Here are two circuits I've simulated. Both have a current source of \$\sin(\omega t)\$ mA with \$\omega=1000\$. They should be equivalent but give different simulation results.

enter image description here

Here are the simulated currents across R1:

I(R1):   mag:  0.0672338 phase:   -137.752°  device_current
I(R1):   mag:  0.0673282 phase:   -137.783°  device_current

Here is how I calculated the new R2 and L1: The total complex impedance of R2 and L1 in parallel is \$1/( 1/R_2 + 1/(j\omega L_1)) = 1/(1+1/j) = 0.5 + 0.5j\$ which can be written as the series resistance and inductance \$0.5+j\omega \times 0.5\times10^{-3}\$.

So my question is: where did this calculation go wrong? Are the circuits not equivalent or have I missed something in the simulation?

I don't think this is a numerical error since the current is wrong in the third significant digit whereas the model should be accurate to the floating-point precision.

  • \$\begingroup\$ I ran a simulation in qucs and it seems the circuits do perform identically. So the issue appears to be in the simulation, but I am not sure where. Are you sure you are using ideal components? \$\endgroup\$ Nov 11, 2013 at 19:13
  • \$\begingroup\$ @alex.forencich I just double-checked and it seems so. Weird. I'm using LTspice IV. \$\endgroup\$
    – Anna
    Nov 11, 2013 at 19:17
  • \$\begingroup\$ Actually, after switching from voltage sources to current sources, I get 0.0672671 at -137.7261 deg for the first circuit and 0.06726708 at -137.7265 deg for the second circuit. So closer than for LTspice, but not the same. My guess is it has to do with how the simulator carries out its calculation. \$\endgroup\$ Nov 11, 2013 at 19:30

2 Answers 2


The problem arises from the 1mohm that's in series with the inductor:

Inductor Properties

When I calculated the current through R1 with the extra 1mohm added my calculations line up perfectly with the simulation results. Alternatively, you can force the series resistance to be 0. Doing this also gave me equivalent results for both circuits from LTSPICE.


These circuits are not equivalent.

You can see this just by looking at the impedance of the L1 R2 combination in the limit as frequency goes to dc.

For the first circuit, the impedance goes to zero. For the second circuit it goes to 0.5 Ohms.

where did this calculation go wrong?

When you wrote,

\$ \dfrac{1}{1/R_2 + 1/(j\omega{}L)} = \dfrac{1}{1+1/j}\$,

you dropped the \$\omega\$.

  • \$\begingroup\$ Sorry -- I meant equivalent at the given frequency. The current source gives sin(1000t) mA. \$\endgroup\$
    – Anna
    Nov 11, 2013 at 19:02
  • \$\begingroup\$ I abbreviated the calculation a bit, sorry about the confusion. Since L=1mH and \$\omega=1000\$ rad/s, \$L\omega=1\$ (omitting the units). \$\endgroup\$
    – Anna
    Nov 11, 2013 at 19:04
  • \$\begingroup\$ In that case, I'll agree with the other comments and guess it's just a round-off error in the calculations. \$\endgroup\$
    – The Photon
    Nov 11, 2013 at 19:33

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.