Deriving transfer function for effect of \$f_T\$ on BJT CE amplifier
\$\beta\$ is function of frequency; as well as temperature, \$I_c\$, and \$V_{\text{ce}}\$. A Laplace expression for \$\beta\$ would be: 

\$\beta (s)\$ = \$\frac{\beta}{\frac{s \beta}{2 \pi  f_T}+1}\$ 

In the development of the linked previous question, that's already rolled into the equations. 

Collector voltage for the circuit is: 

\$V_c\$ = \$-\frac{2 \pi  \beta  f_T V_{\text{in}} R_{\text{load}}}{2 \pi  f_T \left(r_b+(\beta +1) \left(r_e+R_e\right)+R_s\right)+s \beta  \left(r_b+r_e+R_s+R_e\right)}\$ 

This includes both the gain term \$A_o\$ and \$\beta\$ pole frequency term. Of course, after dividing by \$V_{\text{in}}\$, the transfer function remains. I think I left that step out earlier, but it's all nodal analysis and algebra. 

The T model of the BJT is used here. The T model seems to better match the kind of data supported in datasheets than the Hybrid-Pi. Added to the T model though is \$r_b\$, which isn't standard, but becomes important at higher frequencies. Usually in a datasheet, you'll find \$\beta\$, \$f_T\$, and (maybe) \$C_{\text{ob}}\$ (which is almost \$C_{\text{cb}}\$). These all map directly into the T model. If the Hybrid-Pi model is used, there's more work to do to get from \$\beta\$ to \$g_m\$. 



I seem to have the opposite view of simulation than Andy. Getting simulation results from SPICE or any other numerical simulator can lead to too easy acceptance of results and models. An answer is gotten, but causes and fundamentals of behavior can be obscured. It's too easy to think something is known when it is not. Trends are hard to spot. 

Using a simple analytical model makes it more clear where the model is worthwhile and where it's not. With the analytical model you can look at how the parameters interact. Add parameters one a time, see how orthogonal they are. Find out what dominates in which regions of interest. It's an effective way to learn fundamentals and how to design. It's really hard to do this with a numerical model like SPICE.

Still, SPICE can be a useful tool. Someone using it should get to really understand it though. Here's a guideline for SPICE use: 


Make test circuits to measure part model parameters, for comparison to the datasheet. This would be just for the part models, and doesn't include whatever circuit you are interested in. Especially do this if it's a canned model from a manufacturer. Do this consistently, and I think you'll be surprised at what you find. 
Read "Semiconductor Device Modeling" by Massobrio and Antognetti, and have it near at hand whenever using SPICE. 
Maximize AC analysis. Minimize Transient analysis. Fast AC modelling and thinking will work out better than slow transient based models most of the time. 
Transient analysis. Sometimes you have to use it, but be careful because its errors are many and subtle.