I tried your .asc and got it to work with the Ayumi models I use. It does work OK. I got 0.1% THD also. Yours also has a bit of a dip in the response centered on 1kHz, but less so than in my simulation. I'm not sure which one is more accurate. Maybe yours is. I'm not a spice expert at all.
I'll have to play with this some more. You're getting a LOT of gain out of that 6AU6. Much more than I would have expected.
--
I don't think that's actually the case, it appears to me that all of the poles and zeros required are realized in the EQ network connected to the plate of the 6AU6. In any event the deviation from the ideal RIAA response should show up in the simulations if there is a dependence on cartridge inductance for EQ.
Your points about loading and a better tube like the 6N6 IMO are spot on. The Russian 6J9P might be a better choice for the pentode, quiet, and very cheap.
Yes , this is a concern, even if the Ayumi models are very good, who knows if the real thing behaves the same.. replacing the led with a resistor make a lot of difference, for the worse. A 6DJ8 in place of the AU7: awful
Last edited:
The pentode part has less conductance and the triode has a low µ.
Plus the fact that the triode anode is side by side with the pentode control grid makes it not very suitable for this circuit.
Mona
I don't have a model for 6J49P. Is there a western equivalent to that tube? Perhaps the 6J9P is similar, but I'm not sure. So here's the 6J9P pentode model I use.
Code:
**** 6J9P_4 ******************************************
* Created on 11/25/2013 00:58 using paint_kit.jar 2.6
* Model Paint Tools: Trace Tube Parameters over Plate Curves, Interactively
* Plate Curves image file: 6j9p_4.jpg
* Data source link:
*----------------------------------------------------------------------------------
.SUBCKT 6J9P 1 4 2 3 ; P K G2 G1
+ PARAMS: CCG=8.5P CGP=0.03P CCP=3P RGI=2000
+ MU=55.9 KG1=280.9 KP=369.1 KVB=23.1 EX=1.49 KG2=400
* Vp_MAX=480 Ip_MAX=40 Vg_step=0.5 Vg_start=-0.5 Vg_count=5
* Rp=1600 Vg_ac=23.5 P_max=7.5 Vg_qui=-23.4 Vp_qui=240 UL=0.469 EG2=139.2
* X_MIN=73 Y_MIN=50 X_SIZE=365 Y_SIZE=256 FSZ_X=1032 FSZ_Y=742 XYGrid=false
* showLoadLine=n showIp=y isDHT=n isPP=n isAsymPP=n isUL=n showDissipLimit=n
* showIg1=y gridLevel2=n isInputSnapped=n
* XYProjections=n harmonicPlot=y harmonics=y
*----------------------------------------------------------------------------------
RE1 7 0 1MEG ; DUMMY SO NODE 7 HAS 2 CONNECTIONS
E1 7 0 VALUE= ; E1 BREAKS UP LONG EQUATION FOR G1.
+{V(4,3)/KP*LOG(1+EXP((1/MU+V(2,3)/V(4,3))*KP))}
G1 1 3 VALUE={(PWR(V(7),EX)+PWRS(V(7),EX))/KG1*ATAN(V(1,3)/KVB)}
G2 4 3 VALUE={(EXP(EX*(LOG((V(4,3)/MU)+V(2,3)))))/KG2}
RCP 1 3 1G ; FOR CONVERGENCE
C1 2 3 {CCG} ; CATHODE-GRID 1
C2 1 2 {CGP} ; GRID 1-PLATE
C3 1 3 {CCP} ; CATHODE-PLATE
R1 2 5 {RGI} ; FOR GRID CURRENT
D3 5 3 DX ; FOR GRID CURRENT
.MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
.ENDSI don't have a favorite 6N6P model, but here's an Ayumi method model.
