Clarence_A wrote...
Does anyone have a web reference to a spice model of a current
transformer or a site where creating such a model is
discussed?
Current transformers have the same linear spice model as other
kinds of common transformers, with DC winding resistances, the
turns ratio, leakage inductance, magnetizing inductance, etc.
. ---Rp---, ,---+--Rs--###----
. | | | Lell
. #||# #
. #||# # Lm
. turns #||# #
. ratio | | |
. -------' '---+----------
Not all of these parameters play a significant role, e.g. the
magnetizing-inductance component may not be significant, and
it's not a linear parameter anyway. You can assume Rp = 0.
A wideband transformer (>10MHz) may also suffer from winding
capacitance and ac copper losses, but you can ignore them.
Generally the primary is a single turn, from the wire being
measured going through the core. So the turns ratio N is
the number of secondary turns. You can measure or calculate
Lm = A_L N^2 for the secondary inductance in the spice model
and divide that by N^2 for the primary inductance, thereby
setting up the turns ratio for spice (isn't that awkward?).
The leakage inductance Lell is important; it's easily measured
by shorting the transformer, showing as k = sqr[Lm/(Lm+Lell)]
in the classic spice model, but I prefer to leave k = 1 and
add external inductances for Lm and Lell, so their presence
and effect is more clear in the drawing.
When you use a current transformer the load resistance is a
critical item. It's transformed down by N^2 to an effective
series resistance to the circuit being monitored, so you want
to use a relatively low load resistance. The low frequency
limit occurs when Lm shorts out the load, the high frequency
limit when the Lell reactance equals the load.