact the situation is complicated by the fact that Gabe is taking the signal across the speaker and applying it to the EL34s' cathodes as negative feedback. I'm out of my depth here but does that generate a sort of 'inverse Miller effect' actually reducing the effective capacitance to the cathode that the previous stage has to drive ?

EDIT: I don't have access to a very precise capacitance meter I'm afraid, but for what it's worth I've just done some quick and dirty checks on three EL34s in the workshop - a modern JJ one, a modern Electro-Harmonix one and a perhaps 20 year old Svetlana one. Within the experimental error they all measured the same. I laid the valve on the bench and connected one meter lead to its g1 pin. I left the other lead disconnected but very close in physical position to where it would be if it were connected to the g2 pin. The meter read 18pF. I then connected the lead to the g2 pin and the reading increased to 26pF. Finally I connected the anode pin to the g2 pin and the reading increased again to 28pF. There was some background noise but it seemed that these readings were reproducible to better than +/-1pF. The measurements would imply that Cg1g2 is 8pF and Cg1(g2+a) is 10pF. These results are close to kalee20's estimates.

Cheers,

GJ

[G.Castle]

Had a few moments later on Wednesday evening so re did the sim for Gabes second .asc (the valves were missing in the schematic as the types weren't available in my library).

I used models of EL34 and 12AU7 that were available to me, the simulation stalled at 71% but at least shows promise!

I noted that the original files are now posted, if I can get both to work it may be an education as much in the differences between spice models as it shows the predicted performance of the amplifier!

Thanks again Gabe for humouring us!

[Gabe001]

The ayumi models didn't simulate for me. 70% is when the Sig gen starts producing the sine wave - the simulation stalls on my laptop as well. The Koren valve files will work no problem and the SIM runs to completion. The spice error log will give you THD but I found this only to be accurate at max signal. Everything else including voltages and FR are spot on

I played with a few simulations yesterday night. It seems about 2db loss of HF response is due to the gain block and 1 dB due to miller effect or the Hammond opt spice model used. See for yourselves. Now that Jez has set me a challenge I'm determined to get the FR as flat as possible😁 it will never run to 60k due to the parallel triode topology though

[Marconi_MPT4]

Models created by Ayumi Nakabayashi (2008) were originally intended for Spice and would need to be modified for use with LTSpice. Running the unmodified model usually throws an error, certainly for earlier versions of LTS. Change all instances of ^ to **.

For instance in Ayumi:
BM1 M1 0 V=(0.043621772*(URAMP(V(G2,K))+1e-10))^-0.51782633
for LTS:
BM1 M1 0 V=(0.043621772*(URAMP(V(G2,K))+1e-10))**-0.51782633

It is possible later revisions of LTS now accept ^, but still might be worth checking.

There are other caveats, but in the main this should give you a satisfactory simulation.

Rich

[G.Castle]

The Ayumi Nakabayashi models are a bit of a faff, though all the tweaks for those files I posted have been done, (that block were from DIY Audio Forum, it would have been a pain to reassemble what I had, and that's where they came from originally). I find that for me the Koren based sims are the least accurate, and the best done by a Canadian guy called Bob Weaver, I don't know his method but his effort is toward being faithful to published data: though like all nice things his output is rare with very few actual models, and not published as a collection.

I did try myself from scratch, but a carat, or an asterisk or space in the wrong place, and it's a total fail.

I'll have another little go at this as it's in my circle of interest, but may now have to wait until the longer evenings: that will not be long off now

What you have in hardware now, is not a great place to start from if the desire is HF performance: If you succeed in the improvement will you find yourself liking the sound?

[kalee20]

Originally Posted by GrimJosef

In fact the situation is complicated by the fact that Gabe is taking the signal across the speaker and applying it to the EL34s' cathodes as negative feedback

Wow - it is too, GJ, and all this time we've been rabbiting on about no NFB!

Originally Posted by GrimJosef

I'm out of my depth here but does that generate a sort of 'inverse Miller effect' actually reducing the effective capacitance to the cathode that the previous stage has to drive ?

