What components from MultiSim to use, to set voltage input, output and adjust in this 0V to 30V LM317 regulator-based circuit - is it DC_POWER?

[aryniec-pw]

I have such example circuit that uses LM317 voltage regulator: Figure 12. 0-V to 30-V Regulator Circuit

It's from chapter 9.3.1 of Texas Instruments' LM317 documentation.

I wonder what components should I use to set these voltages in LM317 Input, Adjust and Output, i.e. +35V, -10V and 0V?

Currently I'm using DC_POWER component in all three, from Sources -> Power Sources component family, but I have some doubts whether I chose correctly.

Anyone can share a hint with beginner electronics engineer?

[tipa]

Здравствуйте! Промоделировал Вашу схему. Правый график при R3=3кОМ. Есть чёткая стабилизация напряжения на уровне 29,7 Вольт. Момент стабилизации наступает при сопротивлении нагрузки 13,9 Ом и токе 2,14 Ампер.
Левый график ведёт себя по хитрому. В некоторый момент синяя и зелёная кривые меняются местами. От R=152 Ом, до 153.

[tipa]

Это может быть регулируемый, и стабилизатор тока, и стабилизатор напряжения.

[GGoodwin]

Hi aryniec-pw,

I opened the LM317 documentation and I can see that there is/are error(s) in this example circuit that you attached. There are inconsistencies in the circuit and the formula.

When designing an LM317-based voltage regulator which can be adjusted down to 0 V, the most common configuration will be more similar to the circuit which I contributed to Multisim Live (LM317 Adjustable Down To 0 V Voltage Regulator). However, because the components available for Multisim Live Free Subscription is limited, I set the maximum output voltage to just about 12 V in my circuit.

In "my circuit" you can see a component which is represented using the symbol for Zener Diode. This is actually a Voltage Reference IC such as LM313.

I cannot provide more details right now because of limited time available I suggest that you make the modifications to your circuit as tabulated below:

R1 : replace with 200 Ω
R2 : replace with 5 kΩ
Diode : replace with voltage reference IC such as LM313

We can make improvements to this circuit later.

Best regards,

G. Goodwin

[aryniec-pw]

Thanks for hints!

This "0-V to 30-V Regulator Circuit", I'd like to edit and make it from 0V to 20V.
0-V to 30-V Regulator Circuit

Also, I'd like to know for sure, I got this schematics right, so I need to know exactly what the component's name in MultiSim every part has.

Starting from bottom it's grouding.

Going right-to-top from grounding:

1. is simple model 1BH62/package 3-3B1A diode by Toshiba.

2. going top more is R3 resistor, but in my case it should be AD5246 resistor, because I need to use this particular one.

3. upper from R3 is VDC1 power source with -10V voltage value.

4. right to R3 resistor is R2 potentiometer

5. above R2 potentiometer, there's R1 resistor, same as R3 resistor, but different resistance value.

6. above R1 resistor there's Output voltage to the right of R1, which should be measured by some voltage probe; and LM317 voltage regulator to the left of R1

Going left-to-top from grouding:

1. there's capacitor

2. top-left from capacitor is voltage power source with value from 0V up to 20V

3. top-right from capacitor is LM317 voltage regulator

My questions:

1. what percentile tolerance should capacitor have?

2. what percentile tolerance should both R1 and R3 resistors have?

3. what percentile tolerance should R2 potentiometer have?

4. what specific component/tool should be use as a voltage probe for this circuit Output? Currently using default MultiSim voltage probe.

