Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free.

Sign up
Here's how it works:
  1. Anybody can ask a question
  2. Anybody can answer
  3. The best answers are voted up and rise to the top

My question is specifically linked to an exam problem where I had to find a function in terms of time for the current on a capacitor and a resistor. The circuit was very simple: A current time-variant current source in series with 2 subcircuits, each composed of a capacitor and a resistor connected in parallel. Please see the figure below:


So, if I want to simulate this circuit with a SPICE software, should I run a transient analysis, a DC linear analysis, or some other type of analysis?

If the current source was sinusoidal, I would use an AC analysis, but the current source runs a current numerically equivalent to t (in Amperes) where t is the time (in seconds) elapsed since the circuit started working.

Below I have written my netlist file. While it is not a valid SPICE netlist, it illustrates what I am trying to do, focus on the current source Iin:

C2 0 2 20m
R2 0 2 3
Iin 0 1 {time}
R1 1 2 2
C1 1 2 50m

.TRAN 1us 100ms
PLOT V(1)-V(2)


If you tried to simulate this netlist, you would receive an error similar to the following (which I obtained using ngspice):

Original line no.: 4, new internal line no.: 5:
Undefined number [TIME]
Original line no.: 4, new internal line no.: 5:
Cannot compute substitute
 Copies=9 Evals=9 Placeholders=1 Symbols=0 Errors=2

How can I achieve this type of analysis?

share|improve this question
up vote 4 down vote accepted

DC analysis gives you the initial conditions DC steady state values only. You must do a transient analysis to see how the voltages and currents evolve with time. AC analysis is for small-signal sinusoidal steady state only; it is a frequency domain analysis.

I believe you'll need to use a piece-wise linear (PWL) source for your current ramp.

share|improve this answer
The initial conditions could be anything you or the simulator wants. So wouldn't DC be the steady state values? – Kellenjb Jul 12 '12 at 19:49
You're correct, and I don't know why I wrote that. The DC solution is, of course, the final state after all transients have decayed. Doh! – Alfred Centauri Jul 12 '12 at 19:51
Great! The PWL analysis let me do exactly what I was planing. And yes, from what I noticed the DC linear analysis seems to plot the final state of the circuit in each point. – Severo Raz Jul 12 '12 at 21:40

Based on your description of the exam problem, I think a transient analysis is still what you're looking for. In CircuitLab you can just define the current source as having current "T" to generate a linear current ramp proportional to the simulation time: (click here for circuit and simulation)

current ramp

Open and run the transient simulation:

current ramp plot

You can also examine the currents into each element. As you might expect, the currents into C1 and C2 are constant, while the currents into R1 and R2 grow linearly with time.

As far as the ngspice/netlist question, I believe the keywords to be looking for are "behavioral sources". See this page for some examples (one near the end uses TIME as a variable).

share|improve this answer
Hm, sadly ngspice isn't able to run that example using TIME as a parameter. I get the same error I included in my question, it is very unfortunate. – Severo Raz Jul 12 '12 at 21:36
And I almost forgot, thanks for showing me CircuitLab! I might use it in the future. – Severo Raz Jul 12 '12 at 21:38

You would be best to use a transient analysis. Rather than using the time parameter you could setup the current source with the pulse attribute, then specify the rise/fall time accordingly if using a standard current source (Ix). Or use an arbitrary source (Bx) and express the signal mathematically using time as a parameter.

For example, here is the netlist for your circuit in LTSPice using an arbitrarily behavioural current source:

* C:\Program Files\LTC\LTspiceIV\current rc.asc
R1 N002 N001 2
C1 N002 N001 50mF
R2 N002 0 3
C2 N002 0 20mF
B1 0 N001 I=time
.tran 0 15 1m uic

Here is the simulation with V1 - V2 plotted:


share|improve this answer
Isn't B a refdes for a transistor type? – Severo Raz Jul 12 '12 at 21:33
Well, after doing some tweaks to the netlist you provided, I was able to use it successfully, it seems that the .backanno command and the .tran syntax vary between LTSpice and ngspice. I would mark your solution as answer as well but I have already accepted one answer :/ – Severo Raz Jul 12 '12 at 21:48

Your Answer


By posting your answer, you agree to the privacy policy and terms of service.

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