Wouldnt your voltage be 325v?
I thought this was peak voltage input, 230x1.414=325m RMS would be 230?
Yes.
Each voltage source amplitude is peek voltage.
"AC 230 0" is the small signal AC analysis voltage.
Attachments
Validate 6072 SPICE Model
I am trying to use 6072 SPICE model in my circuit. In order to make sure the model is correct, I try to validate the model by the following way.
This is the 6072 SPICE model downloaded from the DiyAudio(it is made by Ayumi Nakabayashi)
*
* Generic triode model: 6072
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sat Mar 8 22:42:09 2008
* Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 6072 A G K
BGG GG 0 V=V(G,K)+0.75743218
BM1 M1 0 V=(0.0057774859*(URAMP(V(A,K))+1e-10))^-0.42611934
BM2 M2 0 V=(0.77876794*(URAMP(V(GG)+URAMP(V(A,K))/38.292098)+1e-10))^1.9261193
BP P 0 V=0.00098547839*(URAMP(V(GG)+URAMP(V(A,K))/49.1701)+1e-10)^1.5
BIK IK 0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.00057643098*V(M1)*V(M2)
BIG IG 0 V=0.0004927392*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)-(0.00052295488*URAMP(V(A,K))^1.5)))+1e-10*V(A,K)
BIGK G K I=V(IG)
* CAPS
CGA G A 1.4p
CGK G K 1.4p
CAK A K 0.5p
.ENDS
I am trying to use 6072 SPICE model in my circuit. In order to make sure the model is correct, I try to validate the model by the following way.
This is the 6072 SPICE model downloaded from the DiyAudio(it is made by Ayumi Nakabayashi)
*
* Generic triode model: 6072
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sat Mar 8 22:42:09 2008
* Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 6072 A G K
BGG GG 0 V=V(G,K)+0.75743218
BM1 M1 0 V=(0.0057774859*(URAMP(V(A,K))+1e-10))^-0.42611934
BM2 M2 0 V=(0.77876794*(URAMP(V(GG)+URAMP(V(A,K))/38.292098)+1e-10))^1.9261193
BP P 0 V=0.00098547839*(URAMP(V(GG)+URAMP(V(A,K))/49.1701)+1e-10)^1.5
BIK IK 0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.00057643098*V(M1)*V(M2)
BIG IG 0 V=0.0004927392*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)-(0.00052295488*URAMP(V(A,K))^1.5)))+1e-10*V(A,K)
BIGK G K I=V(IG)
* CAPS
CGA G A 1.4p
CGK G K 1.4p
CAK A K 0.5p
.ENDS
Then I want to use a real circuit to test the model
I used the 6072 in a SRPP circuit
Then I run the simulation of the circuit in Multisim14, and get the voltage(relative to GND) of 4 point
V1=260V,V2=60.956V,V3=57.379V,V4=3.592V
I made a real circuit of it
and get the real voltage of these 4 point
V1=259.8V,V2=142.76V,V3=137.5V,V4=1.932V
the result is quite different from the simulation, especially V2 and V3, the real data is much higher then the simulation one
Is the model correct ?
I used the 6072 in a SRPP circuit
Then I run the simulation of the circuit in Multisim14, and get the voltage(relative to GND) of 4 point
V1=260V,V2=60.956V,V3=57.379V,V4=3.592V
I made a real circuit of it
and get the real voltage of these 4 point
V1=259.8V,V2=142.76V,V3=137.5V,V4=1.932V
the result is quite different from the simulation, especially V2 and V3, the real data is much higher then the simulation one
Is the model correct ?
It looks like you're not feeding any signal to the bottom triode's grid.
Also, you'll want to put a grid leak resistor from the bottom triode's grid to ground.
I've never tried to run an LTspice simulation with a circuit set up like that, so I don't know if what you're doing will run. Try the above and see if you can at least get it to run.
--
Also, you'll want to put a grid leak resistor from the bottom triode's grid to ground.
I've never tried to run an LTspice simulation with a circuit set up like that, so I don't know if what you're doing will run. Try the above and see if you can at least get it to run.
--
Besides, how do you know your tubes meet the specs, did you trace them?
