Voltage Doubler Circuit to light a LED with a single AAA battery

Question

I told myself this morning if I did not have this solved by tonight myself I would post it on element14 :-) as a Holiday puzzle. It seems simple enough....

The school my grandson goes to gives out little awards from time to time and he recently selected a "spy kit" as his reward. Inside was a little flashlight / torch that wasn't working. Since all spies need a miniature flashlight he asked me to see if I could fix it. It turned out that it wasn't getting good contact on the positive terminal and was fairly easily fixed. This is what it looks like working:

While I had it apart I couldn't help examining it closer. This is the (very cheap and poorly assembled) PCB.

A single AAA battery powers it. Negative is the red wire and positive is the bare wire coming up between the legs of the LED. The datasheets for the two SOT-23 transistors (J3Y and 2TY) are online and the two resistors and inductor are marked. I removed the capacitor and measured 0.5 nF. Using a multimeter and following the traces in the photo above I came up with this for the schematic.

This is what the output to the LED looks like on the oscilloscope:

Voltage is doubled from 1.5V input to ~3V peak to peak output and is a rough square wave with duty of 24% on and 76% off. Frequency is 215 kHZ. I powered it with the bench supply to see how it behaved as the voltage was lowered and it continued to put out reduced light down to 0.7V input without problem.

I tried simulating the schematic above but only get 1.5V DC output. I may have missed something when tracing the circuit but if so I missed it again when rechecking. Or I may not be simulating it correctly / have wrong values somehow.

Having failed to convince myself I understand how it works I have decided to post it here and see what the experts say...

14rhb · Accepted Answer

Hi Frank,

I can see the diagrams OK.

It strikes me as a bit strange that TR2 shorts the PSU - are you sure there isn't a connection between the anode of the LED (and inductor/cap) and the collector of TR2 ? It would make more sense if there was.

Rod

Gough Lui · Answer

fmilburn - it's a known issue with the site that the images on the first post can't be seen by other members (myself included) due to permissions issues. If you can edit your post by making a trivial change (e.g. adding an extra "." at the end), then the images will show for all of us. - Gough

geralds · Answer

Please can you post the second side of the PCB? Than we can better follow the circuit. So I think something is different as you've drawn. Also the value of the cap. may not 500pF, I think it's a bit larger so up to few nF. I have a similar circuit. Please compare it with yours. Thanks Best Regards Gerald ---

jc2048 · Answer

I can't see the pictures either. From the words, it sounds like it might be a boost converter (a variation of the garden light things). If so, it isn't a doubler as such, the 3V comes from the forward voltage of the LED and just happens to be twice the voltage of the new battery. The two transistors will be an oscillator of some description and the inductor does the voltage boost. There's quite a large class of oscillators that can't start up of their own accord from a static situation [the dc analysis that the simulator does at the start] and need some help to get going (in the real circuit, that help can consist of things like merely the supply coming up or sometimes a small amount of random noise at the right frequency). If that's what's happening here, you'd need to try giving it a (virtual) kick. Depending on the simulator, you may be able to set an initial condition somewhere in the oscillator that will bias it (wrongly) at the start and encourage it to fall into oscillation (Tina-TI has a little circle symbol with 'IC' on it for the purpose), or you could maybe use a generator to give a short pulse just after starting and feed it into the circuit somehow (though that will probably change the form of the oscillation through loading). Another possibility that works for some oscillators is simply to make the supply a generator so that the supply can appear (as a step up from zero) after the simulation start time.

gecoz · Answer

Hi Frank, I think Jon guess is spot on. Looking at the PCB, it looks like is basically a 2 stage amplifier, made with 2 common-emitter stages, in a positive feedback configuration, which creates an oscillator. The positive feedback loop is created by C1. I believe your schematic has C1 wrongly positioned: from the PCB picture I would say C1 goes from the collector of the NPN transistor to the base of the PNP one, and so closing the feedback loop. Also, I think one end of L1 is connected to the positive supply and the emitter of the PNP, but the other end should be connected to the collector of the NPN and one end of C1. The led is then connected between the collector of the NPN and ground. Fabio

fmilburn · Answer

Now that you have pointed it out it makes more sense to me also (I still have not developed an intuition for what is happening in these type circuits). I was fooled by using the beeper on the multimeter and of course getting no resistance across the inductor with DC. I revised the model as shown below:

The model output is shown below:

It differs from the observation on the oscilloscope (Voltage only 2V, duty is different, etc.) but I presume that I am now on the right track?

gecoz · Answer

Hi Frank, Yes, I think you did. And you definitely are on the right track. Also, now qualitatively, you are getting the right results. The difference between the scope observation and the model results could be due to the different values used to characterise the transistors in the model. Did you find use the specific SPICE models for the transistors, or used generic NPN and PNP models? Fabio

gecoz · Answer

All good now. Fabio

jc2048 · Answer

I've tried it in Tina-TI with 2N3906 and 2N3904 transistors and a Nichia white LED and it didn't oscillate. It goes ok if the base of T1 is held at 1.5V at the start (so that T1 starts in the off state). These are the waveforms I get.

gecoz · Answer

Hi Frank, Try using some real transistor model for the NPN and PNP instead of the generic ones. The 1.5V peak is probably due to the LED model you are using, changing the LED model (the N parameter in particular) will help you match the scope output where peak voltage is concerned (you can find some info on SPICE LED modelling here ). As for the output not returning to ground level, this is probably due to the charge/discharge cycle of C1 (I'm assuming that the charge retained by C1 will stop the output to drop down to ground level pushes the NPN transistor into saturation). Fabio P.S: I put together your circuit using LTSpice, and simulate it, using 2 common transistor models and creating my own model for the LED. Below you can see my results

Robert Peter Oakes · Answer

Just a small point... This is not a voltage doubler circuit! It is a boost converter for sure, and I think you may find that if you put in two LEDs in series it will still work, the nature of what it is doing with the inductor is well known and you can read more if you google Buck / Boost converters and the operation of inductors, While T2 is conducting it will establish a current through L1 building up a magnetic field When T2 turns off the conductor will want to keep that current flowing and will therefor increase the voltage as much as it can in order to do that, Once it exceeds the voltage of LED1, it will succeed and current will continue to flow until the field is collapsed and then the process repeats, this is a simplification of a boost convertor. if there are 2 LEDs the voltage will simply rise further until it exceeds the sum of the 2 LEDs, and then allow the current to again flow and collapse the magnetic field again Here is a boost circuit from Wikipedia... look familiar at a basic level (In your case the diode is the load) https://en.wikipedia.org/wiki/Boost_converter <-- Great description here Great post and feedback from everyone but as your learning I wanted to correct that minor name error Enjoy

fmilburn · Answer

It has generic values in the SPICE model. The version I am using has lots of different transistor models but of course not the ones in the circuit. I did not see an equivalent on the datasheet that was also in the model. The model parameters are also missing from the datasheet. But I think I still have something wrong even without tuning the transistor model. The output does not return to the original ground which does not make sense to me and the output peak to peak is still 1.5V.

fmilburn · Answer

Hi Gerald, It was securely glued to a plastic tab and I was concerned about breaking the fragile PCB but went ahead and did it in the name of science. I have since managed to get it back together and working. In the photo below the middle has been mirrored and superimposed as if looking down through the PCB from the top. Both transistors have the same pin configuration which I have labelled on the left. The far right is the unretouched bottom.

Voltage Doubler Circuit to light a LED with a single AAA battery

Top Replies