Building an 3-band analog equalizer, part 1
Yes, I'm building my first pedal guitar !
As a bit of context, it has been a little bit longer than 8 years since I began learning and playing guitar; and making my own effects always seemed appealing to me. Also, I did a fair amount of electronics in college but didn't practiced since. (you may have noticed this blog is more software than hardware oriented !)
The first obvious choice to make when trying to build a guitar pedal is whether to make it digital or analog. Owning myself a bit of analog equipment/instruments, I tend to like the imperfection brought in by non-ideal components, aging, temperature sensibility and other non-linear effects of the analog realm. That's my first pro for analog. Second, digital processing is something I'm more familiar with (that's my everyday job), and even if things always go wrong when you think it's easy, I hope learning more on the journey going for a full analog pedal.
Remains to choose the effect to implement. Staying simple would here be wise, since I will probably struggle on basic matters, so I chose to make my own equalizer pedal guitar.
An equalizer alters the frequency response of a given input signal, often in multiples sub frequency bands. Mine will have three bands targeting low, medium and high frequencies; as is often implemented in the audio processing world.
After some research, I decided to implement three filters following the Multiple Feedback configuration. I will review each of the filter in the next sections, as well as orbiting sub schematics that make everything work.
Multiple Feedback Low-pass
The first filter aims to filter low frequency content. The overall circuit is drawn below:
There is an operational amplifier here (the triangle shape), which makes this design an active filter (without op amp, it would be passive). Because I plan to use — like all great pedals — a single supply of $V_{CC}=9V$ to power my circuit (and my op amps), a DC bias on the non inverting input (the plus sign) is mandatory. I use a simple voltage divider in order to achieve this $V_{CC}/2$ value (schematic below).
Ignore for now the first unannotated capacitor, its purpose is simply to decouple the input signal from $0V$ ground.
We can derive its transfer function in Laplace domain as follows:
$$ H(s) = \frac{-\frac{1}{C_1C_2R_1R_2}} {s^2+s \frac{1}{C_1}\left(\frac{1}{R_1}+\frac{1}{R_2}+\frac{1}{R_3}\right)+\frac{1}{C_1C_2R_2R_3}} $$
That's some equation ! The filter frequency response is completely characterized from the values of the configuration parameters, that is to say: $C_1$, $C_2$, $R_1$, $R_2$ and $R_3$.
The main characteristic of the low-pass filter is its cutoff frequency $f_c$: the frequency at which the filter attenuates the input signal power by $3\text{dB}$ (half the power, $10\text{log}_{10}(0.5)$).
I chose $f_c=200\text{Hz}$ and a damping factor $\zeta$ of $1$. You can either derive the values of the components manually or use this great website to compute it.
After a bit of machine work, those values were yielded:
- $R_1 = 4.3\text{kΩ}$
- $R_2 = 9.1\text{kΩ}$
- $R_3 = 4.3\text{kΩ}$
- $C_1 = 220\text{nF}$
- $C_2 = 68\text{nF}$
I'm not sure I will keep those in the final project, but for completeness and reproducibility of this post I prefer to write those values down.
After getting all my values, I implemented the configuration on LTSpice in order to simulate my filter and validate its behavior. Also, the spice files .asc will be available for download at the end of this post were you wanting to play with it.
Running an AC sweep analysis from $10\text{Hz}$ to $100\text{kHz}$ produced the following gain and phase response (spice directive: .ac dec 10 10 100k).
.svg)
Fine, my filter simulation seems to work and to be in adequation with theoretical predictions. Let's move on to high and band pass filters.
Multiple Feedback High-pass
Next, we need some high-pass filtering to ear those magnificent attack and shimmering frequencies. The high pass configuration differs from the low-pass one by switching capacitors for resistors. It looks like that:
Again, it's transfer function can be derived and its parameters chosen to achieve a particular cutoff frequency. It look as digest as the previous one, don't you think? (jokes)
$$ H(s) = \frac{-s^2 \frac{C_1}{C_3}} {s^2+s\frac{C_1+C_2+C_3}{R_2C_2C_3}+\frac{1}{R_1R_2C_2C_3}} $$
I set my cutoff frequency $f_c=4\text{kHz}$, leading to the following components:
- $R_1 = 3.9\text{kΩ}$
- $R_2 = 9.1\text{kΩ}$
- $C_1 = 6.8\text{nF}$
- $C_2 = 6.8\text{nF}$
- $C_3 = 6.8\text{nF}$
As I did with the low pass filter, I implemented separately this high pass filter in order to check everything is good and running.
