• 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.

Audio Note M10 Clone

Jump to Latest
#201
deafbykhorns said:
Wouldnt your voltage be 325v?
I thought this was peak voltage input, 230x1.414=325m RMS would be 230?
Click to expand...

Yes.
Each voltage source amplitude is peek voltage.
"AC 230 0" is the small signal AC analysis voltage.
 

Attachments

  • 270V PSU test2.jpg
    270V PSU test2.jpg
    64.9 KB · Views: 276
#203
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
 
#205
Then I used a software GetData Graph Digitizer to get sample points data
this is the Graph of GE-6072
3.JPG

this is the Graph of 6072 SPICE model
4.JPG

I choose 7 points on -2V line from each Graph for comparision
the plate voltage is around 100,120,140,160,180,200,220
to see the plate current
 
#209
Then I want to use a real circuit to test the model
I used the 6072 in a SRPP circuit
6.JPG

Then I run the simulation of the circuit in Multisim14, and get the voltage(relative to GND) of 4 point
10.JPG

7.JPG
V1=260V,V2=60.956V,V3=57.379V,V4=3.592V

I made a real circuit of it
9.jpg

and get the real voltage of these 4 point
8.jpg
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 ?
 
#211
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.
--
 
#214
rongon said:
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.
--
Click to expand...



This circuit is part of M10, there is no leak resistor. The circuit can run in Multisim14, why can not run in LT-SPICE?
 
#215
jerrylong said:
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?
Click to expand...
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.
 
#218
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
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
 
#219
This is the circuit of M10
M10.gif

and this is the voltage that I tested on my real circuit
5687并管在路静态电压.jpg
All the voltage is reference to the GND

and this is the simulation results that I have run in LT-SPICE
15.JPG

the voltage(refrence to GND) of cathode of 5687 is much lower than real one, why?
 
You must log in or register to reply here.
Top Bottom