# Filter Simulation don't work

Hi, I want to simulate a Butterworth filter 3rd order. I use the same values like in LTSpice, but the results are totally different in dB.
Here are the LTSpice netlist:
V1 N001 0 AC 2 Rser=50
L1 N002 N001 26.5n
L2 0 N003 298p
L3 N004 N003 26.5n
C1 N003 N002 0.238p
C2 0 N003 21.2p
C3 N004 N005 0.238p
R1 N005 0 50
.ac oct 1001 1G 3G
'* Butterworth Filter 3rd Order f_0 2Ghz BandWith 300Mhz (15%) ← this is comment
.backanno
.end
And here the QSpice netlist:
V1 N01 0 AC 2
L1 N05 N04 26.5n
L2 0 N03 298p
L3 N03 N02 26.5n
C1 N04 N03 0.238p
C2 0 N03 21.2p
C3 OUT N02 0.238p
R1 OUT 0 50
R2 N01 N05 50
.ac oct 1001 1G 3G
.plot V(OUT)
.end

Sorry! I can’t upload images as a new user.

What is different to LTSpice? I like the new design of QSpice and I also want to learn how to use it. Maybe someone can help me.
Many thanks! Juergen

Please verify if setting Rpar of Inductor to 0 can resolve your problem. LTspice and Qspice define default parasitic differently. Inductor in LTspice in default with 1mohm series resistance (Rser) and in Qspice in default with parallel resistance (Rpar) = Inductance/15.91/Gmin
Unfortunately, your circuit is sensitive to parallel resistance and that cause the difference. Force Rpar=0 by add this as attribute and see if this is the result you are looking for.
There are different ways to force Rpar=0. Beside of individually add this, you can set .option LFT to infinite value (set LFT=1e308 or 0 can force this value to very large number).
You can goto Qspice HELP for more information. Or, you can goto L. Inductor section in my device guideline which can be found in this location
Qspice/Guideline at main · KSKelvin-Github/Qspice · GitHub

ButterworthFilter_18333.qsch (6.2 KB)

Many thanks for your explanation. The PDF’s on GitHub are very helpful. They are a good resource to start with QSpice and spice simulation in general.