6EM7 dissimilar triode model

[AKSA]

Using a 6EM7 dissimilar triode model

I am experiences difficulty getting this model to work.
Any ideas?
Thanks in advance, HD

.SUBCKT 6EM7_P1 1 2 3 ; P G C

• PARAMS: MU=65.12 EX=1.14 KG1=554.18 KP=1228.6 KVB=4674.43
• RGI=2000
• CCG=2.2P CGP=4.8P CCP=.6P

E1 7 0 VALUE={V(1,3)/KP*LN(1+EXP(KP*(1/MU+V(2,3)/SQRT(KVB+V(1,3)*V(1,3)))))}
RE1 7 0 1G
G1 1 3 VALUE={(PWR(V(7),EX)+PWRS(V(7),EX))/(2*KG1)}
RCP 1 3 1G ; TO AVOID FLOATING NODES IN MU-FOLLOWER
C1 2 3 {CCG} ; CATHODE GRID
C2 2 1 {CGP} ; GRID-PLATE
C3 1 3 {CCP} ; CATHODE-PLATE
D3 5 3 DX ; FOR GRID CURRENT
R1 2 5 {RGI} ; FOR GRID CURRENT
.MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
.ENDS

.SUBCKT 6EM7_P2 1 2 3

• PARAMS: MU=7.288 EX=1.16 KG1=124.11 KP=25.418 KVB=1856.1
• RGI=2000
• CCG=7.0P CGP=10.0P CCP=1.8P

E1 7 0 VALUE={V(1,3)/KP*LN(1+EXP(KP*(1/MU+V(2,3)/SQRT(KVB+V(1,3)*V(1,3)))))}
RE1 7 0 1G
G1 1 3 VALUE={ (PWR(V(7),EX)+PWRS(V(7), EX))/(2*KG1) }
RCP 1 3 1G ; TO AVOID FLOATING NODES IN MU-FOLLOWER
C1 2 3 {CCG} ; CATHODE GRID
C2 2 1 {CGP} ; GRID-PLATE
C3 1 3 {CCP} ; CATHODE-PLATE
D3 5 3 DX ; FOR GRID CURRENT
R1 2 5 {RGI} ; FOR GRID CURRENT
.MODEL DX D(IS=1N RS=1 CJO=10PF TT=1N)
.ENDS

 

[Ray Waters]

SPICE files must be plain text; your subcircuits have bullets and these will cause the simulation to fail. These bullets should be replaced with the + sign.

Attached is a plain text file (6EM7.txt) that should work. It contains both the P1 and P2 models. Just include it in your .asc file and you should be good.

 

[AKSA]

Thank you Ray,
However, it does not yet work.......!
I will continue to futz with it until it works.
Hugh

 

[Ray Waters]

I tested both models and they work fine in a circuit that plots their characteristic curves. Are you getting errors or warnings, or does the circuit just not give the results that you are expecting?

If you upload your LTspice .asc simulation file maybe someone can help you get it to work.

 

[AKSA]

Thank you Ray,
attached.
Hugh

 

[Ray Waters]

Thanks for uploading the .asc file. The problems were easy to spot and easy to correct.

When you insert a symbol into a schematic LTspice will give it an instance label depending on the type of device. For example, the first resistor added to the schematic will get R1, the second resistor R2, etc. For devices defined by a subcircuit, the prefix is U. Tubes are defined by subcircuits so tubes will get instance labels of U1, U2, etc.

After a subcircuit device (like a tube) is applied to the schematic, the name of the subcircuit has to be assigned to the device. In your schematic, these are 6EM7_P1 and 6EM7_P2. The error in your schematic is that you replaced the instance label (U1, for example) with its subcircuit name (6EM7_P1 for U1), and you left both tube's default subcircuit names as "Triode." Since there is no defined subcircuit in your schematic named "Triode" the simulation will fail.

I've attached a revised .asc file that corrects these errors. I've also added a signal source so that you will see something meaningful at the "Output."

I hope this helps.

 

[AKSA]

Thank you very much Ray.
It works perfectly; I can then move onto my tube circuit which will be for a hybrid power amplifier.

Hugh

 

[Ray Waters]

Glad to help.