# Wien Bridge Oscillator not working by its own theory in simulation

#### Vincent Ng

Joined Dec 7, 2015
6
Hello guys, I need some help with the Wien bridge oscillator which I need to generate 150kHz Sine waveform.
According to theory the wien bridge oscillator just need the RC to be work
but when simulated in proteus, the waveform doesnt come out,
I changed to OrcaD, instead the result become like attached, the oscilation become weaker and weaker with triangular like waveform

#### Alec_t

Joined Sep 17, 2013
12,319
Have you read the datasheet for the 741 opamp? The power supply should be dual-polarity, or else have a virtual earth at half the single-polarity supply voltage. Also, the 741 has a low gain-bandwidth product, so will perform poorly at 150kHz.

#### AnalogKid

Joined Aug 1, 2013
9,494
1. There is no current path between the ground symbol and either of the battery terminals. This will cause both the simulation and an actual circuit to fail. The path does not have to be a direct connection, but the non-inverting input needs some kind of reference that is related to the power pin voltages.

2. Getting a 741 to do *anything* at 150 kHz is very difficult because the part has a relatively small gain-bandwidth product.

3. A Wein circuit requires gain-stabilizing components to keep the opamp from saturating. In the classic circuit this is a small incandescent light bulb, but a transistor used as a voltage-variable resistor also works. Search the innergoogle for Wein bridge oscillator schematic to see dozens of examples.

ak

#### Vincent Ng

Joined Dec 7, 2015
6
So do I have to change the op amp?
Have any suggestions for the op amp?

#### crutschow

Joined Mar 14, 2008
28,207
• Change the op amp to one with a gain-bandwidth-product of at least 10MHz. (What op amps do you have available? Look in their data sheets to find one with the desired response.)
• Change to separate plus and minus supplies referenced to ground.
• Change the simulation time to at least 1ms.
• Use the .ic command (or equivalent) to skip the initial DC bias calculation in the simulation.

#### Vincent Ng

Joined Dec 7, 2015
6

I changed the OP amp into LM381 which equivalent to CA3130 which have 15MHz gain bandwidth, produced this result
Whats the problem?

#### Alec_t

Joined Sep 17, 2013
12,319
Do you now have separate plus and minus supplies referenced to ground?

#### OBW0549

Joined Mar 2, 2015
3,566
I changed the OP amp into LM381 which equivalent to CA3130 which have 15MHz gain bandwidth, produced this result
Whats the problem?
Post your updated schematic so we can see it.

There are two other possible problems with your circuit and the simulation that haven't been brought up yet.

First, you've configured the amplifier in your Wien bridge oscillator to have a gain of 3 (set by R3 and R4). While this is theoretically correct, in an actual circuit or in a simulation that gain might not be quite sufficient to initiate and sustain oscillation. Try making the gain slightly greater than 3, for example by increasing R4 to 2.2 kΩ or 2.5 kΩ.

Second, oscillator circuits often fail to start up in Spice-based simulators because once Spice determines the circuit's bias point (always the first step in the simulation process), there is nothing to "kick start" the oscillator into oscillating. In real-world circuits, the noise that's naturally present in semiconductor components and resistors is what gets the oscillation started. In Spice, there is no noise. If this is happening, you can fix it by making your power supply voltage sources start out at 0V and ramp them up to their final value over a couple of microseconds (by using a PWL clause in the voltage source statement).

In any case, post your updated schematic.

#### Vincent Ng

Joined Dec 7, 2015
6

Yeah , i have changed it, and changed the R3 and R4 ,
the result is still same
Second, oscillator circuits often fail to start up in Spice-based simulators because once Spice determines the circuit's bias point (always the first step in the simulation process), there is nothing to "kick start" the oscillator into oscillating. In real-world circuits, the noise that's naturally present in semiconductor components and resistors is what gets the oscillation started. In Spice, there is no noise. If this is happening, you can fix it by making your power supply voltage sources start out at 0V and ramp them up to their final value over a couple of microseconds (by using a PWL clause in the voltage source statement)
I dont quite understand about the second statement, have any tutorial for it?

#### WBahn

Joined Mar 31, 2012
26,398
Is this homework? If so, I can move it to Homework Help.

Your simulations look like they aren't sampling enough (either for the simulator or for the display of the result -- one or the other). Circuits don't behave like the short line segments, so you are missing a lot of what is going on. Try reducing your timestep (or print step) by at least a factor of ten and see what that does.

#### OBW0549

Joined Mar 2, 2015
3,566
I dont quite understand about the second statement, have any tutorial for it?
Sorry, I don't. The User Manual for your simulator should show you how to specify time-dependent voltage sources (SIN, PULSE, PWL, etc.). I don't use Proteus or OrCAD, so I can't give you the details.

#### Alec_t

Joined Sep 17, 2013
12,319
With such low values for R1 and R2 and such high values for C1 and C2 the opamp is struggling to provide enough current. Try decreasing the cap values and increasing the resistor values, e.g by a factor of 1000 or so.

#### Danko

Joined Nov 22, 2017
1,187
Hello guys, I need some help with the Wien bridge oscillator which I need to generate 150kHz Sine waveform.
According to theory the wien bridge oscillator just need the RC to be work
but when simulated in proteus, the waveform doesnt come out,
I changed to OrcaD, instead the result become like attached, the oscilation become weaker and weaker with triangular like waveform
I check your schematic in Multisim - works good. Changed one resistor value only.

#### Danko

Joined Nov 22, 2017
1,187
For frequency 150 kHz change R1, R2 value 2.2 Ohm with 2.2 kOhm
and change R5 value 1 kOhm with 2 kOhm (parts numeration in my schematic).

#### Bordodynov

Joined May 20, 2015
2,939
See R=220 and C=470pF

#### Danko

Joined Nov 22, 2017
1,187
See R=220 and C=470pF
Good.
Frequency f (Hz) = 1,000,000,000,000 / {2Pi * R(Ohm) * C(pF)} , then
if 220 Ohm and 470 pF, we have 1,539,997 Hz, and I see it on simulator.
Maybe 220 Ohm and 4700 pF ?

#### Bordodynov

Joined May 20, 2015
2,939
I would advise you to use 2.2KΩ and 470pF.

#### Danko

Joined Nov 22, 2017
1,187
I would advise you to use 2.2KΩ and 470pF.
Yes, it will 10 times reduce load at the opamp's output than 220 and 4700.