[aryniec-pw]

Btw. I had no LM317 built-in into my MultiSim 14.3 Education Edition, so I copied LM117HV component into User Database end edited it's model using this LM317H model:

.SUBCKT LM317/TI in adj out
* PEI 08/98 p62
J1 in out 4 JN
Q2 5 5 6 QPL .1
Q3 5 8 9 QNL .2
Q4 8 5 7 QPL .1
Q5 81 8 out QNL .2
Q6 out 81 10 QPL .2
Q7 12 81 13 QNL .2
*Q8 10 5 11 QPL .2
Q8 10A 5 11 QPL .2
Q9 14 12 10 QPL .2
Q10 16 5 17 QPL .2
Q11 16 14 15 QNL .2 OFF
Q12 out 20 16 QPL .2
Q13 in 19 20 QNL .2
Q14 19 5 18 QPL .2
Q15 out 21 19 QPL .2
Q16 21 22 16 QPL .2
Q17 21 out 24 QNL .2
Q18 22 22 16 QPL .2
Q19 22 out 241 QNL .2
Q20 out 25 16 QPL .2
Q21 25 26 out QNL .2
Q22A 35 35 in QPL .2
Q22B 16 35 in QPL .2
Q23 35 16 30 QNL .2
Q24A 27 40 29 QNL .2
Q24B 27 40 28 QNL .2
Q25 in 31 41 QNL 5
Q26 in 41 32 QNL 50
D1 out 4 DZ
D2 33 in DZ
D3 29 34 DZ
R1 in 6 310
R2 in 7 310
R3 in 11 190
R4 in 17 82
R5 in 18 5.6K
R6 4 8 100K
R7 8 81 130
*R8 10 12 12.4K
R8 10A 12 12.4K
R9 9 out 180
R10 13 out 4.1K
R11 14 out 5.8K
R12 15 out 72
R13 20 out 5.1K
R14 adj 24 12K
R15 24 241 2.4K
R16 16 25 6.7K
R17 16 40 12K
R18 30 41 130
R19 16 31 370
R20 26 27 13K
R21 27 40 400
R22 out 41 160
R23 33 34 18K
R24 28 29 160
R25 28 32 3
R26 32 out .1
C1 21 out 30PF
C2 21 adj 30PF
C3 25 26 5PF
CBS1 5 out 2PF
CBS2 35 out 1PF
CBS3 22 out 1PF
.MODEL JN NJF (BETA=1E-4 VTO=-7)
.MODEL DZ D(BV=6.3)
.MODEL QNL NPN (EG=1.22 BF=80 RB=100 CCS=1.5PF TF=.3NS TR=6NS
+ CJE=2PF CJC=1PF VAF=100 IS=1E-22 NF=1.2)
.MODEL QPL PNP (BF=40 RB=20 TF=.6NS TR=10NS CJE=1.5PF CJC=1PF VAF=50
+ IS=1E-22 NF=1.2)
.ENDS LM317/TI

[tipa]

Привет, -возможно я не так вас понял. За основу взял эту разработку , и собрал в MS. Поскольку MS не умеет делать анализ параметрический с расширением рабочая точка DC, пришлось схитрить, и вынести точки питания в отдельную схему и не включать её в симуляцию. Таким образом удалось получить по нижней оси-сопротивление, и по боковой- напряжение. А также выяснить на какой максимальный ток способна эта модель, изменяя источник тока в нагрузке.

[tipa]

В этом анализе определим, с какого значения сопротивления нагрузки начнётся просадка напряжения стабилизации. Получилось резкое падение после 15 Ом

[GGoodwin]

Hi aryniec-pw,

Here are the details about the error(s) or inconsistenc(y/ies) in Figure 12, §9.3.1 of LM317 3-Terminal Adjustable Regulator "Documentation" as I mentioned in my previous reply. I hope I did not convey the thought that the formula is wrong. What I mean is, the circuit will not work (accurately) as described "0-V to 30-V Regulator Circuit" and this can be proven using meticulous computations and with the aid of the formula.

Provided below are the computations to determine the minimum (when R2 is adjusted all the way down to 0 Ω) and maximum (when R2 is adjusted all the way up to 3 kΩ) output voltages. Step-by-step computation and substitution of appropriate values to the formula were used to verify that the results are correct. Widen your browser window to properly view the computations.

