4
\$\begingroup\$

I have a distorted signal, and only want to allow frequencies between 95kHz and 105kHz. The input voltage is at 300mV peak to peak.

Thus, I need a Pass Band of 10kHz and a Central Frequency at 100kHz.

I was reading through various analogue electronics books to find out some commonly used variations and topologies and decided to go for the Multiple feedback filter.

I will be using this circuitry:

enter image description here

According to this document:

This circuit is widely used in low Q (< 20) applications. It allows some tuning of the resonant frequency, F 0 , by making R2 variable. Q can be adjusted (with R5) as well, but this also change s F 0 .

I then proceeded by follwoing the equations on that same document, or else on the book, Op Amp Applications Handbook.

My calculations and working is listed below:

First, we must determine the centre frequency, bandwidth, and Q.

enter image description here

The Q is too high to use separate high- and low-pass filters, but sufficiently low so that a multiple feedback type may be used.

enter image description here

Before actually building this circuit I want to be able to simulate it. Here is my circuit implemented on Proteus software.

enter image description here

And this is the respective frequency response:

enter image description here

It may not be clearly visible, I apologize, but the center frequency is only at 63kHz.

enter image description here

LM324 datasheet.

enter image description here

At 100kHz the max output voltage swing is only 1V peak to peak, and thus I am keeping my gain levels, low. (AV = 2)

I followed the instructions, but clearly I am doing something wrong.

How can I get an actual center frequency of 100kHz, and what am I doing wrong?

Any tips and/or suggestions would be appreciated.

\$\endgroup\$
  • \$\begingroup\$ Always good to check DC bias voltages before looking at the AC response. Can you indicate the bias voltages returned from the simulation? Also, what magnitude of input signal are you using? \$\endgroup\$ – scorpdaddy Oct 29 '18 at 17:11
  • \$\begingroup\$ Isn't the LM324 a single supply opamp? At any rate, welcome to the real world, where opamp's input impedance influences your design choices. Try a JFET input opamp, see what you get. Forgot to say, also check the bandwidth, some may not be able to reach that far. \$\endgroup\$ – a concerned citizen Oct 29 '18 at 17:14
  • \$\begingroup\$ @scorpdaddy, input signal is at 150mV amplitude, will add bias voltages. Also, LM324 can be used in single rail or dual rail configuration, as per the data sheet Iwill add to the question. Regarding the bandwidth, it should also be in the limits of what I am trying to achieve. That is in fact why I am keeping the gain (AV) low at 2. Since at 100kHz the output swing is only 1V p-p. \$\endgroup\$ – Rrz0 Oct 29 '18 at 17:24
  • 1
    \$\begingroup\$ Try using an op-amp with high GainBandwidthProduct (GBW). LM324 has gain of about ten at 100kHz. Not really enough. \$\endgroup\$ – glen_geek Oct 29 '18 at 17:29
  • 2
    \$\begingroup\$ Recommendation: Use an IDEAL opamp and check if the parts values are OK. According to my calculation the design mid frequency using your parts is 70.8 kHz. More than that, for hardware realization use another opamp \$\endgroup\$ – LvW Oct 29 '18 at 18:06
3
\$\begingroup\$

Your using the wrong simulator or the wrong opamp. Check the opamp bandwidth and make sure its sufficient (in the simulator, not just on a datasheet). I got 100kHz three ways in LT spice:

enter image description here

The first circuit is using a 1 pole ideal opamp (no loss, no railing, and nearly infinite bandwidth)

The second uses an ideal opamp, but has parasitics (the caps have ESR and I added a small amount of inductance to simulate real world inductance)

The third uses an OP27

enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ There's really no need to get cheap for points in .AC analysis, they come fast even when they are thousands/dec, so the visibility is greatly increased. \$\endgroup\$ – a concerned citizen Oct 29 '18 at 20:50
  • \$\begingroup\$ Good point, I usually run 12 or more but I was in a hurry \$\endgroup\$ – laptop2d Oct 29 '18 at 21:18
  • \$\begingroup\$ Turns out it was both! Tested successfully on LT Spice. Thanks @laptop2d \$\endgroup\$ – Rrz0 Oct 30 '18 at 16:57
2
\$\begingroup\$

Here is a simulation, for +6dB gain, using UA741 and MCP655 (and OPA211 with 1 nanoVolt noise density). First opamp is 1MHZ UGBW, 2nd opamp is 50MHz, 3rd is 45Mhz. I used 100pF capacitors for UA741 and MCP655, and the resistors are quite large in value thus are Boltzmann-noisy and the SNR for 1 volt input is only 68dB. OPA211 uses 1,000pF, and produces 82dB SNR.

enter image description here

Here we compare the two BandPassFilter frequency/phase plots.

enter image description here

And here is the thermal-noise plot

enter image description here

By the way, I reran the tool using 1,000pF capacitors, and SNR only increases to 69.8 dB.

So, I switched to the lowest-noise OpAmp included in the tool, the OPA 211 with 1nanoVolt (62 ohms Rnoise) noise-density. SNR rose to 82 dB with 1 volt input. Here that is

enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.