Second Order Circuit: Sim vs. Algebraic Solution

Discussion in 'Homework Help' started by mjakov, Jan 28, 2015.

  1. mjakov

    Thread Starter New Member

    Feb 13, 2014
    20
    5
    Dear forum experts!

    Please help explain the inconsistency between the algebraic solution and LTSpice simulation for a second order parallel circuit here. The parameters are:
     <br />
R=200 \Omega, L = 0.28H, C = 3.57 \mu F <br />

    [​IMG]

    The capacitor ought to have an initial voltage of 50V. Hence, I us the .ic command in the sim to set the initial voltage for the identifier n001. This identifier seems to correspond with the node above the capacitor.

    By calculating the circuit algebraically it can be shown that the RLC parameters result in an underdamped (oscillatory) case. The algebraic equation for the circuit is:
     v(t) = e^{-700t} * (50 cos (714t) - 49 sin (714t))
    Below you can see the plot of this equation until 10 ms.

    [​IMG]

    The image below shows the simulation. Besides some similarity in the curve shape, the values on the y-axis seem to be off by a factor of  10^6 .

    [​IMG]

    My assumption is that there is something wrong with the simulation, since the algebraic solution has been derived according to my textbook. Could someone please give a hint as to what could be wrong. Other circuits that I have simulated without the initial conditions seemed to be OK in LTSpice. Could it be that one should use the switch element in the sim, e.g., first to charge the capacitor with a source and then move a switch to a desired position?
     
  2. ericgibbs

    AAC Fanatic!

    Jan 29, 2010
    2,503
    380
    hi,
    Look at this version.
    Note the uic
    E
     
    mjakov likes this.
  3. MikeML

    AAC Fanatic!

    Oct 2, 2009
    5,450
    1,066
    Majkov,

    I believe LTSpice over your algebra...;) It did exactly what you told it to do...

    Eric showed you how to name a node in an LTSpice schematic, so that you can refer to its given name in the .IC V(name)= XX or plot statement.

    The use of the uic in the simulation directive forces the current in the inductor to be zero at time=0. Otherwise, the inductor current would be nearly infinite at time=0, which is what happened in your original sim, and you would have seen if you added the current through L1 to the plot as below...

    The better way to do this using a more complex .IC statement is shown below. The LTSpice help file strongly discourages ever using the uic directive. In a more complex circuit, it can lead to unpredictable results.

    132.gif
     
    Last edited: Jan 28, 2015
    mjakov likes this.
  4. ericgibbs

    AAC Fanatic!

    Jan 29, 2010
    2,503
    380
    Mike,
    The uic is still in common usage in many tutorials and examples, however I will look thru more documentation.

    Eric
    Query: have you edited your post since I last read it.:rolleyes:
     
  5. MikeML

    AAC Fanatic!

    Oct 2, 2009
    5,450
    1,066
    Yep. Here is the description of uic:

    uic.gif

    Here is .ic

    ic.gif
     
    Last edited: Jan 28, 2015
  6. ericgibbs

    AAC Fanatic!

    Jan 29, 2010
    2,503
    380
    OK.
    I have already read the LTS Help folder, ref the UIC and I do use the UIC option with caution.
     
Loading...