• 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 is a circuit where I quickly tested model from post 592.
Symbol model is tetrode model from Misc folder and LT spice.
 

Attachments

  • 6P9_pent.jpg
    6P9_pent.jpg
    62 KB · Views: 331
Ex-Moderator
Joined 2011
This is a circuit where I quickly tested model from post 592.
Symbol model is tetrode model from Misc folder and LT spice.
Thanks, I finally got the model to work but I am getting the same results as artosalo... Did you use the same curve data as shown in the picture below?

1. Ua = 102 V, Ug1 = 0 : Ia = 40 mA
2. Ua = 171 V, Ug1 = -3 : Ia = 38 mA
3. Ua = 242 V, Ug1 = -6 : Ia = 38 mA

So my results show too low anode currents.

6P9 Triode-Connected vs. the datasheet:
An externally hosted image should be here but it was not working when we last tested it.
 
Ex-Moderator
Joined 2011
Ayumi models always assign the pin numbers from the top to the botton of the tube, e.g., GU50PP A S G K. So just make sure whichever symbol that you use, assigns the pins in the same order. But this particular model was originally intended for TINA, so I don't think it would work in LTSpice at all... try this one instead:
Code:
*
* Generic pentode model: GU50_AN
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sat Jan 11 08:13:44 2014
*               Plate
*               | Screen Grid
*               | |  Control Grid
*               | |  |  Cathode
*               | |  |  |
.SUBCKT GU50_AN A G2 G1 K
BGG   GG   0 V=V(G1,K)+0.45288699
BM1   M1   0 V=(0.10715305*(URAMP(V(G2,K))+1e-10))^-1.1401545
BM2   M2   0 V=(0.56814856*(URAMP(V(GG)+URAMP(V(G2,K))/4.0302301)))^2.6401545
BP    P    0 V=0.0015719333*(URAMP(V(GG)+URAMP(V(G2,K))/7.0936201))^1.5
BIK   IK   0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.0011497682*V(M1)*V(M2)
BIG   IG   0 V=0.00078596663*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)*(0.916000233*(1-URAMP(V(A,K))/(URAMP(V(A,K))+10))^1.5+0.083999767)
BIK3  IK3  0 V=V(IK2)*(URAMP(V(A,K))+2101.25)/(URAMP(V(G2,K))+2101.25)
BIK4  IK4  0 V=V(IK3)-URAMP(V(IK3)-(0.0011298169*(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)-(0.0011298169*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  0.1p
CGK   G1  K  8.4p
C12   G1  G2 5.6p
CAK   A   K  9.2p
.ENDS
 
Last edited:
Ex-Moderator
Joined 2011
Hi everyone,
I'm trying to do a simulation of Bassman 5F6-A (1959) in PSpice. How can I simulate the output transformer? Use magnetic.lib from spice or create a new model? I don't know nothing about the core...

You can modify the values to suit the 5F6-A's OPT:

Code:
.SUBCKT PP_OUTPUT_XFRMR 1 2 3 4 5
* PUSH PULL OUTPUT XFRMR 
* 5000 OHM PRIMARY
* 8 OHM SECONDARY
* 100H TOTAL PRIMARY INDUCANCE
*
LP1	1	21	50	;Henries
RP1	21	2	70	;ohms
RP2	2	23	70	;ohms
LP2	23	3	50	;Henries
LS1	4	5	0.16	;Henries
CP1 1 3   2NF     ; CAPACITANCE 
KALL LP1 LP2 LS1 .9999875 
.ENDS
 
GU-50:

I am using next model:

.SUBCKT GU50 1 2 3 4 ; P G1 C G2 (Pentode) 21-Nov-2001
+ PARAMS: MU=8.5 EX=1.350 KG1=800 KP=15.9 KC=8000
+ KVB=30.3 VCT=0.00 RGI=1k
+ CCG=14P CPG1=0.4P CCP=9.2P
RE1 7 0 1G
RE2 8 3 1G
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 8 3 VALUE={(PWR(V(7),EX)+PWRS(V(7),EX))/KC*(2.5708-ATAN(V(1,3)/KVB))}
E2 8 4 VALUE={0}
RCP 1 3 1G ;
C1 2 3 {CCG} ;
C2 1 2 {CPG1} ;
C3 1 3 {CCP} ;
R1 2 5 {RGI} ;
D3 5 3 DX ;
.MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
.ENDS


and Tetrode-RY symbol