To create your own spice model, the first step is the determination of MU from a reliable diagram. Diagram must include Ug=0V curve.
I took Telefunken pentode and triode diagrams just for example.
The formula for calculation is:
MU=(Ua-Ua min) / Ug
For pentode, the line passes through operating point and the END of knee @ Ug = 0V, as you can see.
I took Telefunken pentode and triode diagrams just for example.
The formula for calculation is:
MU=(Ua-Ua min) / Ug
For pentode, the line passes through operating point and the END of knee @ Ug = 0V, as you can see.
Attachments
Thanks Raj,
This will allow us to determine mu for the model and then work solely with the other parameters - should make curve fitting a lot easier.
I built a prototype of my new phono stage (the muscovite mini) using a 6Z9P-E pentode in the front end and was gratified at how close the measured performance was compared with the spice model predictions. It even sounds good.. lol (The model is a slightly modified version of the one you gave me, kg2 adjusted to reflect real world screen currents.)
This will allow us to determine mu for the model and then work solely with the other parameters - should make curve fitting a lot easier.
I built a prototype of my new phono stage (the muscovite mini) using a 6Z9P-E pentode in the front end and was gratified at how close the measured performance was compared with the spice model predictions. It even sounds good.. lol (The model is a slightly modified version of the one you gave me, kg2 adjusted to reflect real world screen currents.)
I saw, nice.
I know a few DIYers who use E180F in RIAA preamp.
One of them has E180F in pentode mode as input, and E180F triode mode on output (LED bias, CCS mu-out). He is very happy with sound. I adapted the Russian Teflon capacitors for his RIAA RC network. Simply unwrapped AL/Teflon foils to the required value. See atach.
Attachments
well , I'm dumb .... but that's hardly anything new .....
what I'm doing wrong ?
current from PSU to tube is 8A , but I'm still puzzled where is it going
Kad tvoj atas proslijedim u LTspice, sve je korektno. Radna tacka: 395V/99,4mA/-11,93V,
Tako da trenutno ne bih znao.
translation:
When your atach I put in LTspice everything works correctly.
So currently I do not know ....
I know , main problem is still - short circuit between headphones of operator
especially in "younger" time
well , I'm dumb .... but that's hardly anything new .....
what I'm doing wrong ?
current from PSU to tube is 8A , but I'm still puzzled where is it going
Replace ^ with ** to convert syntax to LTspice model
Different I/V curves for different brands of same tube type?
I tried the Joel’ pspice models, and noted that his library refers the tube brand datasheet, for every tube type, so I tried to see how different could be the I/V curves for some different brands of the same tube type.
Surprisingly, I came across with differences in Vp as great as 10% for the same Ip and Vg !
Have a look at the attached graphs, of the 12AT7 from BRIMAR, GE and MAZDA (Phillips).
I tried the Joel’ pspice models, and noted that his library refers the tube brand datasheet, for every tube type, so I tried to see how different could be the I/V curves for some different brands of the same tube type.
Surprisingly, I came across with differences in Vp as great as 10% for the same Ip and Vg !
Have a look at the attached graphs, of the 12AT7 from BRIMAR, GE and MAZDA (Phillips).
