Cannot simulate coupled inductors

Schematic Simulation (Ngspice)
1

I am playing around with KiCad 7.0.10-ubuntu22.04.1 and I am trying to use the L_Coupled component.

My schematic is very simple:

image
image1411×417 17.6 KB

I then try to simulate the transient behavior of the circuit. Inspect > Simulator > Sim Command

No matter what I try I still get this error “Error reading simulation model from symbol ‘L1’: failed to read simulation model from fields”

I can sim basic components, including inductors.

One thing I tried was to edit the device propertied > simulation model. After clicking thru the same error as above twice, I can try to use a built in spice model; ie inductor + mutual. after setting the desired params I try to simulate and get the console error

Note: Compatibility modes selected: ps lt a
Circuit: KiCad schematic
Error on line 5 or its substitute:
kl1 __l1 1m 1m 0.5
unknown parameter (0.5) 
Error: circuit not parsed.

The SPICE netlist is:

.title KiCad schematic
.save all
.probe alli
.tran 1u 10m
KL1 __L1 1m 1m 0.5
V1 Net-_L1-Pad1_ 0 DC 0 SIN( 0 1 1k 0 0 0 1 ) AC 1 
R1 Net-_L1-Pad3_ 0 1k
.end

which i know is garbage. I have an idea of what I should be seeing from this thread but I am not sure what buttons are where.

2

There are at least two ways to simulate a coupled pair of inductors.

The simple one: place 2 separate inductors, say L1 and L2, into the circuit and wire them appropriately (check their polarity). Then place a coupling statement
K1 L1 L2 0.98
in a text box on the Eeschema canvas.
For achieving convergence you may need to add a small series resistance to each coil. Or put a staement
.options Rseries=1m
in a text box on the Eeschema canvas (which adds this series resistance to all coils in the circuit).

The more complex one, using the symbol L_Coupled: L_Coupled is just a symbol with 4 pins, a drawn template definitely without any ngspice model. In fact you may use any symbol with 4 pins for the following.

You have to create a ngspice model. This cannot be a .model line, as there is no intrinsic coupled L model available in ngspice. Thus you have to create a subcircuit model.

The subcircuit frame is

* model for a simple transformer
.subckt Couple2Ls n1 n2 n3 n4
.ends

with Couple2Ls being the name of the subcircuit, n1 to n4 the four nodes (arbitrary names for the nodes may be given).

What is inside of the subcircuit?
First of all we have the 2 inductors and their coupling statement. However, we also should put some sries resistance to each coil, as this is required when just connecting a voltage source to any inductor.

* model for a simple transformer (series resistance still missing)
.subckt Couple2Ls n1 n2 n3 n4
Ls1 n1 n2 10m
Ls2 n3 n4 5m
Ks1 Ls1 Ls2 0.99
.ends

Now with series resistance:

* model for a simple transformer
.subckt Couple2Ls n1 n2 n3 n4
R1 n1 nint1 1m
Ls1 nint1 n2 10m
R2 n3 nint3 1m
Ls2 nint3 n4 5m
Ks1 Ls1 Ls2 0.99
.ends

You may add the correct values for the inductances, sheet resistances and coupling constant. Put this subcircuit model into a file, save it to your project folder. Then attach the model to the symbol in the usual way. The pin order has already been taken into account by the pin sequence in the .subckt line.

3

Between V7 and V8 there were some important work on Spice in KiCad, I think.
I’m not using Spice (I have only once tried in V7 and then in V8) so I can’t list these changes, but probably if you want to use Spice it is worth of installing V8.

4

I fired up a latest ubuntu vm with version 8 and was able to replicate the issue

Thank you so much for the in-depth response! Adding the coupling to a text box was the simplest and worked for me!