Code:
*
* Generic triode model: 6N6_AN
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Fri Sep 27 17:21:24 2013
* Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 6N6_AN A G K
.PARAM X1=-0.12412617 X2=0.017099117 X3=-0.49413473
.PARAM X4=0.75220594 X5=14.491629 X6=1.9941347
.PARAM X7=0.0034675681 X8=19.265507 X9=0.0020032288
.PARAM Y1=0.001733784 Y2=0.0020072404
BK IK 0 V=U(V(G,K)+X1)*X7*URAMP(V(G,K)+X1+URAMP(V(A,K))/X8)**1.5+(1-U(V(G,K)+X1))*X9*(X2*URAMP(V(A,K)))**X3*(X4*URAMP(V(G,K)+X1+URAMP(V(A,K))/X5))**X6
BA A K I=URAMP((Y2*URAMP(V(A,K))**1.5)-URAMP((Y2*URAMP(V(A,K))**1.5)-V(IK)+Y1*URAMP(V(G,K))**1.5*(URAMP(V(G,K))/(URAMP(V(A,K))+URAMP(V(G,K)))*1.2+.4)))+1E-10*V(A,K)
BG G K I=Y1*URAMP(V(G,K))**1.5*(URAMP(V(G,K))/(URAMP(V(A,K))+URAMP(V(G,K)))*1.2+.4)
* CAPS
CGA G A 3.5p
CGK G K 4.4p
CAK A K 1.8p
.ENDSHere's the Ayumi 6AU6 pentode model.
Code:
*
* Generic pentode model: 6AU6
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sat Mar 8 22:39:10 2008
* Plate
* | Screen Grid
* | | Control Grid
* | | | Cathode
* | | | |
.SUBCKT 6AU6_AN A G2 G1 K
BGG GG 0 V=V(G1,K)+0.24107953
BM1 M1 0 V=(0.014176045*(URAMP(V(G2,K))+1e-10))**-0.93570358
BM2 M2 0 V=(0.61583848*(URAMP(V(GG)+URAMP(V(G2,K))/27.099343)))**2.4357036
BP P 0 V=0.0032162308*(URAMP(V(GG)+URAMP(V(G2,K))/44.003978))**1.5
BIK IK 0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.0020681021*V(M1)*V(M2)
BIG IG 0 V=0.0016081154*URAMP(V(G1,K))**1.5*(URAMP(V(G1,K))/(URAMP(V(A,K))+URAMP(V(G1,K)))*1.2+0.4)
BIK2 IK2 0 V=V(IK,IG)*(1-0.4*(EXP(-URAMP(V(A,K))/URAMP(V(G2,K))*15)-EXP(-15)))
BIG2T IG2T 0 V=V(IK2)*(0.71681629*(1-URAMP(V(A,K))/(URAMP(V(A,K))+10))**1.5+0.28318371)
BIK3 IK3 0 V=V(IK2)*(URAMP(V(A,K))+15750)/(URAMP(V(G2,K))+15750)
BIK4 IK4 0 V=V(IK3)-URAMP(V(IK3)-(0.0017183702*(URAMP(V(A,K))+URAMP(URAMP(V(G2,K))-URAMP(V(A,K))))**1.5))
BIP IP 0 V=URAMP(V(IK4,IG2T)-URAMP(V(IK4,IG2T)-(0.0017183702*URAMP(V(A,K))**1.5)))
BIAK A K I=V(IP)+1e-10*V(A,K)
BIG2 G2 K I=URAMP(V(IK4,IP))
BIGK G1 K I=V(IG)
* CAPS
CGA G1 A 0.0035p
CGK G1 K 3.3p
C12 G1 G2 2.2p
CAK A K 5p
.ENDSAnd finally, here's the Ayumi N. 12AU7 model.
Code:
*
* Generic triode model: 12AU7_AN
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sat Mar 8 22:41:08 2008
* Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 12AU7_AN A G K
BGG GG 0 V=V(G,K)+0.89005722
BM1 M1 0 V=(0.028826571*(URAMP(V(A,K))+1e-10))**-0.90897681
BM2 M2 0 V=(0.622671*(URAMP(V(GG)+URAMP(V(A,K))/13.089625)+1e-10))**2.4089768
BP P 0 V=0.00087237591*(URAMP(V(GG)+URAMP(V(A,K))/21.021735)+1e-10)**1.5
BIK IK 0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.00055330711*V(M1)*V(M2)
BIG IG 0 V=0.00043618795*URAMP(V(G,K))**1.5*(URAMP(V(G,K))/(URAMP(V(A,K))+URAMP(V(G,K)))*1.2+0.4)
BIAK A K I=URAMP(V(IK,IG)-URAMP(V(IK,IG)-(0.00049917061*URAMP(V(A,K))**1.5)))+1e-10*V(A,K)
BIGK G K I=V(IG)
* CAPS
CGA G A 1.5p
CGK G K 1.6p
CAK A K 0.4p
.ENDSThanks, I do use Ayumi N. models whenever I can, but for some reason these russian tubes were not in my files.
