I am trying to simulate a RL circuit in DC with LT-spice as follows: enter image description here

NOTE that the inductance is 0.0229 H although in the picture you see 229

Now, according to my calculation, what I would expect is that, because of the inductor, the current needs some time, say 4.4 tau to be close to the theoretical value of V/R = 1.497 A.

Below you can find the data of the circuit:

Inductance (H): 0.0229

Resistance (Ohm): 3.34

DC voltage (V): 5

Current (A): 1.4970059880239521

Tau: 0.006856287425149701

Critical time (s): 0.03016766467065869

Now, when I simulate the circuit in LT-spice, this is not what happens, the current jumps up to 1.497 immediately, not showing the exponential behaviour it should have in a circuit like this. What am I doing wrong I checked and doublechecked but I cannot find out what I am missing! As you can see with LT-spice I looked very close to t=0 to check whether I was missing out on the timescale, but the current behaviour is not exponential at t = 0 + dt either!

From my calculation, the theoretical behaviour before 0.03s should be the following: enter image description here


You need to start the transient analysis at zero volts, else it will start at a steady state of 5VDC with the current already flowing.

Add the keyword 'startup' to the .tran string, or tick the box 'Start external DC supply voltages at 0V:' in the simulation command panel.

| improve this answer | |
  • \$\begingroup\$ It worked perfectly, thanks! What a silly mistake to make! \$\endgroup\$ – mickkk Jul 12 '15 at 9:49

Although the solution using the keyword 'startup' seems to work, I would recommend not to use the "startup" condition (unless it is explicitely desired to have the DC source also starting up from 0V).
It's better to use initial condition directive .ic i(L1)=0, so voltage source V1 is 5V at time = 0 seconds.

The "startup" option lets DC sources ramp from 0V to their final value in 20 microseconds. In OP's circuit and shown waveform, this effect will hardly be visible as the plot covers 60 milliseconds.

See also LTSpice: simulate transient voltage and current in RL-circuit

| improve this answer | |

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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