Step 9: Validate the results

Simple Checks

Does the deformed shape look reasonable and agree with the applied BCs? We checked this in step 8.

Do the reactions at the supports balance the applied forces for static equilibrium? To check this, select

Main Menu > General Postproc > List Results > Reaction Solu

Select All struc forc F for Item to be listed and click OK.

There are no applied forces in this problem, so the total reaction force should be zero for equilibrium. The total reaction force in the radial direction (FX) is 4.6 N which is close to zero. We can lower it even further by refining our estimate of rc. The total reaction forces FY in the cirumferential direction and FZ in the axial direction are small but not zero. This is possible because FX is small but not zero. So the structure is in equilibrium to a reasonable degree of approximation.

Refine Mesh

Let's repeat the calculations on a mesh with twice the no. of mesh divisions in the radial and axial directions while retaining a single division on AC and BD. We need to reset NDIV and SPACE on the following lines:

Line no.












Let's use a different jobname for the refined mesh case. Change jobname: Utility Menu > File > Change Jobname

Enter cbeam2 as the New jobname and click OK.

Main Menu > Preprocessor > Meshing > MeshTool

Delete the current mesh: Select clear under Mesh: and Pick All in the pick menu. The mesh is deleted.

Utility Menu > Plot > Lines

Under Size Controls and Lines, click Set. This brings up a pick menu.

Pick lines L2,L4,L8, and L12 and click OK in the pick menu. Enter 10 for No. of element divisions, leave Spacing Ratio blank and click Apply.

Pick lines L7,L9, and L11 in the Graphics window and click OK in the pick menu. Enter 16 for No. of element divisions, 0.3 for Spacing Ratio and click Apply.

Pick line L5 in the Graphics window and click OK in the pick menu. Enter 16 for No. of element divisions, 1/0.3 for  Spacing Ratio and click OK.

Select Volumes for Mesh: and Hex for Shapes:, then click Mesh.

Since we applied the BCs to the finite-element model rather than the solid geometry model, the BCs were deleted along with the mesh. So we have to reapply the BCs again. Repeat step6 to reapply the BCs. It might feel like a chore but consider it as good practice. Since the vface2 table for applying the BC on face 2 already exists, you need not recreate the function or the table.

Save your work: Toolbar > SAVE_DB

This will create the file cbeam2.db in your working directory.

After reapplying the BCs, solve the problem as in step7.

Plot Circumferential Stress

Display theσθstress distribution over face 1:

Utility Menu > PlotCtrls > Pan,Zoom,Rotate > Right

Main Menu > General Postproc > Plot results > Contour Plot > Nodal Solu

Select Stress from the left list, Y-direction SY from the right list and click OK.

(Click Picture for Larger Image)

Compare this result with the plot obtained on the coarser mesh. The results on the two meshes compare well indicating that the coarse mesh provides good resolution. Similarly, compare the von Mises stress results on the two meshes.


Utility Menu > File > Exit

Select Save Everything and click OK.


Cook, R.D., Malkus, D.S., Plesha, M.E., and Witt, R.J., Concepts and Applications of Finite Element Analysis, Fourth Edition, John Wiley and Sons, Inc., 2002.

Back to Problem Specification

See and rate the complete Learning Module

Go to all ANSYS Learning Modules

  • No labels