PSpice/LTSpice model for 6AU6/EF94?

[Robert McLean]

Ryan
The nodes are as given in the model first line
ie
.SUBCKT 6AU6 A S G K

so A anode or plate, S screen grid, G control grid (or just grid ), k cathode

So for example lets say I have R1 100K resistor to plate and 250 volts, R4 to screen and 250 volts, R2 1K resistor from cathode to ground and R3 270K from grid to ground

and lets say the 250 volt supply is node 101, my tube grid is node 104, cathode is 105, screen is 103, anode is 102 ( they can be any number you like, I am not sure how much Spice to assume you know )

then this section of Spice would be

XU1 N102 N103 N104 N105 6AU6
R1 N101 N102 100K
R2 N105 0 1K
R3 N104 0 270K
R4 N101 N103 1Meg
V1 N101 0 250

etc

just pass the line calling the tube subcircuit the node numbers of the tube elements in the order given in the subcircuit first line : A, S, G, K.

 

[Robert McLean]

a couple of things to point out, you may already know this :
So far as modeling is concerned, just ignore pin 2 on the 6AU6. It is the suppressor grid, and the subcircuit model assumes it is already connected to the cathode.

Also, if it is the vibrato circuit that you are modeling, be aware that the cathode resistor on V2 is shared by several other tubes in other parts of the preamp. So you need to either include those other tubes in your model, at least the dc part, or , add in about 1 mA of current to the V2 cathode resistor with a current source.
Otherwise you will not get the 1.7 volts indicated at V2 cathode.