• WARNING: Tube/Valve amplifiers use potentially LETHAL HIGH VOLTAGES.
    Building, troubleshooting and testing of these amplifiers should only be
    performed by someone who is thoroughly familiar with
    the safety precautions around high voltages.

Vacuum Tube SPICE Models

This has been the subterfuge I used successfully in LTSpiceIV, I unfortunately have to report that this doesn't work in the 64 bit version of LTSpice XVII that I am now using. You can still edit the standard.mos file, but even after restarting LTSpice it ignores the entries. The values listed (variable names) are not correct for the new version either, I think they've changed the model used.

I recently installed the 64 bit version of LTSpice XVII. After copying the AN models into the *document* directory I see jack. Is it wiser to stick to the old IV version or does a primer exsist for freshmen like myself?
 
Best model sets at this time in history? (noob)

This LT Spice thread is so very long and I noticed that some posts recommended using models from one source over another. Without having to read all 400+ posts here...

Can someone provide some links as to what are the "best" models to download at this time in history?

I have a tube tracer with the capability to output an exact model for a single specifically measured tube, but I still need a collection of good models based on the published factors so I dont have to measure dozens of tubes to create models. I will use my tracer to generate models accurate to a specific physical tube if/when I want ultra-accuracy as a sanity test.

I have a lot to learn with LT but I wanted to get the current recommended models loaded at the outset.
 
I recently installed the 64 bit version of LTSpice XVII. After copying the AN models into the *document* directory I see jack. Is it wiser to stick to the old IV version or does a primer exsist for freshmen like myself?

You can put your models wherever you please, just tell it to LTspice: Tools -> Control Panel -> Sym. & Lib. Search Paths. Note the plural: more than 1 location is permitted.
 
Thanks you, Windcrest77. I have that zip file, but there is not the 100th spice model. I have tried also the following one:
Code:
* SPICE tube models for TINA simulator generated by Ayumi's method.
* 100TH*2SK79*4E27(Triode Strapped)*6H3/6N3*6H6/6N6
* 6H30/6N30*6J4P (Russian 6AC7)*6J4PT (Triode Strapped)
* C3g*C3g (Triode Strapped)*E92CC*6688 (E180F)*6688 (Triode Strapped)
* 805*814*814(Triode Strapped)*GU50(Russia)/FU50(China) Triode Strapped 
* GU50/FU50 
* **************************************
* Generic triode model: 100TH
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Fri Nov 26 13:06:10 2010
*             Plate
*             | Grid
*             | | Cathode
*             | | |
.SUBCKT 100TH A G K
.PARAM X1=-0.99906964 X2=0.0014094818 X3=-0.083738904
PARAM X4=0.94712581 X5=37.513209 X6=1.5837389
.PARAM X7=0.00034469629 X8=39.607419 X9=0.00027070609
.PARAM Y1=0.00017234814 Y2=0.00018548443
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))^X
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 2p
CGK G K 2.9p
CAK A K 0.3p
.ENDS
*
** Generic triode model: 2SK79
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sun Feb 28 23:48:12 2010
*               Plate
*               | Grid
*               | | Cathode
*               | | |
.SUBCKT 2SK79 A G K
.PARAM X1=0.10157886 X2=0.005502006 X3=-0.28096081
.PARAM X4=0.84224201 X5=28.672814 X6=1.7809608
.PARAM X7=0.019995035 X8=34.043439 X9=0.012489311
.PARAM Y1=0.0099975173 Y2=0.010884964
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 15p
CGK G K 16p
CAK A K 4p
.ENDS
I have added the missing dot (.PARAM) and also tried all the "X" values missing, from X1 to X9, but it does not work properly. Anyone that could have a working 100TH model ? (LTC)

Thanks again,
 
Try this:
Code:
.SUBCKT 100TH A G K
.PARAM X1=-0.99906964 X2=0.0014094818 X3=-0.083738904
.PARAM X4=0.94712581 X5=37.513209 X6=1.5837389
.PARAM X7=0.00034469629 X8=39.607419 X9=0.00027070609
.PARAM Y1=0.00017234814 Y2=0.00018548443
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 2p
CGK G K 2.9p
CAK A K 0.3p
.ENDS
 
Tina TI Pspice Model 5670 aka WE396A Ayumi

Newbie here at TinaTI Pspice and adding / simulating tubes. I've noticed a difference in the Ayumi models for LTSpice and TinaTI, however, I can't find the 'secret decoder' ring. I tried reading from Ayumi's site with GoogleTranslate, but still no luck. I'm pretty sure that somehow the parameters for Ayumi are run through an equation and the PARAMx PARAMy values pulled from these and then reinserted. The tube I'm interested in is the 5960 which is close to the WE396A. Jazbo8 provided an LTSpice model, which I tried to insert by changing the file from .inc to .cir, however, that didn't work. Probably a bad idea, but that's part of the learning process. Right below the post I noticed cogsncogs provided a post for a different valve in both LTSpice and TINA TIpspice, which when I tried the TINA version, it worked fine. When trying the LTSPice I get error message about operand ** line 15 or 16. Any help you can provide is appreciated. Thank you in advance.
 
Ex-Moderator
Joined 2011
TINA 5670 SPICE Model

Here you go:

Code:
*
* Generic triode model: 5670_AN
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Wed Nov 29 08:47:18 2017
*               Anode
*               | Grid
*               | | Cathode
*               | | |
.SUBCKT 5670_AN A G K
.PARAM X1=-0.044770209 X2=0.032175849 X3=-2.2476294
.PARAM X4=0.40025303 X5=18.639663 X6=3.7476294
.PARAM X7=0.0040093865 X8=46.569699 X9=0.0099503146
.PARAM Y1=0.0020046932 Y2=0.0021345255
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 1.1p
CGK G K 2.2p
CAK A K 0.1p
.ENDS
 
New generic Spicemodell copes secondary emission!

Hi all

One year after my introduction of new precise vacuum diode and triode spice models, I'm proud to present my new generic pentode model which is capable to mimic the secondary emission effect.
It has its roots in Derk Reefmans approach to describe this effect, but is highly improved to get the related parameters independently. :D

As a first tube, i fitted the 6L6GC based on the GE datasheet.
You will find the spice code here:
http://adrianimmler.simplesite.com/440956786

all the best, Adrian
 

Attachments

  • Bild1_6L6GC_Vg2=250V.png
    Bild1_6L6GC_Vg2=250V.png
    907.3 KB · Views: 375
  • Like
Reactions: 1 user