LTspice: behavioral modelling elements for propagation delay
What you have there is not exactly an AND, because if the inputs don't have logical levels of [0:1], you're in trouble. And that syntax is not SPICE friendly, so it must be some proprietary way of defining a delay.
For an agnostic model you could use a behavioural source and a transmission line with:
B1 0 1 I = V(a) &amp; V(b)
T1 1 0 out 0 Td={td} Z0=1
R1 out 0 1

where I used &amp; for the logical AND. IIRC, ngspice uses &amp;&amp;, others may have their notations, as well, but the behavioural source shoud be SPICE compatible. If not, at the expense of manually setting the output levels, you could use:
I = Vlow + (Vhigh - Vlow) * ( ( u(V(a) - (Vhigh + Vlow) / 2) ) * (u(v(b) - (Vhigh + Vlow) / 2 ) ) )

I think u() is SPICE compatible. I've also avoided the use of the builtin delay() (or absdelay()) because 1) it might be particular to LTspice (or only a few), and 2) the tline is SPICE compatible (and better behaved for fixed delays). The output resistance can be changed to have other values, in which case the expression in the current source would have to be changed to (&lt;expression&gt;)/R and the transmission line's impedance to Z0={R}.
Otherwise, if you can tolerate an LTspice-only solution, I would highly recommend the builtin A-device [Digital]/and with td={td} (you may also want to use tau and tripdt, or vhigh, vlow, etc, see more in the help).