What about PSRR of these circuits?
I simulate a couple of simple 3-tube "passive" designs adding 2 to 5 mV AC 50Hz in the DC Supply rail (5mV in 300VDC is really good) and this 2 to 5mV "ripple" appears in the output (5mV in 400mV is really BAD). (almost 0dB of PSRR).
BTW: The "Bokarev" really works, at least on LTSpice. But compared with other designs it is a DC current hog, making worst the power supply issue. The 6N6p is a excellent buffer, very low Rp, but draws a lot of filament current (better DC regulation, thick wires, etc).
Any suggestions?
I simulate a couple of simple 3-tube "passive" designs adding 2 to 5 mV AC 50Hz in the DC Supply rail (5mV in 300VDC is really good) and this 2 to 5mV "ripple" appears in the output (5mV in 400mV is really BAD). (almost 0dB of PSRR).
BTW: The "Bokarev" really works, at least on LTSpice. But compared with other designs it is a DC current hog, making worst the power supply issue. The 6N6p is a excellent buffer, very low Rp, but draws a lot of filament current (better DC regulation, thick wires, etc).
Any suggestions?
jdrouin if we haven't lost you....
I reported earlier that my friend found his Tubecad Tetra a little cold blooded. I borrowed it and found that right away it sounded really wrong. So wrong that I suspected the RIAA eq was off. I did some probing and there was a wrong resistor value in both channels.
After I corrected this it sounded quite nice. Very low noise and hum with a separate chassis for the PS-1 and Tetra Sans PS boards. My friends version uses ECC88s for the input and 12AT7s for the output tube. The gain was a little low with the ECC88s but even cranking up the volume a little more the noise was low. It sounded good being fed with an Ortofon 2M Red.
Good luck on your build, Steve
I reported earlier that my friend found his Tubecad Tetra a little cold blooded. I borrowed it and found that right away it sounded really wrong. So wrong that I suspected the RIAA eq was off. I did some probing and there was a wrong resistor value in both channels.
After I corrected this it sounded quite nice. Very low noise and hum with a separate chassis for the PS-1 and Tetra Sans PS boards. My friends version uses ECC88s for the input and 12AT7s for the output tube. The gain was a little low with the ECC88s but even cranking up the volume a little more the noise was low. It sounded good being fed with an Ortofon 2M Red.
Good luck on your build, Steve
We unexpectedly moved house recently, so I haven't been able to participate in the forum much and just wanted to say thanks again for all of your input. In studying Morgan Jones and Sound Practices I've come to see the linkages among Jeremy Epstein and a number of you other guys here posting schematics, measurements, and thoughts. Pretty cool when it all comes together like this.
I have a Mac, on which LTSpice won't work without a Windows virtual machine, so I've been trying to teach myself to use Eagle. Once I've finished learning more about circuit calculation and analysis, and taking into account what you all have posted here, I'll make an informed decision on a phono pre project I hope next month.
You guys are fantastic.
I have a Mac, on which LTSpice won't work without a Windows virtual machine, so I've been trying to teach myself to use Eagle. Once I've finished learning more about circuit calculation and analysis, and taking into account what you all have posted here, I'll make an informed decision on a phono pre project I hope next month.
You guys are fantastic.
Distortion predictions in LTSpice (or any Spice) should be taken with a grain of salt. The predictions are no better than the quality of the model used permits. I generally find that in the real world measured distortion is 10 - 15dB worse than predicted using models made from real tubes I have on hand. Some of the canned models on the web produce much better results in simulation than they do in the real world. It pays to do a reality check.
