Uncertain on the results of coupled inductor simulation with initial values

marcel hendrix — Thu, 23 Apr 2026 20:01:29 -0000

A 5th order integration method (like PLECS is using) needs 4 initial derivatives in addition to the initial value itself. IIRC, SPICE does a number of steps (with a low order integrator) to approximate these derivatives. This approximation will be inaccurate, and anyway there is no guarantee that the values are what the user intended. However, I think it reasonable to expect that SPICE-based simulators will show the same result. With SIMPWL I know for sure that it does not need unknown derivatives. However, PLECS, like SIMPWL, claims to be state-space based but gives a wildly different result.

The circuit has indeed additional problems: there is a cutset of currents, one of the 3 inductor currents is dependent on the others. I don't think a SPICE simulator will invest the time to find out which is the dependent and which are the independent variables, and modify the matrices so that the initial values line up with the independents (if it is possible with MNA at all).

The example is indeed contrived (unless we are building an HV generator) but I like to know the limits of my tools.

Uncertain on the results of coupled inductor simulation with initial values

dick freebird — Thu, 23 Apr 2026 18:27:50 -0000

Might check that mutuals are sane. I have had trouble in
other simulators in other times, trying to do complex
couplings (without clue) and evidently there's some
stuff about making sure matrices are sparse and the
k values rolled up, still sub-unity (?).

I just gave up trying to model bond wire k couplings.
C, OK. L,OK.

Anyway, different simulators might respond to the
physically impossible in various ways. I'd dig there
first, "why?". Then maybe run a "settling" tran job
to get to a DC-stable or cyclic-stable IC that maybe
is more solvable (rather than NaN-precursor, like).

I don't think initial conditions which are jacked, make
any simulator's job easier. Maybe just provoke different
paths to failure.

Uncertain on the results of coupled inductor simulation with initial values

marcel hendrix — Wed, 22 Apr 2026 11:22:48 -0000

Thanks, Felix!

I'll ponder gnucap's documentation.
BTW, I tried OpenModelica and SIMBA (demo version) just now. Modelica is a monster that I can not make sense off. SIMBA gave an interesting result. The initial values are obeyed but neither the frequency nor the damping are correct.

Uncertain on the results of coupled inductor simulation with initial values

Felix — Wed, 22 Apr 2026 09:43:11 -0000

see http://gnucap.org/dokuwiki/doku.php/gnucap:manual:tech:spice2verilog?s[]=uic#algorithmic_peculiarities

tl;dr; The issue is somewhere between model specification and simulation algorithm. The way Spice implements UIC makes no physical sense in general (cf. the currents at time 0). Particularly, (spice, ngspice) UIC was not originally intended for the purpose shown here.

NB: Other simulators may do different things. Not rocket science, but at the cost of losing Spice compatibility.

Uncertain on the results of coupled inductor simulation with initial values

marcel hendrix — Tue, 21 Apr 2026 19:12:05 -0000

I am struggling with the simulation of a coupled inductor when initial values are specified.
By now I did the same simulation (see attachment) in NGSPICE, LTspice, PLECS, and SIMPWL, with four rather different outcomes.
The LTspice result is clearly completely wrong. It simply does not obey the IC=... specification when using .TRAN with the UIC option. At least the sum of the three inductor currents is 0, as it must be.
NGSPICE

Measure RMS current of inductor in SPICE

Hai Yang — Fri, 10 Apr 2026 19:59:23 -0000

Thank you for your response. Following is the result from SPICE,

Note: Compatibility modes selected: ps lt a

Circuit: 

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

Using SPARSE 1.3 as Direct Linear Solver
Operating point simulation skipped by 'uic',
  now using transient initial conditions.

Warning: command 'plot' is not available during batch simulation, ignored!
    You may use Gnuplot instead.

No. of Data Rows : 10011
irms                =  6.35351e+00 from=  1.00000e-08 to=  1.00000e-02
irms = 6.353514e+00

I got best result. You are great! Thank you again!

Measure RMS current of inductor in SPICE

Hai Yang — Fri, 10 Apr 2026 19:56:27 -0000

Thank you for your response. I am pretty new to SPICE. I am going to try UIC

Measure RMS current of inductor in SPICE

Hai Yang — Fri, 10 Apr 2026 19:45:56 -0000

Thank you for your response. You are genius. I modified my netlist, and increase the length to 4 second. The result get much better.

* Inductor RMS current measurement
V1 in 0 SIN(0 282.28 50)
R1 in n1 0.10
L1 n1 0 100mH

.tran 0.2ms 4000ms 1000ms

.control
run
meas tran Irms RMS i(L1) from=2000ms to=3000ms
print Irms
.endc
.end

Following is the result,

Note: Compatibility modes selected: ps lt a

Circuit: 

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

Using SPARSE 1.3 as Direct Linear Solver

Initial Transient Solution
--------------------------
Node                                   Voltage
----                                   -------
in                                           0
n1                                           0
l1#branch                                    0
v1#branch                                    0

No. of Data Rows : 15001
irms                =  6.40150e+00 from=  2.00000e+00 to=  3.00000e+00
irms = 6.401500e+00

You save me a lot of time. Thank you again!

Measure RMS current of inductor in SPICE

Hai Yang — Fri, 10 Apr 2026 19:38:48 -0000

Thank you for your response, For this circuit, the theorical calculation value is, 6.37A. The margin of error is too high. I modified my netlist, and got a better result from SPICE.

Measure RMS current of inductor in SPICE

Holger Vogt — Fri, 10 Apr 2026 16:20:06 -0000

Use initial conditions:

* Inductor RMS current measurement
V1 in 0 SIN(0 282.28 50)
R1 in n1 0.10
L1 n1 0 100mH ic=-9

.tran 10us 2 uic

.control
run
plot  i(L1)
meas tran Irms RMS i(L1)
print Irms
.endc
.end

Recent posts to Discussion

Uncertain on the results of coupled inductor simulation with initial values

Uncertain on the results of coupled inductor simulation with initial values

Uncertain on the results of coupled inductor simulation with initial values

Uncertain on the results of coupled inductor simulation with initial values

Uncertain on the results of coupled inductor simulation with initial values

Measure RMS current of inductor in SPICE

Measure RMS current of inductor in SPICE

Measure RMS current of inductor in SPICE

Measure RMS current of inductor in SPICE

Measure RMS current of inductor in SPICE