Continue to Site

Welcome to our site!

Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

  • Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

741 Bandpass filter

Status
Not open for further replies.

ryukyu

New Member
I am attempting to build a bandpass filter using the 741 (I have also tried the LM324) and I am having some difficulties. When using the 324 I get no bandpass response at all, more like a linear high-pass through 120 kHz.

I am looking for a center frequency of 33kHz, and have used this calculator to get me in the ballpark:

Active Filter Calculator - Bandpass with OpAmp Designer in Javascript

I am using typical E12 resistor values for R1 and R2, which I know will skew my center frequency and BW a bit, and a variable 1k pot for R3

**broken link removed**

The values I've used are as follows:
fc= 33000 Hz
BW=1500 Hz
A=10
C=1 nF

And theses are the initial results
Q=20
R1=10610 Ω
R2=212207 Ω
R3=111 Ω

I then used the second tool and used these standard values

R1=10k
R2=220k
R3=100Ω

which yielded,

fc=34101.2 Hz
BW=1447 Hz
Q=23.5

When I use these resistors (within the best tolerance possible) my peak output occurs at 20kHz. The caps I am using are 102J polyester film. I have access to drawers full of electrolytics but the lowest I've seen is .47uF which yields resistor values that are all under 100Ω and 1 being 0Ω using the calculator.

Am I trying to get too much out of this amp?
Too much Q?
Unreliable capacitor size?
I don't want to pay more for shipping than the cost of replacing the caps with 10nF caps unless this is the likely culprit.

I would prefer to use an amp that is quad with gnd to V+ instead of rail to rail as there are size constraints on the project.

I would be grateful for any suggestions or help.
 
The component values are correct. The 741 and 324 op amps do not have enough gain-bandwidth for your desired frequency, gain, and Q. According to my simulations the op amp needs a gain-bandwidth of about 100MHz to give the desired response and those are not common.

You might try LTSpice (free) to simulate your filter. It will save you a lot of breadboard time.
 
I appreciate the response. I have simulated this is PSpice (OrCad) using a 741 and it provides the desired frequency response, which is why I ran with it.

I was under the impression that the gain-bandwidth product was cutoff*bw which
I had 10*1500=15k.

If the GBW of the 741 is 1MHz at G=1 then isn't it 100kHz when gain =10 which should allow for the parameters given?

I can reduce the gain of the filter, as I do have 2nd and 3rd stage inverting amps to pick up the slack.

I am looking to boost 1mV-pp at 33kHz to 3Vpp when it's all said and done. I need to do this without any bleedover from a 44kHz signal.

My configuration is the filter shown into two cascaded inverting amplifiers. Being that they are just being used for amplification, and not filtering, I assume they are not limited by the GBW...
 
A lousy old 741 opamp has slew-rate limiting beginning at only 9kHz. Then its output becomes a triangle-wave and higher frequencies cause its max level to be reduced.
The 741 opamp is also much too noisy to amplify a signal that is only 1mV.

1mV to 3V is a voltage gain of 3000. If two 741 opamps are cascaded and each has a voltage gain of 54.8 then their output drops above only about 10kHz.

Why don't you try a low noise TL072 dual opamp that has a full output to 100kHz? At a gain of 54.8 its output drops above 60kHz. Its cost is almost as low as one 741 opamp.
 
And you are running split power supplies on the opamps, right?
 
I appreciate the response. I have simulated this is PSpice (OrCad) using a 741 and it provides the desired frequency response, which is why I ran with it.
You should recheck your simulation, particularly the 741 model.

I did the simulation in Electronic Workbench (also a Spice simulator) and I got a peak frequency of 23kHz, close to what you measured (see below).

Filter Response.jpg
 
Last edited:
Here is another view:
 

Attachments

  • BP.png
    BP.png
    34.1 KB · Views: 501
  • BPF.png
    BPF.png
    32.4 KB · Views: 766
Last edited:
audioguru,

I have been looking for alternatives. The first I found was a LM359, but a lot of sellers that have lower minimums/handling fees don't carry this. It looks like the TL072 will work. Radio Shack (I cringe to think of going in there and being asked if I need batteries) carries the TL082 which appears to be a slightly inferior chip to the 82 but it is immediately available. (I have a proof of concept deadline.)
 