I find Spice much more trustworthy for things like predicting gain and frequency response, and very poor on noise predictions and poor on distortion. (It is good for predicting trends in most respects however.)
If you have OS X 10.7 or above, you don't need Windows VM. There is a download for OS X 10.7+ for LTspice IV. I just downloaded the current LTspice.dmg.
Indeed.
Yes, but looking for trends only, what if you have a circuit, let's say it uses a 6AU6 into a 12AU7 as mosquito's does, and let's say spice says it'll get 0.1% THD at 1V rms output. I take that figure of 0.1% THD with a large grain of salt. Perhaps it's really more like 0.3% THD in real life.
Let's say I want to try a different pentode in the first stage to compare performance. Let's also say the models are equally good or bad as compared to each other.
Let's say I use a 6J9P in the first stage instead of the 6AU6. I adjust my circuit to be optimized for 6J9P, and spice says it will yield 0.05% THD at 1V RMS out. Again, I understand that real life performance will be much worse than this, but my goal is not to say the distortion will be exactly this or that. I'm looking to compare the two pentodes.
So the question is, in simulation, if the 6J9P shows half the distortion at 1V RMS out compared to 6AU6, do you think that's a reasonably trustworthy estimation that I'd get lower distortion from a 6J9P than from a 6AU6 in real life?
That may indeed be the case, but probably depends a lot on the relative quality of the models used.
(Yes I know that sounds wishy washy..)
I think I understand what you mean. Thanks to you and others who have generously shared your knowledge and experience, I've learned a ton by participating in this forum. So first, thanks for being so patient with us non-engineers.
One thing I've learned is that there ain't no free lunch, and just about everything is a compromise. If you gain something, you just about always lose something else. Very rarely does one find a win-win solution to a set of problems.
Spice modeling allows me to spit out virtual prototypes one after the other, and compare them in minutes. That's a big gain for my understanding. The thing lost is that spice simulations don't predict real life performance very well. Like you wrote earlier, one has to take the results of these simulations with a grain of salt.
I've seen people jump into threads, leaping to conclusions based on their simulations that don't stand up in real life. Heck, I've done it. That too was a learning experience.
So back to the unbelievably good 6AU6 > 12AU7 results... I've found some unbelievably good looking operating points that are probably the result of distortion cancellation nulls in simulation. What I do is keep a library of alternative models to use (i.e., I have at least two models of each active device, tube, MOSFET, JFET, etc.). If something looks too good to be true, I'll swap 'devices' to see if the results hold up. They rarely do. Too good to be true usually is just that.
--
Rongon, excellent strategy (last paragraph). I have multitudes of models for this reason for a few types of tubes I use in places where this is a concern.
When I first started using spice I was somewhat surprised with the lack of correlation to the real world in terms of operating points, distortion, and of course noise. The pleasant surprise is that gain and frequency response measurements have proven to be quite close. Better models helps with distortion simulations and gives you some sense of what to expect..
For me the problem is often compounded as I use transformers for coupling in some of my designs, and of course the transformers are simplistic linear models that work well in the frequency domain and for predicting gain, but usually result in unusually good distortion measurements since I have not bothered to figure out how to model core nonlinearity. There other ways to model transformers besides the coupled inductor model commonly used so that might provide some possibilities.
Spice is great for testing scenarios and finding the ones likely to give the best results, but I still run into situations (rarely) where a circuit in the real world works well and in simulation I have trouble getting it to work.
When I first started using spice I was somewhat surprised with the lack of correlation to the real world in terms of operating points, distortion, and of course noise. The pleasant surprise is that gain and frequency response measurements have proven to be quite close. Better models helps with distortion simulations and gives you some sense of what to expect..
For me the problem is often compounded as I use transformers for coupling in some of my designs, and of course the transformers are simplistic linear models that work well in the frequency domain and for predicting gain, but usually result in unusually good distortion measurements since I have not bothered to figure out how to model core nonlinearity. There other ways to model transformers besides the coupled inductor model commonly used so that might provide some possibilities.
Spice is great for testing scenarios and finding the ones likely to give the best results, but I still run into situations (rarely) where a circuit in the real world works well and in simulation I have trouble getting it to work.
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.