Export to FEA and Run the Analysis

We are now ready to export the results to our finite element analysis program where we can analyze our model.

1. Click Home > Export > Export to Structural Package.
2. Click Browse and select the directory where you would like to save the files. Name the file coupon_ame and click Save.
3. Ensure the 23.0 [C] temperature environment is selected and click Export.

   

4. Navigate to the directory where the files were written. You will see two files, coupon_ame.cdb and coupon_ame.sif. The .cdb file is the structural input file that contains the part geometry, mesh, and loads. The .sif file (structural interface file) contains the mapped fiber orientations and the Ramberg-Osgood parameters.

Before we run our analysis, we will open the coupon_ame.cdb file we just exported and add post-processing commands. These post-processing commands will automatically write the load-displacement results to a text file after the analysis has completed.

1. Open the coupon_ame.cdb file with a text editor and scroll to the end of the file.
2. Copy and paste the following lines at the end of the .cdb file.

   /POST26
   *CFOPEN, coupon_ame_output, txt
   *VWRITE, 'Time', 'U2Top', 'U2Bottom', 'RF2'
   (A4, 5X, 6(A10,7X))
   NUMVAR,100
   
   NSOL, 2, 284, U, Y, U2
   NSOL, 3, 192, U, Y, U2
   RFORCE, 4, 21, F, Y, RF2
   
   STORE, MERGE
   *GET, size,  ACTIVE, 0, SOLU, NCMSS
   *DIM, STS, ARRAY, 100, 4
   VGET, STS(1,1), 1
   VGET, STS(1,2), 2
   VGET, STS(1,3), 3
   VGET, STS(1,4), 4
   *VWRITE, STS(1,1), STS(1,2), STS(1,3), STS(1,4)
   (F4.2, 10(',',3X, E12.6))
   *CFCLOSE
   
   FINISH

3. Save the file.

Now we are ready to run our analysis.

1. Open a command prompt and navigate to the directory containing the .cdb and .sif files (use the Command Shell desktop shortcut to easily open a command prompt).
2. Enter the following commands to submit the model for analysis (in this case with ANSYS 15.0)

   >>ansys-helius 150 coupon_ame.cdb

   Note: The .cdb and .sif files must have the same name.