Second Order Low Pass Filter Proteus Simulation
Here's your schematic drawn up in LTspice:

(I've used \$U_4\$ instead of \$U_3\$ and I've added some resistors at the (+) inputs of each opamp.)
The transfer function is:
$$\begin{align*}
\frac{V_\text{OUT}}{V_\text{IN}}=\mathcal{H}\left(s\right)&amp;=K\frac{\omega_{_0}^{\,2}}{s^2+2\zeta\,\omega_{_0}s+\omega_{_0}^{\,2}}\\\\
&amp;\text{where,}\\\\
A_{v}&amp;=\frac{R_5}{R_4}\\\\
K&amp;=\frac1{A_v}\frac{R_6}{R_2}\\\\
\omega_{_0}&amp;=\frac1{\sqrt{\frac1{A_v} R_3 R_6 C_1 C_2}}\\\\
\zeta &amp;= \frac1{2\sqrt{A_v}}\cdot \sqrt{\frac{C_2}{C_1}}\cdot \frac{\sqrt{R_3 R_6}}{R_1}
\end{align*}$$
If you set \$R_3=R_6=R\$ and \$R_4=R_5\$ and \$C_1=C_2=C\$, then this nicely reduces to:
$$\begin{align*}
K&amp;=\frac{R}{R_2}\\\\
\omega_{_0}&amp;=\frac1{R \cdot C}\\\\
\zeta &amp;= \frac1{2}\cdot \frac{R}{R_1}
\end{align*}$$
Given that you select a convenient value for \$C\$, you then simply select a value for \$R\$ in order to set a desired \$\omega_{_0}\$. Once that's done, you use \$R_2\$ to set the overall voltage gain and you set \$R_1\$ to set the damping factor. It's really simple!! Which is the cool thing about this particular schematic. (Also known as a state-variable filter.)
Bearing in mind that the gain-bandwidth of the LM348 is \$1\:\text{MHz}\$, here's a Bode plot from the above, using LTspice:

We expect about a low-pass band voltage gain of \$20\log_{10}\left(\frac{15\:\text{k}\Omega}{1.5\:\text{k}\Omega}\right)=20\:\text{dB}\$. Which the above shows.
If I run a transient analysis (.TRAN) then I get the following with an input of \$2\:\text{kHz}\$ with a peak-to-peak voltage of \$1\:\text{V}\$:

Which looks about as you'd expect, since \$K=10\$.
Now, from the Bode plot I expect that at \$f=100\:\text{kHz}\$ that \$k\approx \frac1{10}\$. So let's plot that out using a transient plot:

Almost exactly as expected, yes?
Frankly? I'm not having any troubles at all. I suspect that you may have not connected up the (+) and (-) rails, properly. That's the place I'd be looking, right now. I simply do not have problems with the circuit. It works just as analysis would suggest.
I can't tell you specifically what is wrong because I don't use your Spice tool and I really don't know what you did wrong. But it's clear that when I attempt to replicate your issues using a different tool, LTspice, then I find exactly what I do expect to see.
Hopefully, someone familiar with your tool will be able to find your error. I apologize that I cannot do more than I have.