Attachments
Freshly made, just out of the oven
Code:
*
* Generic pentode model: 12J1L_AN
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Wed Dec 11 14:54:51 2013
* Plate
* | Screen Grid
* | | Control Grid
* | | | Cathode
* | | | |
.SUBCKT 12J1L_AN A G2 G1 K
BGG GG 0 V=V(G1,K)+0.98709898
BM1 M1 0 V=(0.037076469*(LIMIT(V(G2,K),0,1e16)+1e-10))**-1.4371722
BM2 M2 0 V=(0.51069528*(LIMIT(V(GG)+LIMIT(V(G2,K),0,1e16)/13.197177,0,1e16)))**2.9371722
BP P 0 V=0.0011571547*(LIMIT(V(GG)+LIMIT(V(G2,K),0,1e16)/25.841588,0,1e16))**1.5
BIK IK 0 V=IF(V(GG)>0,1,0)*V(P)+(1-IF(V(GG)>0,1,0))*0.0010881412*V(M1)*V(M2)
BIG IG 0 V=0.00057857734*LIMIT(V(G1,K),0,1e16)**1.5*(LIMIT(V(G1,K),0,1e16)/(LIMIT(V(A,K),0,1e16)+LIMIT(V(G1,K),0,1e16))*1.2+0.4)
BIK2 IK2 0 V=V(IK,IG)*(1-0.4*(EXP(-LIMIT(V(A,K),0,1e16)/LIMIT(V(G2,K),0,1e16)*15)-EXP(-15)))
BIG2T IG2T 0 V=V(IK2)*(0.84036243*(1-LIMIT(V(A,K),0,1e16)/(LIMIT(V(A,K),0,1e16)+10))**1.5+0.15963757)
BIK3 IK3 0 V=V(IK2)*(LIMIT(V(A,K),0,1e16)+5550)/(LIMIT(V(G2,K),0,1e16)+5550)
BIK4 IK4 0 V=V(IK3)-LIMIT(V(IK3)-(0.00064639118*(LIMIT(V(A,K),0,1e16)+LIMIT(V(G2,K),0,1e16)-LIMIT(V(A,K),0,1e16))**1.5),0,1e16)
BIP IP 0 V=LIMIT(V(IK4,IG2T)-LIMIT(V(IK4,IG2T)-(0.00064639118*LIMIT(V(A,K),0,1e16)**1.5),0,1e16),0,1e16)
BIAK A K I=V(IP)+1e-10*V(A,K)
BIG2 G2 K I=LIMIT(V(IK4,IP),0,1e16)
BIGK G1 K I=V(IG)
* CAPS
CGA G1 A 0.007p
CGK G1 K 2.4p
C12 G1 G2 1.6p
CAK A K 3.7p
.ENDSInstalling Tube Libraries In LTSpice
OK so you want to install a collection of tube models and their supporting symbols. Note both are provided with no warranty implied or otherwise.
There are two directories you need to locate. LTspice is a 32 bit program and will be installed in program files in xp or Program Files (X86) in Win 7. Locate the LTC folder..
Path to tube symbols is \LTC\LTspiceIV\lib\sym - unzip the tube_sym zip and paste the folder here.
Next step:
Path to tube library is \LTC\LTspiceIV\lib\sub - unzip the tube_lib zip file and paste the file here.
Start LTspice and under the component folder (AND gate on the menu) you will see a folder called 'Tubes' click on this and you will find diode, triode, tetrode, and pentode folders. Click on the folder of your choice and you will get a number of choices. I have lots of triode models and fewer pentodes, tetrodes and diodes. A few models may be funky, but most work ok.
OK so you want to install a collection of tube models and their supporting symbols. Note both are provided with no warranty implied or otherwise.
There are two directories you need to locate. LTspice is a 32 bit program and will be installed in program files in xp or Program Files (X86) in Win 7. Locate the LTC folder..
Path to tube symbols is \LTC\LTspiceIV\lib\sym - unzip the tube_sym zip and paste the folder here.
Next step:
Path to tube library is \LTC\LTspiceIV\lib\sub - unzip the tube_lib zip file and paste the file here.
Start LTspice and under the component folder (AND gate on the menu) you will see a folder called 'Tubes' click on this and you will find diode, triode, tetrode, and pentode folders. Click on the folder of your choice and you will get a number of choices. I have lots of triode models and fewer pentodes, tetrodes and diodes. A few models may be funky, but most work ok.
Attachments
On linux, it is just to decompress the archive, go into the directory where the inc files are, and run:
Code:
for i in *.inc; do sed -i -e 's:\^:**:' $i; done
