Offset problem in simulating current and voltage phase relation of parallel rlc circuit, Is it a bug ?

[bangkaew]

 tested multisim for Parallel RLC Circuit with voltage source as in 
http://www.electronics-tutorials.ws/accircuits/parallel-circuit.html

But the current flows through the inductance L has DC component as in the picture attached (the red sine wave).  Is it  a bug ?, please tell me how to correct it.

[bangkaew]

It may be difficult to use Multisim to illustrate and explain the phase relation of RLC  circuit in parallel in the same way as what many people  usually do without no offset as in , 

Anyway, Multisim is perfect for   RLC  circuit in series as in the  photo attached.

What is wrong ?  should it be corrected to make it consistent with what most people think. ?.

[Tien_P]

In Multisim select menu Options>>Global Preferences>>Simulation,  under "Positive phase shift direction" change the phase shift setting and then press Apply and OK.  Double click on your AC source on the schematic and verify the phase shift is correct and simulate your circuit again, this will likely fix the simulation error.

[Tien_P]

a

[bangkaew]

Thanks, Tiens

I tried it ,but to no effect.

The problem is not the phase shift , but the magnitude which contain offset or DC component in the current flowing through ideal inductance.

I attached the file for your testing.

[yyao]

Hi there,

As strange as this may sound, this is not a bug. OK, this sounds really funny, but I am totally serious, and I am going to explain why:

1. In a circuit energy must be conserved.
2. An inductor is a purely reactive component, that is, it does not dissipate any power.
3. When simulation starts, Multisim assumes the inductor current to be 0, which may seem reasonable. The voltage across the inductor is also 0 at this point. This is the initial condition.
4. The voltage across the inductor increases, and thus, the current increases. The current keeps increasing during the first 2 quadrants of the sinusoidal phase output.
5. The current never decreases until the voltage drop is negative.
6. But by the time an entire cycle is over, the current is back to 0. This makes sense as energy is conserved and the inductor is not absorbing any energy.

OK. Now look at what happened. During the whole cycle, the current was positive only! The current increased during the first half of the cycle and returned to 0 during the second half. This is because of the fluke of initial conditions! In fact, a good circuit simulator will maintain the DC offset for a long duration. The DC offset may drift because of rounding errors and the like.

This will never be observed in real life as real inductors have winding resistance and other problems.

OK, so, if you would like to see no DC offset, do the following:

1. Run your simulation
2. Record the DC offset that you want to eliminate
3. Stop your simulation
4. Double click the offending inductor in the Multisim schematic
5. Click on the Value tab
6. Check the Initial conditions box under Additional SPICE simulation parameters
7. Enter the negative of the DC offset that you recorded in step 2 into the box right next to it
8. Start your simulation. Did your offset go away? Or did it double?
9. If your offset doubled, take away the sign from the DC offset that you entered in step 7. I bet you know why.

It took me a while to figure this one out. Hope that helps!

[bangkaew]

Thanks, Yi

I have tried what you said, but to no effect.(nothing changes, the phasor diagram tool shows the same offset) 

and I don't think this is a good solution.

When I changed from voltage source to current source, the offset disappears.

Is it possible that current and voltage phase relation of inductor is derived from current as input and voltage drop as output, when you reverse the cause and effect , the result may not be the same.

So, when pure inductor is found directly connected to a voltage source, Multisim should perform some procedure to maintain a steady state value with no offset. I think.

[yyao]

I'm attaching your original file that has been modified to have no DC offset in the inductor.

I don't have your phasor VI, so I substituted an ordinary 4 channel oscilloscope. You can replace it with a phasor VI again and it should work fine.

[bangkaew]

Thanks, Yyao

Your file can not be download or opened.

I have tried what you said by connecting to 4 channel oscilloscope as attached , but to no effect.(nothing changes, the signal  shows the same offset as the green sine wave) 

[digitalguy]

FYI, the file opens and works perfectly for me. I have Multisim 11.

Howard