## Step 4: Solve!

Before solving, we need to exit the model creator preprocessor (`/PREP7`

). To do this we will use command `FINISH`

, which is also part of the original file.

`FINISH`

We can now enter solution module and solve:

`/SOL`

`SOLVE`

`FINISH`

This is equivalent to entering the solution tab in the ANSYS Main Menu and solving the current LS.

At this point, the modified log file should be as follows:

`/Title, Orthotropic Plate with a Hole`

`*SET,a,60e-3`

`*SET,r,7e-3`

`*SET,p,1e6`

`*SET,E1,59.3e9`

`*SET,E2,22e9`

`*SET,G12,8.96e9`

`*SET,nu21,0.047`

`/PREP7`

`ET,1,PLANE82`

`MP,EX,1,E1`

`MP,EY,1,E2`

`MP,NUXY,1,NU21`

`MP,GXY,1,G12`

`RECTNG,0,a,0,a,`

`CYL4,0,0,0,0,r,90`

`ASBA,1,2`

`LESIZE,8,,,50,0.25,,,,0`

`LESIZE,9,,,50,0.25,,,,0`

`LESIZE,5,,,40,,,,,,0`

`SMRT,1`

`MSHAPE,0,2D`

`MSHKEY,0`

`AMESH,3`

`DL,8,3,SYMM`

`DL,9,3,SYMM`

`SFL,2,PRES,-p,`

`FINISH`

`/SOL`

`SOLVE`

`FINISH`

#### Verify Progress

Let's verify that a solution is generated with the list of commands we have created so far. Again, restart ANSYS or go to Utility Menu > File > Clear & Start New and select Do not read file.

Copy the list of commands we have generated so far and paste them in the ANSYS Command Input window. ANSYS performs the solution and a yellow window should pop up saying "Solution is done!".