How to Model a Transformer in LTSpice

Question

I am modeling a low voltage single phase electrical distribution system with a step-down transformer using LTSpice (source is 480Vrms step down to 120Vrms). In LTSpice instead of setting the turns ratio, the inductance of the primary and secondary winding is set. However, I cannot find inductance values in low voltage transformer datasheets, and the results of my simulation seem to depend on the actual value of each winding, not only on the ratio.

For example, if I set \$L1=16\mu H\$ and \$L2=1\mu H\$ I get the following result for the current through R5 and R4 but if I set \$L1=16 H\$ and \$L2=1 H\$ I get the following result for the current through R5 and R4 It makes sense that the magnitude of the current will be different since different L values produce different impedances, so what is the best strategy to model this step-down transformer? Thanks.

Answer 1

So what is the best strategy to model this step-down transformer?

You have to find something in the data sheet that tells you about the no-load primary current (aka magnetization current). Then you calculate what the primary inductance will be for the voltage stated. It is going to be henries and not micro henries so your 2nd graph appears more reasonable.

Secondary inductance is smaller than primary inductance by turns ratio squared.

Answer 2

I am modeling a low voltage single phase electrical distribution system with a step-down transformer using LTSpice (source is 480Vrms step down to 120Vrms). In LTSpice instead of setting the turns ratio, the inductance of the primary and secondary winding is set. However, I cannot find inductance values in low voltage transformer datasheets, and the results of my simulation seem to depend on the actual value of each winding, not only on the ratio.

Inductance is a good start but not enough for completely modeling a transformer. There are other things to consider such as:

Core Material

Transformer cores are typically made from a ferrous material, but this creates problems for modeling because its nonlinear in that it has hysteresis and saturates. LT spice does have a non linear model, but the problem is still relating it to physical parameters. The Jiles Atherton Model is useful for modeling these effects.

Source: Qoura

Leakage and Mutual Inductance

Because only part of the magnetic field from one coil flows through the other coil, leakage needs to be accounted for in the model, as shown below in the inductors \$ L_{LP} \text{ and } L_{LS}\$ the mutual inductance is the one below. These can be simulated in LT spice.

Source: Power Electronics: Efficiency in Power conversion circuits

Wire Resistance and capacitance

The parasitic resistance of the winding needs to be accounted for, this can be approximated by measuring with an ohm meter. The wire resistance can be modeled as a resistor in parallel with the inductor. There also exists parallel capacitance between all of the winding, which can be modeled as a resistor in parallel. with the transformer inductance. Both the parasitic capacitance and resistance help determine the bandwidth of the transformer. Sometimes you can get an idea of the paraisitcs of the transformer if an impedance vs frequency chart is given.

Source: IRF

Most of these parameters will need to be modeled yourself. The method I used to find inductance is found here. Before simulating one needs to decide which parameters need to be modeled and what level of accuracy the simulation needs to achieve. Because these parameters are typically not available measuring the transformer becomes a necessity.

In most cases the least time consuming thing would be to either use designs that have already been fabricated and tested (Example: by using the DC to DC IC's recommendations which have already been tested). Or by building the circuit and testing it yourself.

If simulation is desired, then a way to reduce time is to find manufacturers of transformers that already have spice models available. There have been a few tools I've seen that can take parameters and generate a spice model, but the physical nature of the transformer (such as wires size and turns ratio) need to be known.

Answer 3

Impedance ratio of the transformer is square of turns ratio. Then there's also the coupling factor of the transformer. With '1' you model an ideal transformer without stray fields, or magnetic losses.

Try the transformer impedance at second side at 1mH and calculate primary impedance by turns ratio. Then multiply both impedance by 100 and you'll notice no change in currents.