There was a time when taking a low DC voltage — say a single battery — and converting it to a higher voltage was painful. Now, however, cheap and easy-to-use DC to DC converters are readily available. For some small tasks, though, these can seem like overkill. For example, consider a case where you need to supply a higher voltage for a MOSFET gate that doesn’t draw much current. Perhaps you need that higher voltage to trigger a microcontroller’s programming mode and nothing else. The current draw is minimal, and a full-blown DC to DC converter is overkill. For cases like that, it is tempting to use some voltage multiplication scheme. There are many, but for this post, I’m going to take you inside a Dickson charge pump. This is Circuit VR because not only are we going to discuss the circuit, we’ll look at an LT Spice simulation you can try yourself.

The Dickson is interesting because it doesn’t require any AC conversion or transformers. Instead, it uses diodes or other switching elements to transfer charge between capacitors in stages. Each stage will effectively increase the voltage by the supply voltage — in theory. Reality isn’t so kind, though, as we’ll see.

Perfect World

Here’s the LTSpice schematic for the charge pump. You can download the file from GitHub.

Vin is just the supply voltage: 3.3 V in this case. Vphase0 and Vphase1 are two square waves that are the opposite of one another. That is, when Vphase0 is high, Vphase1 is low and vice versa. These are probably outputs from a microcontroller, although it could be a 555 and an inverter or any other two-phase clock source you can dream up.

Consider the very first moment of operation. C1 is empty and Vphase0 is low. C1 will charge through D1 until it is at voltage Vin.

Then Vphase0 goes high. The capacitor stores energy so it can’t just go to zero volts across it like a resistor would. In fact, when we say C1 will charge to Vin, what we really mean is the voltage across the capacitor will charge to Vin. And since Vphase0 is now at Vin, the voltage across C1 is still Vin and so the voltage from the junction of D1, C1, and D2 will be twice Vin: Vin from Vphase0 and another Vin from C1.

The process repeats with the next stage. C2 charges to 2 x Vin while Vphase1 is low and then jumps to 3 x Vin when Vphase1 goes high. In theory, you could add as many stages as you like to get an integer multiple of your input voltage. The final capacitor, C5, doesn’t add any voltage because it connects to ground, but smooths out the output.

Reality Check

Of course, the reality is a little different. The diodes drop some voltage. I used Schottky diodes to minimize the effect, but still. The output square waves are not going to get all the way to the supply rail. The more current you draw, the more you are going to droop the capacitors when they are storing energy instead of charging and that’s going to affect the output, too.

So how bad is it? LT Spice can easily answer that question. If you haven’t used it before, LT Spice is a great adaptation of Spice which is well-known circuit simulation software. LT Spice is from Linear Technologies, but they offer it to the community without charge. You can download it from the Linear website. If you need a quick tutorial, we had one earlier you can check out, or have a look at the video at the end of this post. Although LT Spice runs under Windows, it works well on WINE so you can run it on your other computers, too.

Spice Tricks

It is really easy to just draw a schematic and simulate it. However, I used a few tricks to make things easier. C1 to C4 all have the same value and if you want to experiment with the values it is very painful to enter each one of them. The three voltage sources are the same, too. While there is only one RL, representing the load resistor, it is also a parameter you probably want to change during testing.

To make things easier, I didn’t assign specific values for these items. For C1 to C4, I assigned {C} as the value. This means somewhere else I have to specify a parameter named C. I also used parameters {RL} and {V}. If you look near the top left of the schematic, you’ll see a .params command that sets the three parameters. This makes it really easy to change things to try different scenarios.

The other nice thing you can do once you have a parameter is to sweep it to different values. That’s what the .STEP directive at the very top does. It varies C to three different values. You can also omit the LIST keyword and just provide a start, stop, and increment. For example, .STEP C 0.1u 1u 0.2u would cause the simulation to use 0.1, 0.3, 0.5, 0.7, and 0.9 as step values. Of course, you can remove the .STEP line if you just want a simple simulation.

Result

You can see from the results below that larger capacitors (C1–C4) help to a point. Of course, the bigger C5 and the higher RL, the longer it will take to charge to the final value. The green trace is the 10 μF run. The blue and red traces are for 1 μF and 0.1 μF, respectively.

You’ll notice the period of both clock signals is 1 ms or 1 kHz. Each stays on for exactly half that time (500 μs) but Vphase1 has a 500 μS delay at the start. This is what keeps them out of phase. If you want to experiment with frequency, duty cycle, or rise and fall times, you can open those two sources and make changes. In general, higher frequency leads to better results and smaller capacitors, at least to a point. Parasitic capacitance is always a problem and gets worse as frequency increases.

You might also want to try different values of C5 or try replacing the diodes with ordinary diodes to see what that costs you. Of course, changing the load resistance to draw more current will change things. For example, look at the simulation below that uses .step param rl 1k 10k 100k.

At 1 kΩ, you barely get any increase at all. The load is drawing almost 4 mA. With 10 kΩ you get between 3X and 4X multiplication. At 100 kΩ you get more than 4X. Try changing C to 10 μF and you’ll see better results. Or try 47 μF. You might also want to increase C5 at 1 kΩ to get better filtering. You can see how thick the lower traces are which is the unfiltered ripple.

Probably the best thing to do, though, is to simply probe different parts of the circuit to visually see how each stage builds on the previous one. Don’t forget you can measure currents, too, which can often provide insight into circuit operation. However, when using the .STEP command, you only get the nicely colored traces if you display only one value. If you add multiple traces, each family of traces will get a single color.

The Value

That’s the real value to simulation. A few minutes of playing with this circuit and you’ll have a feel for what parameters change the output. That incredibly valuable. Sure, you could breadboard the circuit and that’s probably the next thing you should do, but it isn’t nearly as time and cost effective as using a simulator like LTSpice when you want to tweak many parameters.

Is it perfect? No, a breadboard version will probably be a little different because I used ideal capacitors. If you right click on each capacitor and pick a model of an actual capacitor, you might notice some slight differences because the model takes into account parasitic resistance and other effects.

There are other techniques you can use to modify the Dickson charge pump. For example, on an IC, the diodes are likely to be MOSFETs. There are also variations that try to overcome the diode switching threshold or correct other undesirable effects.

One of the most interesting things about simulation like this is you can easily probe anywhere and quickly try out new ideas. Maybe you’ll come up with a new architecture for a multiplier and they’ll name it after you.