No, I have no equipment to trace tubes. But this is a EH 6072 and I think it's specs should not quite different from GE 6072
It looks like you're not feeding any signal to the bottom triode's grid.
Also, you'll want to put a grid leak resistor from the bottom triode's grid to ground.
I've never tried to run an LTspice simulation with a circuit set up like that, so I don't know if what you're doing will run. Try the above and see if you can at least get it to run.
--
This circuit is part of M10, there is no leak resistor. The circuit can run in Multisim14, why can not run in LT-SPICE?
As rongon replied, you need a signal source and a grid leak resistor for the bottom triode; its grid is floating. Also in Ayumi's 6072 model, you need to change all instances of "^" with "**", minus the quotes.I try to silmulate this SRPP circuit in LT-SPICE
View attachment 641274
and it is the simulation sets
View attachment 641275
But it runs too slow after 10 min only finished 0.1%, is tere something wrong with the setting?
It may be that Multisim places a 1G resistor from all nodes to ground.This circuit is part of M10, there is no leak resistor. The circuit can run in Multisim14, why can not run in LT-SPICE?
Need help: Building 5687 SPICE Model
I have succeed made the 6072 SPICE model, and thanks for the kind-hearted guys helped me with it
and then I want to make 5687 model, because I want to simulate the M10 Preamp circuit. Now I am trying to building this preamp, then I want to use the model to simulate the whole circuit, it will be convinent to use it to adjust the real circuit.
But now I have some difficult with the model.
This is the model that I used Paint_Kit to trace the curve of TUNG-SOL 5687 document
I have succeed made the 6072 SPICE model, and thanks for the kind-hearted guys helped me with it
and then I want to make 5687 model, because I want to simulate the M10 Preamp circuit. Now I am trying to building this preamp, then I want to use the model to simulate the whole circuit, it will be convinent to use it to adjust the real circuit.
But now I have some difficult with the model.
This is the model that I used Paint_Kit to trace the curve of TUNG-SOL 5687 document
Code:
**** 5687_BIG ******************************************
* Created on 10/21/2017 19:38 using paint_kit.jar 3.0
* [url=http://www.dmitrynizh.com/tubeparams_image.htm]Model Paint Tools: Trace Tube Parameters over Plate Curves, Interactively[/url]
* Plate Curves image file: 5687-big.jpg
* Data source link:
*----------------------------------------------------------------------------------
.SUBCKT 5687 1 2 3 ; Plate Grid Cathode
+ PARAMS: CCG=3.1P CGP=4P CCP=0.45P RGI=2000
+ MU=18.7 KG1=424.1 KP=82.5 KVB=375 VCT=0 EX=1.29
* Vp_MAX=400 Ip_MAX=50 Vg_step=2 Vg_start=0 Vg_count=6
* Rp=4000 Vg_ac=55 P_max=40 Vg_qui=-48 Vp_qui=300
* X_MIN=50 Y_MIN=50 X_SIZE=1006 Y_SIZE=627 FSZ_X=1696 FSZ_Y=1026 XYGrid=false
* showLoadLine=n showIp=y isDHT=n isPP=n isAsymPP=n showDissipLimit=y
* showIg1=n gridLevel2=n isInputSnapped=n
* XYProjections=n harmonicPlot=n harmonics=y
*----------------------------------------------------------------------------------
E1 7 0 VALUE={V(1,3)/KP*LN(1+EXP(KP*(1/MU+(VCT+V(2,3))/SQRT(KVB+V(1,3)*V(1,3)))))}
RE1 7 0 1G ; TO AVOID FLOATING NODES
G1 1 3 VALUE={(PWR(V(7),EX)+PWRS(V(7),EX))/KG1}
RCP 1 3 1G ; TO AVOID FLOATING NODES
C1 2 3 {CCG} ; CATHODE-GRID
C2 2 1 {CGP} ; GRID=PLATE
C3 1 3 {CCP} ; CATHODE-PLATE
D3 5 3 DX ; POSITIVE GRID CURRENT
R1 2 5 {RGI} ; POSITIVE GRID CURRENT
.MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
.ENDS
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
- Home
- Amplifiers
- Tubes / Valves
- Audio Note M10 Clone