Look at the line that starts the definition of the subcircuit.
?
?
.SUBCKT 06HPR33 1 2 3
You will notice that the subcircuit has 3 external nodes (1 2 3). The native inductor has only two external nodes. You cannot use the inductor symbol and assign this subcircuit to it because of the node mismatch. If you look in the Files section of this group,
?
Files > Tut > S-Parameter > S-Parameter to SPICE
you will find a symbol file for a 2-port device (S2PORT.asy). Your s-parameter file is a 2-port file as designated by the extension .s2p. You will notice that the 2-port symbol has three external nodes. Two of them connect to the nodes in your circuit where you would connect the inductor. The third node is ground.
?
?
________________________________
From: ayman_hendawy <ayman_hendawy@...>
To: LTspice@...
Sent: Wednesday, July 10, 2013 6:50 AM
Subject: [LTspice] import Touchstone file (s2p) to LTSpice
?
Hi,
I have ".s2p" files of some inductors and I need to import this file as a model to the inductors I have drawn in LTSpice in order to use it in the simulation, in order to do a practical simulation.
I downloaded the "s2spice_097.exe" from the "group files" and generate the .lib file, I get a file like this:
/***/
.SUBCKT 06HPR33 1 2 3
* MHz S MA R 50
* Z1=50.000000 Z2=50.000000
R1N 1 10 -5.000000e+001
R1P 10 11 1.000000e+002
R2N 2 20 -5.000000e+001
R2P 20 21 1.000000e+002
*S11 FREQ MAG PHASE
E11 11 12 FREQ {V(10,3)}= MAG
+( 1.000000e+006, 4.400000e-002, 2.585500e+001)
+( 1.047000e+006, 4.400000e-002, 2.681900e+001)
+( 1.097000e+006, 4.500000e-002, 2.780500e+001)
.
.
.
/**/
Then I added to my inductor in the spicemodel field: 06HPR33 , and add in the spice directive the following: .lib "the path to my .lib file".
But when I run the simulation I get nothing for the inductor, so kindly advice what I'm doing wrong.
Thanks
