Your circuit can be simulated, for sure. But it will need some efforts.
In designing the circuit diagram, you have used KiCAD symbols. The simulation up to now has spitted a lot of error messages, most dealing with missing models.
To do a simulation, each symbol will need a Spice model. For resistors, this is included. For OpAmps and Sensors it is not. So you have to take care. For the OpAmp LM321 you might google for a suitable vendor’s Spice model. Then you have to add this model to your OpAmp symbol. Please have a look at http://ngspice.sourceforge.net/ngspice-eeschema.html#OpAmp how to do that. This tutorial will give you also some hints on establishing PSPICE compatibility, typically needed for using commercial OpAmp models. Concerning the power supply, better choose ngspice compatible symbols as you may find in the Simulation_Spice symbol library.
More difficult will be handling the sensor. There seems to be no Spice model available from the vendor. So you have to create one yourself. The reliable source available is the data sheet from Honeywell. You correctly have shown 3 electrical pins in your sensor symbol. But that’s not all. A sensor has another connection to the environment, the humidity entrance. Of course KiCAD and ngspice don’t have any notion of humidity nodes. But why not replace them by an electrical node, say a voltage input with 0V for 0% and 100V for 100% humidity? If you want to follow this idea (very common in sensor design), you have to add another pin (e.g. named ‘humidity’) to your symbol. The humidity then may be represented by a voltage source.
You definitely have to look at the data sheet. One point is that the power supply voltage is 5V. In your circuit with ±5V on the sensor, it probably would ‘explode’. The -VE should better be connected to 0V.
How to create a model? Unfortunately this will need some knowledge of ngspice netlists. As you (hopefully) have recognized, the OpAmp model is a subcircuit model. So you have to create a ngspice subcircuit description, put it into a file and then add it to your sensor symbol as you have done with the OpAmp. Inside of the subcrcuit we will need an (electrical) equivalent of the sensor’s behavior. This may be found by again looking at the data sheet. There you will find the output versus humidity equation, that is Vout=Vsupply*(0.0062*RH + 0.16). In ngspice there is a B source availabe that allows to describe such functions. The subcircuit starts with a title, then the .subckt line with subcircuit name and nodes, then the internal description, followed by the .ends line. I will give you a hint (not tested):
* HIH-4000 simple subcircuit model
.subckt HIH-4000 -VE OUT +VE RH
Bout OUT -VE V = (v(+VE) - v(-VE)) * (0.0062 * v(RH) + 0.16)
So node 1 is -VE, node 2 is OUT, node 3 is +VE, and node 4 is RH, the humidity input. If you firstly just put the sensor, an output resistor to ground and a voltage source as humidity input, you may do a .dc simulation to check if the sensor model is doing what the data sheet says. Then you may add your OpAmp circuit to obtain the final output between 0 and 1V.