Electronics > Beginners
DC dummy load circuit calibration
<< < (10/20) > >>
VEGETA:
Thanks for the update.

It got more complicated, I started feeling that the USB input is doing all the evil. However, powering it from a DC jack (12-24v) seems a solution but it would require another wall charger that is not as available as the USB one. I myself have a Chinese laptop charger with adjustable voltage from 12 to 24v.

I started thinking about putting two 9v batteries to get 18v from which we could get a negative rail, then make the USB charger to power the panel meter display only. How much would these batteries last?

I don't quite understand what you did. We still have a V_ctrl which I suppose it is coming from our 10-turn POT in which it is powered by a resistor divider as I mentioned earlier.

However, you put another POT which is RV1 and this one I don't seem to be able to control it. Also, we have R1 and R5 which I assume are variable resistors not pots for trimming. I hoped to get only 10k pots so I guess I can change them.

I don't like LM317, it gives extra cost for nothing. I would just put a resistor divider instead, will it work?

So we need to make it a bit simpler especially if the 2 batteries thing works fine.
VEGETA:
Your version 3 seems nice for 12v input, which I can work with now assuming all these stuff that results from 5v. I've got to make sure it doesn't have the balancing issues. Even version 4 seems easy but without individual calibration
Ian.M:
I should have drawn a box round the Vctrl source and labelled it 'Sim only'.   All it does is provide a 0% to 100% control input for the wiper position to the symbol for the 10K pot RV1.  (The pot model takes an absolute voltage 0 to 1V, as its wiper position.)

RV1 represents your 10K ten turn pot that will be the 'master control' to set the current.  R1 and R5 are presets - you adjust them ONCE to get zero current at one end of RV1's range and your desired maximum current at the other.   However as the value won't be convenient, you'll probably use a fixed resistor + a preset in series, or if you've got a limited selection of presets available , maybe with an extra resistor in parallel to the series pair. 

As the circuit only needs about 100mA, a laptop charger would be stupid overkill.  OTOH 9V batteries will give you nothing but trouble with the voltage change as they discharge causing the set load current to drift.  They are great for quick breadboard experiments, but a horrible way of getting even a few mA for long periods unless portability is the major factor.   If it weren't for the need to provide a stable regulated voltage to the potentiometer the batteries wouldn't be such a problem, but  the 10mA minimum load current needed by the LM317 makes them impractical. 

My main objection to USB chargers for powering test equipment (apart from the generally high ripple and poor regulation of the cheap ones) is the risk of user stupidity, especially when doing something unconventional like grounding their positive output terminal  to get -5V from them.   An alternative to mounting the USB charger internally would be to take one with a permanently attached output lead, cut off its USB plug and replace it with a DC power jack.  That removes the risk of someone powering the unit from a PC or a multi-output USB charger without even thinking about it.


I don't like the LM317 either, but its essential to have a clean well stabilised supply to the control potentiometer.    Even though the positive rail is from a regulated supply, the load on it varies considerably and as its a switching supply, there will be a lot of ripple so putting it through a LM317 to clean it up and drop it to a far more convenient voltage for the pot.  Alternatively, you could use a Zener fed by a resistor from the positive rail, or even use a forward biassed LED in place of the Zener, which can also do double duty as a power LED.  If you can get TL431 shunt regulators locally, that would be great - 2.5V is more than is ideal to feed the pot, but R1 can easily be increased to compensate.

Version three powered by 12V will have its own issues - a Vbe multiplier isn't a very good shunt regulator, as its voltage changes significantly with the current through it, and with temperature and I didn't add any parts to ensure the MOSFET can be controlled right down to zero current.   Also, the display current ground return goes through the Vbe multiplier, which means neither the negative nor the positive rail will be stable enough to derive the control voltage from by a simple resistor divider.
VEGETA:
Here is my more friendly ltspice, changes are:

1- Made the 10-turn pot a friendlier version of 2 resistors to make it easier for me to see.
2- put 100k fixed upper limit which corresponds to 2.08A maximum current, which is what we want. this could be a pot but I didn't want to get other values than 10k pots and the resistors we use.
3- made the zero trimmer 10k pot, but set it to around 1k.
4- adjusted the supply options. I ditched the USB completely and put 12v DC jack from laptop\wall charger (the laptop one is 5$). Now we have apporx. 9v positive and -3 negative.
5- I kept LM317 for now since there are no better options available. TL431 will need another month to arrive so meh. Plus, I don't know how to use it yet.
6- Instead of 120 ohm for LM317, I added an LED to act as power on LED. I guess 1.25v could give us around 10mA without any series limiting resistors.

