Breadboarding a Simple MOSFET Booster

Once I finished building LPB-1 boost pedal, I thought why not taking another boost design and maybe see how that works. How does it relate to the one I already built? Are there any similarities? What about differences?

I’m looking into seeing how pedals are designed around different active components, like for example MOSFET transistor. I learned a lot from amzfx web site and there, I came across Jack Orman’s AMZ Mosfet Booster. It is relatively simple boost effect, but in lots of ways different from LPB booster I built earlier.

In this article I’ll get to know the circuit, run some simulation in SPICE and then breadboard it. In the follow-up article I’ll prepare the enclosure and complete the pedal on a protoboard.

Getting to Know the Effect

Now, this is a bit silly heading. The best way to get to know an effect is to play guitar through it. This is getting to know it from technical perspective I suppose.

I got the schematic from the official page for the effect. The page gave me a good introduction to the effect itself. So let’s go through the schematic and familiarize ourselves with it.

By looking at the schematic I can tell straight away that the effect is more complex than the one I made earlier. Here are the important bits:

Amplifier

The amplifier part is all that’s not highlighted. It is a common source MOSFET amplifier. The active component is Q1 – MOSFET transistor, and on the image, that is BS170. The effect’s page gives several possible options for suitable MOSFETs.

LPB-1 is using BJT (bipolar junction) transistor, but AMZ Mosfet booster is using a different one – a MOSFET transistor. MOSFETs are FET (Field effect) transistors and they are working on a different principle from BJTs.

In simple terms, difference between BJTs and FETs is that BJTs are current controlled devices and FETs are voltage controlled devices. In FETs, voltage is controlling the current gain – hence the gain parameter for FETs is transconductance. That makes the circuit design different, causing different parts of the circuit to have different trade-offs.

The rest of the components are there to establish DC bias and to stabilize quiescent point. That is very similar to the LPB-1 circuit; however, things are a bit more complex than biasing BJT. In order to work as a linear amplifier, the MOSFET needs to be kept in saturation region (equivalent to active region in BJTs). Unlike BJT, its transconductance, and thus gain (which is equivalent to gain – h_FE or beta – in BJTs) depends on Q-point, whereas for BJT is almost constant.

R1 & R2 are forming voltage divider and are setting the biasing point of the transistor. R4 and R5 contribute to this greatly. R4 helps with Q-point stability, but lowers the gain of the amplifier. Gain is directly proportional to the R5 value. R5 establishes the output impedance. But everything is a trade off, R4 and R5 need to also keep transistor in saturation, changing their values changes drain current which changes transconductance.

R3 and C3, strictly speaking are not needed for biasing, but in this configuration help with noise and input impedance. C3 is there to help with noise or ripple coming from DC supply and since that would short AC (input signal) to ground, R3 is added. R1 and R2 voltage divider is bypassed by C3 for AC signals, so input impedance is going to be equal to the value of R3.

Coupling Capacitors

Coupling capacitors serve the same purpose in all of the effects – blocking DC component on input and letting only signal go to the output. Output capacitor is 100nF like in the LPB circuit. But the input one is just 1nF which is different to the LPB circuit.

Values of these capacitors could affect frequency response but 100nF is big enough value not to cause any effect. C1 forms high pass filter with very large resistor R3 and that gives us about 15Hz cut-off frequency, that won’t affect our sound either. (I used a filter calculator for this calculation).

Transistor Protection

BS170 has maximum V_GS value of 40V (non-repetitive). Voltages over this may (and will) get it fried. Zener diode is there just to prevent this damage from happening, it does not affect sound.

Optional Cap

Optional Cap – C2, it is there to help with RF interference.

Gain Control

I left this for last, this is the biggest difference to me from LPB circuit. The gain of LPB is fixed, but here – potentiometer is affecting source resistance and thus the gain. C5 cap is there so potentiometer does not affect the biasing point – for DC current it acts as open circuit, for AC signal it acts as short circuit.

Small signal gain of the amplifier is roughly resistance at the drain divided by resistance at the source – in this case it is: -R4/(R5||R6). Notice the pot wiring: going clockwise (CW) the resistance decreases thus casing the gain to go up. Going counterclockwise (CCW), resistance increases, thus gain is decreasing. Note the negative sign since this is inverting amplifier.

Now, at maximum gain (pot completely CW) – transistor source is at ground, so the above formula does not work. The gain depends more on transconductance and is in line with what the effect’s page says – about 35dB (my very crude calculation says about 32dB – but transistor parameter values vary so much that it’s not miles off). Minimum gain is around 3dB as expected.

C5 is large enough so the gain is evenly applied across the whole frequency range.

Simulating Effect in SPICE

One thing that I always do when I am working with new schematic is to simulate the circuit in SPICE (“Simulation Program with Integrated Circuit Emphasis”). Definitely not a required step – but highly recommended.

SPICE allows me to simulate the circuit and get better understanding how the circuit works. For example, it can show me DC characteristics (so I can confirm my calculations – or catch any of my errors), I can see frequency response of the circuit, then how the actual signal looks like (good to see if there’s any clipping for example), etc.

The Circuit in SPICE

SPICE covers all components that I need here. I’m using LTSpice – but any will do. It’s very simple to draw circuit in it:

Looks nearly the same as the original drawing, right? Word of caution is in order here: SPICE is great – but the result is only as good as the model used. For this simulation, I got a model of BS170 online since it does not come with LTSpice. I always take these simulations as a guide only, even when I’m absolutely certain about the models used, the real devices have a lots of variability anyway.

Couple of notes – I took a 9.1V Zener diode model that comes with LTSpice, not the one I have but it is not important since it does not affect signal (but if I had it incorrectly wired it would’ve).

I created a function – pot_linear_ccw – that takes 2 parameters – pot resistance and gain. Gain has value from 0 to 1 (0 meaning minimum gain, 1 maximum gain).

Bits not shown on the circuit image above are here:

I kept all the commands I’ll be using on the same file. Using semicolon (;) to comment out various commands I don’t use at the time. I’ll touch upon them when I use them later.

DC Operating Point

It’s very easy to get our DC operating conditions in SPICE (bias point). Command for that is .op and gives the following result:

The important values:

• V(A): 5.4173 V (within expected range, but remember, this is simulation, needs to be verified once I breadboard the circuit)
• Id(Q1): 1.32692 mA – our bias drain current

That’s it … not too many important bits, but at least they confirm what I expected to get (within wide tolerance margin anyway).

The .param Gain value is not important since there’s no input signal and C5 acts as an open circuit so it does not affect DC point.

AC Analysis

For this I used step param and .ac commands:

.step param command will cause simulation to be run 11 times – once for 0, 0.1, 0.2 … 1 values for the Gain. Each graph will be plotted in different colour and will show me frequency response and gain I would expect if I turned pot knob clockwise 10% each time.

Here’s the result:

The top graph is when the pot is all the way to the max, the gain is about 28dB with cut-off frequency of 15Hz (give or take). So the max gain according to SPICE is lower than what was expected. Again, 2N7000 might give different result, the physical device I put into the circuit might give different result, just something to keep in mind.

When the pot is at 90%, the gain isn’t 90% – the gain is about 14dB, then when pot is at 80% the gain is about10dB. Minimum gain is about 3dB. I think I mentioned in the article on LPB that due to how ear perceives loudness, for perceived linear increase in volume – the actual increase in signal level has to be exponential.

Gain Control Law

If I do a gain control law for the circuit (I can do this by still using step param for Gain but do frequency analysis at 1KHz – .ac list 1000) and plot ideal control line I get this:

I plotted ideal (exponential) curve on a log scale (thus plotted as straight line) in blue. That would be the ideal gain curve. The green is the expected gain. It deviates a lot from the ideal, again, this is all in theory. In practice, based on this, I should expect that volume increase will go slowly and at the last 20% of rotation of the pot it will just go louder very quickly. We’ll see later if theory matches practice.

I assumed linear pot, I didn’t see anything stated on the effect’s page. Using log pot would cause even greater deviation. Big factor in this is that source resistance is affected by R5 that is in parallel to the pot.

Transient Analysis

Finally, let’s see transient analysis. I’ll do it for 50%, 80%, 90% and 100% pot position. Command .tran 50ms plots 50ms of the wave signal:

Green graph is for pot at 50%, blue at 80%, red at 90% and azure (huh?) at full rotation. (Conveniently, for a pot with 300^o rotation range, which I’ll be using, that translates to 12, 3, 4 and 5 o’clock respectively).

I suppose, the main takeaway here is that at the highest gain, signal clipping will start occurring. Looks like this will only happen at the very last 10% of pot rotation. It is going to be interesting to hear how that sounds. Note that input signal for this simulation is set to 0.1V.

Characterizing the Effect

In order to describe the pedal, all pedals list input/output impedance, gain, and lots of them give expected power consumption. After I’ve done all the calculations and simulations this is what I get:

Parameter	Value
Input Impedance	10 Mohm (set by R3)
Output Impedance	about 2.7Kohm (set by R4)
Gain	From 3dB to 28dB
Current Draw	1.3 mA average (without LED indicator)

All parameters are very good for a boost pedal.

Breadboarding the Effect

Let’s breadboard the effect and hear how it sounds.

I did a short video on just getting it to work on the breadboard.

Ideally – steps before making the pedal permanent might be getting the drain voltage to exactly where you want it, voltage wise. Check out the sound between BS170 and 2N7000 for example and choose which one you like (if you can tell the difference).

One thing to note is the pinouts for BS170 and 2N7000 are different (if you’ve seen my video you know this by now … DOH!) Anyway, I’ll be soldering the effect soon enough so stay tuned.