Simulating in LTspice with LM1875
It's a bad model, full of behavioural conditionals and limit()s which bring discontinuities in the derivative. Many capacitors are directly connected across current sources which act as integrators, probably, or try to smooth out the discontinuities, but which have no parallel resistor to provide a DC path to ground. It's begging for "timestep too small" errors and outputs swinging to kV or more (which is what happens in my case).

There's also an unneeded .END at the end of the block of text which cancels any attempt to replace the faulty opamp with one from the internal database, with the error: unknown subcircuit .... The .END is a keyword that signifies the end of all the netlist. Anything added after it is simply discarded, for example adding an opamp causes the adjacent .lib call to fail, since it falls outside the scope of the netlist.

If you correct .END into an .ENDS, suitable for the end of a subcircuit definition, it complains about a stray .ENDS. Which means it's safe to be deleted.

The solution is to replace the opamp witn another, preferably a working one. Once you delete it and replace the faulty opamp, you'll see the simulation flying. For example, placing the first available opamp in LTspice's library, AD549, makes the simulation run. Three more random attempts, AD8565, LT1022, LT1369, all work (though the AD8565 is slower, the model might not be quite so well made). Your choice about what to do next.