What I need to understand is :

1- how can this circuit achieve balancing better that previous methods?
2- why now choose 1k as feedback resistor?
3- Can we use ceramic only caps in this design? or should decoupling caps be electrolytic?

Can we call this the final design?
Ian.M:
1.  The balancing is purely due to each MOSFET having its own  OPAMP and individual source current sense resistor.  The individual MOSFETs are *NOT* in parallel so one cant hog more current - its own feedback loop prevents it taking more than the voltage at its OPAMP's in+ commands.

2.  I decided to simplify the design, knowing you prefer 1K 10K 100K etc resistor values.    It makes little difference except to the -3dB bandwidth enforced by it and the 100pF cap.

3. I'd use a mix - ceramic up to whatever value a good quality electrolytic becomes significantly cheaper above.  N.B.  High K ceramics are very voltage sensitive, with the capacitance dropping as the voltage across them increases.  If you run them near their max rated voltage, you only get a small fraction of their nominal capacitance, so you'll need 50V rated ceramics to get anywhere near their nominal capacitance from them.

Its not a final design - its taken several steps backwards from the last one I posted.

The sim has major problems - you've got 10 Million Amps flowing through that LED you added, and replacing my voltage controlled  potentiometer with fixed resistors makes it impossible to do any sort of stability testing.   However as an experiment I added a behavioural current source (standard LTspice component 'bi') sinking current from the Vcc rail to Gnd to represent the current drawn by your LED panel meter using the expression

--- Code: ---I=20mA+40mA*rand(time*100)
--- End code ---
which is a current somewhere between 20mA and 60mA randomly changing 100 times a second.   The results were horrifically bad - nearly a volt peak to peak of noise on the Vcc and Vee rails, and a lot of breakthrough to the controlled load current which will jump around like a flea with hot feet.

The LED issue is just stupid - a real LED wont draw 10mA with 1.25V across it unless you are very very lucky but it certainly wont draw 10MA - thats an artifact of it defaulting to the default diode model because you didn't select a LED.  Never the less, its Dumb with a capital D to attempt to drive a LED directly from a low impedance voltage source.  If you want to stick a LED in somewhere put it in series with R4, which keeps the Vbe multiplier biassed.   You could probably even remove the LM317 and use the voltage developed across the LED to feed the pot*.   Here are some LED models for you to sim that with:

--- Code: ---*Typ IR LED from optocoupler: Vf=1.2V @10mA
.model LED0 D (IS=1p N=1.999644 RS=0 BV=6 IBV=10u
+ CJO=10p EG=1.424 TT=500n)

*Typ RED GaAs LED: Vf=1.7V Vr=4V If=40mA trr=3uS
.MODEL LED1 D (IS=93.2P RS=42M N=3.73 BV=4 IBV=10U
+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)

*Typ RED,GREEN,YELLOW,AMBER GaAs LED: Vf=2.1V Vr=4V If=40mA trr=3uS
.MODEL LED2 D (IS=93.1P RS=42M N=4.61 BV=4 IBV=10U
+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)

*Typ BLUE SiC LED: Vf=3.4V Vr=5V If=40mA trr=3uS
.MODEL LED3 D (IS=93.1P RS=42M N=7.47 BV=5 IBV=30U
+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)
 
*Typ small White LED: Vf=3.2V Vr=5V If=35mA
.MODEL LED4 AKO:NSSWS108T

--- End code ---

If you go with this design without resolving the issue with the Vbe multiplier and the meter supply current, I'm washing my hands of this whole project and ignoring this topic.   Just in case: Thank you for an interesting technical challenge so far, its been pleasant working with you.

* using the voltage across a LED as a reference isn't ideal but if you don't care much about its initial accuracy and stability it works well enough if the current through the LED is near constant.  Its even been done in commercial products - e.g. Microchip's original ICD debugger used a red LED as a reference.
Navigation
Message Index
Next page
Previous page
There was an error while thanking
Thanking...

Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod