problem to compute RC circuit in ngspice

[indigo33]

Hi,

I did the following analysis of a simple RC circuit in ngspice, it works fine.

V1 1 0 1
R1 1 2 100K
C1 2 0 10u
.ic V(1)=0 V(2)=0
.tran 0.2s 5s
.plot tran v(2,0)
.end

But, if I invert the order of R and C, the analysis starts with the capacitor already charge. Why? When components are in series, does the order matter?

V1 1 0 1
C1 1 2 10u
R1 2 0 100K
.ic V(1)=0 V(2)=0
.tran 0.2s 5s
.plot tran v(1,2)
.end

 

[h_vogt]

.tran 0.2s 5s uic
will force v(1) to 0, during the first time step it jumps to 1 as given by V1 1 0 1.

If not using uic, ngspice has to calculate an initial value with the contradictory inputs
V1 1 0 1 and
.ic V(1)=0
which leads to results depending on the circuit.

Even better would be not using just
V1 1 0 1, but
V1 1 0 1 pwl(0 0 0.2 0 0.205 1)
which will start with all zero and then pose a voltage jump with controlled slope at node 1.

Holger

 

[indigo33]

Thank you very much! It works perfectly now.