Analog Design Center Tools Calculators Ltspice Simulator

Simulating LPF with Gain using LTspice XVII January 25, 2020

Posted by haryoktav in Interest.
trackback

I wrote this post to extend my memories ^^

LTspiceXVII was downloaded from https://www.analog.com/en/design-center/design-tools-and-calculators/ltspice-simulator.html

The LPF has a cut-off frequency of 40Hz with a gain of 50. LT1014 was selected since it is similar to LM324. The input signal to this circuit has a bandwidth of 0 – 40 Hz and an amplitudo of around 10 mV.

Fig 1. LT1014 from Linear Technology

With the formula of f-cut-off = 1/( 2*pi*R3*C1), the C1 was chosen to be 47uF. This gives the R3 to about 82 ohm. These values slightly move the cut-off frequency to 41.3 Hz.

The LPF was constructed with a non-inverting amplifier with the gain = 1 + (R2/R1). Since I want to analyze the output with a varying of R2, the R1 was set to 10k, and the R2 was stepped from 100k to 500k.

So, put the components.. connect them with the wires.. add some label nets.. and here comes the schematic: Don't forget to set the value of the R2 with {R}, use the curly brackets. The reason is that the R2's value will be varied for each analysis.

Fig 2. Low pass filter with gain

Now, preparing for the Transient analysis. Transient analysis gives time domain waveforms which are plots of voltage or current versus time.

Set the value of V1 and V2 to 5 Volt.
Set the input signal V3. By right-clicking the V3, a form titled Independent Voltage Source – V3 will appear as shown in Fig 3. Choose the functions of the V3 as SINE with the DC offset of 0, the amplitudo of 10m (milivolt), and the frequency of 50 Hz. Also for AC analysis, set the AC Amplitude with 1 and the AC Phase with 0. After the OK button was clicked, the text of "SINE(0 10m 50)" and "AC 1 0" will be printed near the V3 symbol as shown in Fig 2.
Simulate –> Edit Simulation Command. Select Transient tab, set the stop time to 0.1 (second) as shown in Fig 4.
Edit –> SPICE Directive. Write ".step param R 10k 560k 100k" in the text box. This means the value of R2, which is {R}, will be varied from 10k to 560k with a step of 100k, as shown in Fig 5.

Fig 3. Input signal V3

Fig 4. Transient analysis

Fig 5. The .op command

Simulate –> Run. Window –> Tile Vertically. Move the mouse's cursor to the schematic and "probe" the voltage VS and Vin. As shown in Fig 6, the input signal of 10 mV was attenuated to about 6.3 mV. Now, "probe" the VOUT, and Fig. 7 will appear.

Fig 6. VS vs Vin

Fig 7. VOUT with varied value of R2

To see the peak of the Vout, move the mouse's cursor and click the text "V(vout)", the measurement cursor will appear. But when one tries to move the measurement cursor to the left or to the right, it seems that the measurement cursor was stick on a particular trace. By pressing the up-down arrow of the keyboard, the measurement cursor will stick to the other trace.

Now, for the AC analysis. AC analysis gives the voltage or current versus frequency in a linearized version of the circuit.

In Fig 2, right-click the text ".tran 0.1" or select Simulation –> Edit Simulation Command. Choose the AC Analysis tab. Type of sweep is Decade, Number of points per decade is 10, Start frequency is 0.1, and Stop frequency is 1Meg. Click OK. Notice that, in the schematic, the text ".tran 0.1" will be changed to ".ac dec 10 0.1 1Meg".
Select Simulate –> Run. Move the mouse's cursor and "probe" the VOUT, Fig 9 will show up. In Fig 9, there is a phase information along with the frequency responses. The phase information can be turn off by right-click the Right Vertical Axis with the degree scale, then click "Don't plot phase" button.

Fig 8. AC Analysis

Fig 9. Frequency responses

As shown in Fig 10, it was observed that the cut-off frequency was around 41.209752Hz (I modified the Number of points per decade from 10 to 1000 to get a bit detail step).