Simulating Power PMOS using LTSpice
To model the P-MOS transistor in LTspice you do not need to know the \$W\$ and \$L\$. 

The simples model used the \$K\$ factor and \$V_{TH}\$. 

The drain currency is equal to: 

$$I_D = \frac{K}{2}(V_{GS} - V_{TH})^2$$   

And using the datascheetplot, we can also find \$V_{TH}\$ using this equation: 

$$V_{TH} = \frac {V_{GS1} \sqrt{I_{D2}} -V_{GS2} \sqrt{I_{D1}}}{\sqrt{I_{D2}} - \sqrt{I_{D1}}} $$   

And \$K\$ factor: 

$$K=\left ( \frac{\sqrt{2I_{D1}}-\sqrt{2I_{D2}}}{V_{GS1} - V_{GS2}} \right )^2$$

For example, if we used the datasheet http://www.irf.com/product-info/datasheets/data/irf9z24n.pdf 

We can use this plot: 

 

And find that: 

\$I_{D1} = 2A\$ and \$ V_{GS1} = 4.8V\$

\$I_{D2} = 4A\$ and \$ V_{GS2} = 5.5V\$

We have \$V_TH = -3.11V\$ and \$K = 1.4 \$

And finally, in LTSpice we can use this statement: 


  .model p1 PMOS (LEVEL=2 KP=1.4 VTO=-3.11)




But most of the time we can find a spice model of a MOSFET on google.