LTspice simulation of SAW Filter (*.s2p)

Thread Starter

Kevil

Joined Jun 28, 2020
127
I am trying to simulate the Infineon GPS SAW Filter B2618. I have converted the S-Parameters *.s2p file by s2spice.exe B2618_WB.s2p Z1 Z2 to *.lib file and imported it into LTspice with autogenerated symbol.

When I run the AC simulation I got error:
u1:r2p: Resistance must not be zero

What I am doing wrong?

B2618_WB.png
 

Attachments

eetech00

Joined Jun 8, 2013
3,110
I am trying to simulate the Infineon GPS SAW Filter B2618. I have converted the S-Parameters *.s2p file by s2spice.exe B2618_WB.s2p Z1 Z2 to *.lib file and imported it into LTspice with autogenerated symbol.

When I run the AC simulation I got error:
u1:r2p: Resistance must not be zero

What I am doing wrong?

View attachment 258868
The model definition file is missing some resistance values:

R1N 1 10 0.000000e+000
R1P 10 11 0.000000e+000
R2N 2 20 0.000000e+000
R2P 20 21 0.000000e+000

these are resistors with 0 (zero) values

There is also a pin mismatch in the .subckt definition. The .subckt specifies 3 pins but the definition only has two.

The subckt model is not defined correctly.
 

Papabravo

Joined Feb 24, 2006
18,125
As far as the simulation is concerned you have a bit of work to do. I can auto generate the symbol but the results look ugly regardless of the orientation. I tried adding 50Ω of source impedance to V1, but it was no help; the response still looks really ugly.

1643315202119.png

Are you sure about the implementation. It almost seems like you might be missing something.
 
Last edited:

Papabravo

Joined Feb 24, 2006
18,125
That's more like it. A little bit of sweat equity pays off.
If you post the .asy file for the symbol I can clean it up and make it more intuitive for you. Maybe label the pins "IN", "OUT" and "GND"
 

Thread Starter

Kevil

Joined Jun 28, 2020
127
Perfect, I am not familiar with the .asy file editor. Maybe you can write "IN" "OUT" "GND" and e.g. "SAW Filter" as description. See attached example and my current .asy
 

Attachments

Papabravo

Joined Feb 24, 2006
18,125
OK, Here is the result. I made new files, with "_PB" tacked on the end of the name, so you can compare them in both LTspice and in a text editor. I made the rectangular outline slightly wider so that the boundary will be on a grid line. The labels inside the rectangle use ordinary text so that I can use a smaller font. The actual pin labels have been changed to "In", "Out", and "Gnd" but they have been rendered invisible because they only have one font size. I changed the <Value> field from NAME to "B2618_WB" since that is the handle the spice engine uses to find a subcircuit in a library. I added the name of the library in the ModelFile field. This all works as long as the schematic (.asc file), and the symbol (.asy file) and the library are all in the same folder. At some point if you want them more generally available in your system we can talk about how to do that.

1643376360287.png

Here is the result on my system

1643376577754.png
 

Attachments

Top