# LTSpice, Current is not the same after going through identical step up and down transformers

I'm modeling my transformers as coupled inductors with appropriate values. I'm stepping up the current from my generator and then stepping it down at the load with identical inductor values (just flipped to represent step down vs step up). Since the turns ratios are identical the current should be the same on the generator side as it is on the load side. But when I am simulating it, my load current has an amplitude of 136ish A versus the generators current of 193ishA. Why aren't they the same?

The isolated center part of your circuit is not loss-free. You have resistor elements R1G, Rline and R1M in that circuit. That means that the voltage across L3M is not the same as across L3G. Another way of looking at it is that these resistors consume power, so the power reaching the primary of the second transformer is not equal to the power exiting the secondary of the first transformer.

You have a bunch of series elements between the two transformers. The load current that passes through these components drops voltage and therefore, your voltage on the load has to drop.

It's the same for the primary winding on the left transformer and the secondary winding of your right-hand transformer - series components drop voltage.

Since the turns ratios are identical the current should be the same on the generator side as it is on the load side.

But, you have also to consider the magnetization current into the left hand transformer - this is present whether you have a load connected or not - did you factor this into your analysis anywhere?

It looks like your left-hand primary inductance is 22.5 mH and this has an impedance of 8.48 ohms at 60 Hz. With 604 V peak voltage applied (if I read your numbers correctly), that's an RMS of 427 volts and, a magnetization current of just over 50 amps - this does not flow to the load.

And your right hand transformer also has magnetization current.

• That makes sense! My goal was to produce a specific voltage at the load and I calculated the current needed for that (163 amps). I referred all my impedance to the right side and used the referred impedance to calculate the voltage my generator would need to produce. I didn't account for magnetization current in my analysis which could be why my load current still isn't as I designed it. Is there a way to disable that in ltspice?