And you are running split power supplies on the opamps, right?

On the breadboard I have been. We have a size constraint to deal with so I was toying with the idea of using a 9V with a virtual ground at 4.5V once I actually get a nice peak at the center frequency we really want. I'd really hate to add a second 9V if we don't have to.
 
You should recheck your simulation, particularly the 741 model.

I did the simulation in Electronic Workbench (also a Spice simulator) and I got a peak frequency of 23kHz, close to what you measured (see below).

View attachment 47118

I think the OrCad model for a UA741 is slightly idealistic. I decided to consult a few forums for advice rather than trying to troubleshoot the parameters of the model.

I do appreciate you taking the time to run a simulation in EW. I think I need to get that back on my system. I miss having the ability to "Run" a circuit and toggle switches.
 
Did you notice the excellent bandpass curve posted by MikeMl when the opamp is "ideal"? The lousy old 741 opamp is completely different.
 
Did you notice the excellent bandpass curve posted by MikeMl when the opamp is "ideal"? The lousy old 741 opamp is completely different.

Here is the LTSpice repeated with a 741 model. Note the reduction in gain, and the shift of the resonant peak...
 

Attachments

  • BPFni.png
    BPFni.png
    47.3 KB · Views: 478
I don't believe that a 741 opamp performs so well. But I haven't used one for such a long time (about 30 years) that I forget that they still have a few uses today.
 
I have attempted to rebuild this filter using an LM6132 amp. I went to National searching for an op amp for this filter and they had a an interactive tool called Webench that regurgitated an output for me including a simulation result and component values. The circuit is, as expected, the same as that in the original post, but they are showing VCC and VEE on the opamp. I took this to mean +5/-5 on the rails, but the the datasheet (this was discovered after the fact) says V+=5 and V-=0. This doesn't make sense to me for a rail to rail I/O. I haven't got back to the lab to see what changing the input voltages accordingly will do, but when hooked up as described with VCC=5 and VEE=-5 the circuit oscillates with no input at all. When attempting to get bandpass results the output is uniform from 1 Hz to 1MHz, ie the input has no effect on the output.

I'm guessing that changing VEE to gnd will have a rather large effect though, as it will bring the positive input "down" to the rail voltage. My closing question: is load (greater than the impedance of an oscope) required for proper operation?
 
I have attempted to rebuild this filter using an LM6132 amp. I went to National searching for an op amp for this filter and they had a an interactive tool called Webench that regurgitated an output for me including a simulation result and component values. The circuit is, as expected, the same as that in the original post, but they are showing VCC and VEE on the opamp. I took this to mean +5/-5 on the rails, but the the datasheet (this was discovered after the fact) says V+=5 and V-=0.
The (+) input of an opamp is its DC reference voltage. Your first posted circuit has the (+) input at ground so it needs a plus and minus power supply. If the (+) input is biased at half the supply voltage then any opamp will work with just a positive supply.

If your first circuit has just a positive supply then its (+) input is at 0V. The inputs of ordinary opamps do not work when they are within 2V or more from the negative supply. The output of the opamp might be as low as it can go. But its output cannot go negative when the circuit's input goes negative.

When the (+) input is biased at half the supply voltage then the output idles at half the supply voltage so the output can swing equally up and down with the AC input signal.

the circuit oscillates with no input at all. When attempting to get bandpass results the output is uniform from 1 Hz to 1MHz, ie the input has no effect on the output.
Then either you made it on a breadboard where the stray capacitance and stray coupling messes it up, or you connected it wrong.

Is load (greater than the impedance of an oscope) required for proper operation?
An opamp works the same with or without a load if the load is within its output current capacity. But many high speed opamps oscillate when directly driving a shielded cable because the cable has capacitance. Adding a 100 ohm resistor in series with the output of the circuit allows the opamp circuit to drive a shielded cable. A 'scope probe has a shielded cable.
 
Status
Not open for further replies.

Latest threads

New Articles From Microcontroller Tips

Back
Top