creating new component with cir files

Thread Starter

Seongwoo Oh 1

Joined Aug 26, 2018
2
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.

I have also attached my asc file contaning the circuit I was trying to test.
 

Attachments

Alec_t

Joined Sep 17, 2013
11,650
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?
Here's the model :-
*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 BATF34143
.ENDS
**** GaAs MESFET MODEL PARAMETERS
.SUBCKT ATF34 D G S
.MODEL BATF34143 GASFET ( LEVEL=2, Vto=-0.95, Beta=0.24, Lambda=0.09, Alpha=4,
+ B=0.8, Tnom=27, Vbi=0.7, Delta=0.2, Cgs=0.8 pF,
+ Cgd=0.16 pF, Rd=0.25, Rg=1, Rs=0.125, Cds=0.04 pF,
+ Is=1 nA, P=0.65)
.ENDS


The ATF34143 model calls the BATF34143 GASFET model. Unfortunately LTspice doesn't recognise the GASFET type and its listed parameters.
 

eetech00

Joined Jun 8, 2013
1,992
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.

I have also attached my asc file contaning the circuit I was trying to test.
Hi

Try model attached.
Be sure to change mesfet symbol "prefix" attribute from Z to X (if it isn't already X).

eT

1583008054119.png
 

Attachments

Top