Dependent voltage source simulated in my schematic LTSpice not work?
You can see something is not right because I(R1) is reported as non-zero, but I(B2) is 0.
From the LTSpice Help file on the expression syntax for the &quot;B&quot; element:

Expressions can contain the following:
o ...
o Circuit element currents; for example, I(S1), the current through switch S1 or Ib(Q1), the base current of Q1. However, it is assumed that the circuit element current is varying quasi-statically, that is, there is no instantaneous feedback between the current through the referenced device and the behavioral source output. Similarly, any ac component of such a device current is assumed to be zero in a small signal linear .AC analysis.

So it seems the &quot;B&quot; element (arbitrary controlled voltage or current source) is not much use (except possibly to set up the operating point) in an AC analysis. This makes some sense, because a nonlinear element would produce harmonic output that can't be accounted for in an AC analysis.
Since your relationship is linear, you can use the &quot;F&quot; element, a linear current-controlled current source, instead.