RC Low-Pass Filter Circuit based on LTSpice file Lpfilter1.cir

RC Low-Pass Filter Spice file Lpfilter1.cir

CAD III SIMULATION – STEP BY STEP

Original elr audio amp schematic

elr audio amp mod suggestion from Alan Yates

ELR mods LTSpice .asc files

LTspice Tutorial sites

RC Low-Pass Filter

CIRCUIT

                                 LPFILTER1.CIR              Download the SPICE file

Here’s a simple circuit for you to dive into running SPICE simulations and plotting results.

What is the purpose of this circuit? Basically it has two roles: to pass the desired low frequency signals and stop the unwanted high frequency signals.

TIME RESPONSE

Open the netlist file “lpfilter1.cir” with your SPICE simulator. Most simulators display the netlist in a text editor window. You can view, modify and save the netlist from this window.

Run a simulation. (TopSpice users click the traffic light on the toolbar; PSPICE users click the blue square.) View the transient (time) analysis at the input V(1) and output V(2). For R1=1k, C1=0.032uF and sinewave generator at 2kHz, you should see the 2 kHz sinewave (desired signal) pass through to the output V(2) except for a slight decrease in signal and slight shift in time.

Now change the sinewave frequency to 40 kHz by editing the voltage source line to look like

     VS   1      0      AC     1    SIN(0  1 40KHZ)

Save the file and run another simulation. Assume this 40 kHz signal represents the undesirable noise in a system. Did the filter reduce the 40 kHz signal?

CUTOFF FREQUENCY

As stated above, the circuit has two roles: to pass the desired low frequency signals and stop the unwanted high frequency signals. But at what frequency does the filter change its behavior from passing the low ones to stopping the high ones. This is called the cut-off frequency.

For R1=1k and C1=0.032uF you get fc = 5kHz. Run a simulation. Plot the AC (frequency) sweep results for the output magnitude VM(2) and phase VP(2). What does the magnitude look like before and after 5kHz?

SPICE FILE

Download the file or copy this netlist into a text file with the *.cir extention.

LPFILTER1.CIR - SIMPLE RC LOW-PASS FILTER
*
VS	1	0	AC	1	SIN(0	1	2KHZ)
*
R1	1	2	1K
C1	2	0	0.032UF
*
* ANALYSIS
.AC 	DEC 	5 10 10MEG
.TRAN 	5US  500US
* VIEW RESULTS
.PRINT	AC 	VM(2) VP(2)
.PLOT	AC	VM(2) VP(2)
.PRINT	TRAN 	V(1) V(2)
.PLOT	TRAN 	V(1) V(2)
.PROBE
.END

SwitcherCAD III SIMULATION – STEP BY STEP

SwitcherCAD III from Linear Technology is the only free version with no component limit. You can download a free demo version (See Demos and Downloads). Here’s how to run a simulation for the SPICE file named LPFILTER1.CIR, plot various results and modify the circuit.  

DOWNLOADING THE CIRCUIT FILE.

1. From the Circuit Collection page on this site, click on a circuit such as  RC Low-Pass Filter. You’ll see a schematic along with circuit and simulation notes that you can print out.

2. Download the SPICE file LPFILTER1.CIR by clicking on download the SPICE file on the web page.

RUNNING A SIMULATION. 

1. Start the SwictherCAD III program.

2. To open a SPICE circuit file select Open > File. Drop down the Files of Type box and select Files of Type (*.cir) to make the *.cir files visible. Move to folder where you saved your SPICE circuit (LPFILTER.CIR), click on the filename, then click on Open. Your SPICE circuit file will appear in a text editor window.

3. Select Simulate > Run or click the simulation icon (running man) on the top toolbar.

 NOTE   You can specify an .AC or .TRAN Analysis in the netlist but not both simulatenously. If both exist in your netlist, just place a "*" before one of the statements to tell SPICE to ignore the line.

PLOTTING VOLTAGES AND CURRENTS.

1. SwitcherCAD III automatically opens a window for you to select which waveforms to plot. The PRINT statement tells SPICE which waveforms to make available. Excluding the PRINT statement makes all of the voltages and currents available for selection.

2. To add waveforms select Plot Settings > Add Traces. Click on one or more of the voltages or currents available and then click OK.

 MODIFYING YOUR CIRCUIT.

1. In the text editor’s window, modify component values or change analysis commands in your SPICE circuit file.

2. Save the file by selecting File > Save or can click the simulation icon (running man) to save and run a new simulation.