# import new component into LT Spice with .cir file

my desperate attempt to simulate a circuit led me here.

I have a low noise amplifier which has a HEMT as its transistor. (ATF38143). I have been trying to create a component in LT Spice and came across this website. The page linked here is a .cir file for ATF34143 and it was the closest HEMT I could find.

I copied and pasted the script in a text editor and saved it in the .cir format. Then, I opened it with LT Spice, highlighted the name of the HEMT in the first line of the .cir file to create a new component.

Unfortunately, when I attempt to simulate the circuit, it results in an error. I have tried the same simulation without the user defined HEMT and the result of the simulation appeared reasonable.

I have also tried the .cir file of a different transistor from the same website (linked here) and went through the exact same steps to create a component corresponding to the .cir file. It worked smoothly.

Could someone take a look at the content of the cir file for the ATF34143 transistor shown on the website and point out what's wrong with it? Given that I was able to create a new component with a different .cir file, I am certain what's in the .cir file for ATF34143 is wrong.

Shown below is what the website says the .cir file should have. (It's a bit unclear which parts should be in the .cir file given that there are two instances of ".SUBCKT" and ".ENDS")

I edited the model into something LTspice understands. The model had a few issues with the SPICE syntax (LTspice is pretty strict about using Spice3 derived syntax).

Here is a updated model, and a discussion of the changes and compromises will follow:

*ATF-34143 packaged FET model
.SUBCKT ATF34143  16   14   15
RR2 2   1   0.1
RR9 4   3   0.1
RR5 1   5   0.1
LL2 5   SOURCE  0.1nH
LL7 SOURCE  7   0.1nH
LL6 SOURCE  8   0.1nH
RR6 8   2   0.1
RR7 7   2   0.1
RR8 DRAIN   9   0.1
LL5 9   11  0.1nH
LL8 2   15  0.05nH
LL10    15  1   0.1nH
LL1 14  4   0.8nH
LL9 11  16  0.6nH
CC3 11  2   0.15e-12
CC4 1   4   0.15e-12
LL4 3   GATE    0.1nH
*CALL DIE MODEL
XDIE DRAIN GATE SOURCE  ATF34
.ENDS
****     GaAs MESFET MODEL PARAMETERS
.SUBCKT ATF34   D   G   S
CC1 D S 0.04pF
RR1 G GATE 1
Z34 D GATE S BATF34143
.ENDS
.MODEL BATF34143 nmf ( LEVEL=2, Vto=-0.95, Beta=0.24,
+                     Lambda=0.09, Alpha=4, B=0.8, Pb=0.7,
+                     Cgs=0.8pF, Cgd=0.16pF, Rd=0.25,
+                     Rs=0.125, Is=1nA)


I had to remove the spaces between the values and units in the model, which accounted for a lot of the ignored parameters right off the bat.

And LTSpice does have a GASFET model, but it is named nmf (for n channel MESFET). Changing the model to the correct type for LTSpice further reduces the ignored parameters.

Most of the those parameters are secondary parameters (and thus are included in a model for convenience, but can be modeled just as well using a netlist around the model) which I accounted for in the ATF34 subcircuit. Specifically, ohmic gate resistance and fixed drain to source capacitance.

The Tnom parameter is simply the nominal temperature, which is a global parameter in LTSpice and already defaults to 27 anyway, so that isn't needed.

Delta is the power law for triode region operation and isn't accounted for by LTSpice's nmf MESFET model, so we will have to do without. But if your application is a LNA, then I would assume you'd only care about the saturation region, in which case this doesn't really matter for your application anyway and shouldn't influence your simulation meaningfully.

Vbi is just a different term for the gate bias voltage, which is referred to by Pb in LTSpice, so I changed it to the correct parameter name. That leaves just one unrecognized parameter, P.

This is the drain noise coefficient, and is not part of the model. The Statz model includes the flicker noise coefficient, and LTSpice's model DOES support that parameter, so I added it (Kf).

It should work reasonably well but the noise might not be modeling drain noise noise correctly, and of course triode region voltage to current power law behavior.

• Now I see I omitted the MESFET. My point was that you could use it as something else, but then the results should not be the ones expected. +1, and shame on me. Aug 14 '21 at 16:29