How to find the output and input impedance of an amplifier
Since you have already entered the schematic into LTSpice, the easiest way is to use the simulator. For each port (here you have two ports, input and output) that you care about, 


Add a load termination on the other port representing how it will be used in a bigger circuit.
Add an AC current source to the port you are testing. Give this source an amplitude of "1".
Add a net name to the net at the port you are testing (for example "VIN" or "VOUT").
Run an AC simulation over the frequency range you are interested in.
Plot the voltage at the port you are testing. 


Because your AC source has a value of 1, the voltage you plot is equal (at 1 ohm per volt) to the equivalent input/output impedance at that port. Never mind that in reality a 1 A current source would drive your circuit into all kinds of nonlinear behavior. A SPICE AC simulation uses a strictly linearized version of the circuit and won't include any nonlinear behavior.

Note that this method works even if you don't approximate the capacitors with wires. In fact, if you don't, it will let you see the effect those capacitors have on the in/output impedance at frequencies below where they are well-approximated by wires.

Second, if you have simulator models for the transistors, you don't even have to reduce the transistors to their ac-equivalent model. The simulator will do this for you. It will also include parasitic capacitances in the transistor so that you know whether the transistor has adequate response at the frequencies you're using for the simple model to be accurate.