It will, the Cgk is bootstrapped so plays a smaller part! And the stage gain is reduced so Miller multiplication of Cg(g2+a) is reduced.

These of course push the HF roll-off back up in frequency, good news for the amplifier design - but pushes it back farther away from Gabriel's actual measurements.

Originally Posted by GrimJosef

The measurements would imply that Cg1g2 is 8pF and Cg1(g2+a) is 10pF. These results are close to kalee20's estimates.

Thanks! An ounce of measurement is worth a pound of guesswork, though I'm glad the calibration of my guesstimator isn't far off!

[Gabe001]

Originally Posted by G.Castle

What you have in hardware now, is not a great place to start from if the desire is HF performance: If you succeed in the improvement will you find yourself liking the sound?

I don't think the -3db at 20k is noticeable by myself (and the majority of adults), but I'm sure I'll fix it. There is no reason to leave it as is; after all that effort it'll be a pity to have a parameter not measuring well even though the quality of the sound will likely not change significantly. I use digital music sources and oscilloscope tests indicate that a significant number of digital files are truncated at 15khz anyway (rather disappointingly, presumably to reduce the file size)

The simulations indicate there's a phase shift around the gain block (v1a) that is limiting the HF response, so I need to apply some compensation (I'm not sure if these are the correct terms,easier seen than explained). I've got a good idea on how to address this

You'll see for yourself once you get LT spice running with the valves up where the majority of HF loss is happening.

[Jez1234]

Originally Posted by Gabe001

The ayumi models didn't simulate for me. 70% is when the Sig gen starts producing the sine wave - the simulation stalls on my laptop as well. The Koren valve files will work no problem and the SIM runs to completion. The spice error log will give you THD but I found this only to be accurate at max signal. Everything else including voltages and FR are spot on

I played with a few simulations yesterday night. It seems about 2db loss of HF response is due to the gain block and 1 dB due to miller effect or the Hammond opt spice model used. See for yourselves. Now that Jez has set me a challenge I'm determined to get the FR as flat as possible😁 it will never run to 60k due to the parallel triode topology though

My figures were off the cuff one's I'd regard as a minimum for amps with NFB of 15dB as a minimum (too little can be a very bad thing and worse than none at all under some circumstances) and using power mosfets as the output devices. You ain't going to get a full power bandwidth of 50KHz+ with a zero NFB SET.... so no challenge Gabe

It's the output transformer primarily but also to some degree the lack of feedback that are the limitations here and not the valves... or at least it doesn't need to be the valves with the right topology. I've designed and built hybrid power amps which are valve everywhere except for the output mosfets and which have managed -3dB @ 1MHz at a few Watts and could do 20KHz full power square waves that looked pretty much the same as the input. It can be done... but not with an output transformer in the way!

I have a nearly ready prototype (after spending weeks on it "work work" got in the way so I ended up putting it all away with only a few hours work remaining... about 6 years ago!) again valved other than mosfet output stage, which should do certainly 100KHz or more full power bandwidth and THD <0.01% and is completely DC coupled from input to output. The PSU is probably more complex than the actual amp and has IIRC +/- 400V (so 800V total between + and -) and all rails are regulated including the heater supplies. I know it works (prob needs some debugging yet) as I did get as far as a messy lash up of one channel with a tiny heatsink which only allowed testing for a few minutes

[Gabe001]

Jez , I was joking about the challenge. Good luck with your projects. I am sure that with your knowledge and experience they will sound great.

So, here is an idea to address the HF loss. Attached please find the frequency response at the point probed which is the anode of the first section of the ecc82 (see first 2 pictures). You can see significant HF freq loss here (in green) which is where most of the issue is.

I am attaching a pic of my proposed modification (c14+r14) and the new FR at the same point (in red)

The final pic shows the new FR (blue) compared to the old (green) at the speaker, in LTspice of course, but so far this has been a good reflection of actual measurements. There is still going to be a very minor miller and opt effect at 20k to reduce the FR, but this is expected to be just under 1db. LT spice is putting the -3db point at around 35k

The final FR should work out 20-20k - 1db.

Does anyone see any issues with the proposed modification?