Current in R1 (Ir1)

Ir1  =  Vr1 ÷ R1
Ir1  =  1.25 v ÷ 120 Ω  =  (250 ÷ 24) mA
Ir1  =  10.416666666666666666666666666667 mA

Voltage drop in R3 (Vr3)

Vr3  =  Ir3 * R3  ≈  Ir1 * R3
         Vr1            1.25 V
Vr3  ≈  ───── * R3  ≈  ──────── * 680 Ω
         R1             120 Ω
Vr3  ≈  7.0833333333333333333333333333333 V

Minimum output voltage

Minimum voltage drop in R2

Vr2(min)  =  0 V

Vout(min)  =  Vr1 + Vr2(min) + Vr3 - 10 V
Vout(min)  =  1.25 V + 0 V + 7.0833333333333333333333333333333 V - 10 V
Vout(min)  =  -1.6666666666666666666666666666667 V

Maximum output voltage

Maximum voltage drop in R2

Vr2(max)  =  Ir2 * R2(max)  ≈  Ir1 * R2(max)
              Vr1                 1.25 V
Vr2(max)  ≈  ───── * R2(max)  ≈  ──────── * 3 kΩ
              R1                  120 Ω
Vr2(max)  ≈  31.25 V

Vout(max)  =  Vr1 + Vr2(max) + Vr3 - 10 V
Vout(max)  =  1.25 V + 31.25 V + 7.0833333333333333333333333333333 V - 10 V
Vout(max)  =  29.583333333333333333333333333333 V

We will verify these step-by-step computed values of Vout(min) and Vout(max) using the formula

Minimum output voltage
                  ┌                    ┐
                  │      R2(min) + R3  │
Vout(min)  =  Vr1 │ 1 + ────────────── │ - 10 V
                  │           R1       │
                  └                    ┘
                     ┌                   ┐
                     │      0 Ω + 680 Ω  │
Vout(min)  =  1.25 V │ 1 + ───────────── │ - 10 V
                     │         120 Ω     │
                     └                   ┘
Vout(min)  =  -1.6666666666666666666666666666667 V

Maximum output voltage
                  ┌                    ┐
                  │      R2(max) + R3  │
Vout(max)  =  Vr1 │ 1 + ────────────── │ - 10 V
                  │           R1       │
                  └                    ┘
                     ┌                    ┐
                     │      3 kΩ + 680 Ω  │
Vout(max)  =  1.25 V │ 1 + ────────────── │ - 10 V
                     │         120 Ω      │
                     └                    ┘
Vout(max)  =  29.583333333333333333333333333333 V

Here we can see that the values of Vout(min) and Vout(max) computed step-by-step and using the formula match.

We first evaluate the maximum output voltage, Vout(max). The computed value of 29.583333333333333333333333333333 V is 416.66666666666666666666666666667 mV lower than 30 V. If I am going to build a real circuit, this deficiency is unacceptable because it can be reduced by rigorous computation of resistances. Nevertheless, it might be acceptable to you if you only want slack specifications for your circuit.

On the other hand, the computed value of -1.6666666666666666666666666666667 V for the minimum output voltage, Vout(min), is certainly objectionable. It is larger in magnitude than the minimum obtainable with the more rudimentary circuit (Figure 9. Adjustable Voltage Regulator, §9.2 of LM317 3-Terminal Adjustable Regulator "Documentation") as shown below

In the circuit depicted in the image above, the minimum output voltage, Vout(min), obtainable is about +1.25 V. Take note of the + sign, that is to emphasize that Vout(min) does not go negative. Reversal of polarity can be catastrophic for many kinds of loads.

Therefore, Figure 12. 0-V to 30-V Regulator Circuit, §9.3.1 of LM317 3-Terminal Adjustable Regulator "Documentation", where you want to base the circuit that you want to create, is erroneous and potentially dangerous. It is more complicated, requires more components, yet needs to be sedulously revised to become usable.

Best regards,

G. Goodwin

[aryniec-pw]

So why would Texas Instruments publish erroneous schematics?

Someone made a mistake?

Because I doubt they would do this on purpose, so people recreating this schematics physically could get hurt.

On the other hand, we decided to change the range and go with 0V to 20V instead of 30V.