.svg)
So far so good, let's tackle the last filter!
Multiple Feedback Band-pass
A band-pass filter can be thought about like the combination of a low and high pass, letting only specific frequencies sneak in the output signal. The MFB band-pass schematic is depicted below:
Designing this one is a bit different than the two previous ones, a band pass filter doesn't have cutoff frequency per se (it has two, even if we can compute them that is not how we define them). The critical value here is the center frequency $f_0$, the frequency response is symmetrical around it and displays unity gain ($0\text{dB}$).
The Laplace transfer function is written like so:
$$ H(s) = \frac{-\frac{s}{R_1C_1}} {s^2+s\left(\frac{1}{R_3C_2}+\frac{1}{R_3C_1}\right)+\frac{1}{R_3C_1C_2}\left(\frac{1}{R_1}+\frac{1}{R_2}\right)} $$
Because I wanted to have a symmetrical combined frequency response, I chose $f_0$ at the intersection of the two last frequency responses, which gave me a value around $900\text{Hz}$. The components values would then become:
- $R_1 = 6.2\text{kΩ}$
- $R_2 = 15\text{kΩ}$
- $R_3 = 7.5\text{kΩ}$
- $C_1 = 15\text{nF}$
- $C_2 = 68\text{nF}$
Implementing the design in LTspice and running the AC sweep made it clear: all filters went through the design step!
.svg)
Something is still missing though, how to merge everything together now ? The essence of an EQ pedal is to be able to amplify or attenuate certain frequencies. We need something like a weighted summing circuit...
Summing amplifier
I love this little piece of circuit, it feels natural and clean. All it does is combining every input signals (here our three outputs coming from the three different filters) with an amplitude function of the three series resistors $R_{HP}$, $R_{BP}$ and $R_{LP}$.
The output voltage is computed via this formula:
$$ V_{out} = -R_F\left(\frac{V_{HP}}{R_{HP}}+\frac{V_{BP}}{R_{BP}}+\frac{V_{LP}}{R_{LP}}\right) $$
The minus sign tells us it's an inverting circuit. The nice thing is that by changing the values of the input resistors, we can either amplify or attenuate the incoming signals, independently. I plan to place potentiometers at those location in order to realize my EQ controllers.
Setting unity gain for all inputs (setting $R_*$ to $R_F$), the global output voltage is plotted next.
.svg)
This is not entirely satisfying, to not say another thing. The ideal response of an EQ pedal, without touching any of the knobs, would be to pass-thru the input signal without any alteration on the frequency response.
But we are doing analog here, and cheap, and ... fast ? I guess ? I'm trying to find excuses. Adding more bands to my design would definitely help solve this problem. For now, I consider that this highly non-flat ugly response will contribute to what every musician calls the tonal character (that's some high level reality dodging right here, I must admit).
I may have to undergo slight modifications / additions (like amplifying first the really weak signal coming from passive guitar pickups) but the meat and potatoes are all there.
And here we have it, a really straight-forward and simple design of a 3-band EQ pedal which runs fine in simulation. I did not research, on purpose, examples of 3-band EQ circuits already existing on the internet. I will when I'm done in order to check how bad I did on my own.
The next step is therefore to order every component, prototype the heck out of those circuits and hopefully solder a working version of this in near-term.
Wish me luck.
Spice full circuit
For reference, the full circuit in format .asc to use with LTSpice is available for download here (along other files on random things I tested before writing this).
You will probably need the library files for the specific op amp I'm using, the TL072. The .sub and .asy can be found in the same repository under the folder simulation/lib/TL072.
