simulating equations in LTSPICE
If I get it right, you have a sensor in your project that acts as a current source generating a current proportional to a measured pressure squared and you want to simulate this sensor in the circuitry with the purpose of being able to perform, for example, a parametric DC sweep analysis sort of 'the instrumentation circuit output versus measured pressure'. If this is the case, you need a behavioral current source (symbol name BI**) of the LTSpice component registry.
To give you an idea of behavioral modeling, I show you a circuit that you can simulate in the online CircuitLab simulator on this page.



simulate this circuit &ndash; Schematic created using CircuitLab
You press the button Simulate this circuit and, in Simulation panel, select DC Sweep. The parameter to sweep is an ext_P voltage source voltage, which represents in our simulation a pressure to be measured. We imply that volt units of this parameter correspond to pressure units -- millibars, for example. The component MUL1 squares this parameter, and the MUL1 output is fed to a dependent current course VCCS1. The subcircuit of these three components, ext_P, MUL1, and VCCS1, is a model of your pressure gauge. The output current sourced is measured at a terminal of VCCS1 or of an ammeter.
You select start and end parameter values (e.g., 0 and 5), a step value (0.1), and press Run DC Sweep. The results of simulation is plotted to a graph window.

Using a behavioral current source, you can construct an LTSpice simulation in a similar way. With LTSpice, you need not compose a subcircuit of three components ext_P, MUL1, and VCCS1 as I did with the online simulator. Your pressure gauge will be modeled in your circuit with a behavioral current source BI with a duly selected parameters.
Among these 'duly selected parameters', of course, is a function-expression, 'I=[expression]', like in

BI1 n1 n2 I=square(ext_P)

According to B sources (complete reference), square(x) is an undocumented function; if you have doubts about using undocumented functions, you can use a documented power function pow(x,y)

BI1 n1 n2 I=pow(ext_P, 2)