ANSYS - 3D Curved Beam step 8

Problem Specification
1. Start-up and preliminary set-up
2. Specify element type and constants
3. Specify material properties
4. Specify geometry
5. Mesh geometry
6. Specify boundary conditions
7. Solve!
8. Postprocess the results
9. Validate the results

Step 8: Postprocess the results

Enter the postprocessing module to analyze the solution.

Main Menu > General Postproc

Plot von Mises Stress

To display the von Mises stress distribution as continuous contours, select

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

Select Stress from the left list, von Mises SEQV from the right list and click OK.

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

(Click Picture for Larger Image)

The maximum von Mises stress is 147 MPa and occurs at the bottom on the symmetry line.

Plot Circumferential Stress

σ_θis the SY stress component in cylindrical coordinates in ANSYS. Activate the cylindrical coordinate system for results display (you need to do this even if you were working in the cylindrical system in the preprocessor):

Main Menu > General Postproc > Options for Outp

Select Global Cylindric for Results Coord System.

To display theσ_θstress distribution over face 1 as continuous contours, select

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

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

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

(Click Picture for Larger Image)

Check where the maximum (MX) and minimum (MN) σ_θvalues occur in the plot. The circumferential stress is tensile (positive) and compressive (negative) on the inner and outer portions of the cross-section, respectively. Is this what you'd have expected? Theσ_θcontours are more closely spaced at smaller r values. This agrees with the prediction of curved beam theory that the stress gradients will be highest on the edge nearest the center of curvature.

Plot Neutral Axis

The neutral axis is the locus of points where σ_θis zero. To visualize the neutral axis, we'll change the contour levels that are plotted.

Utility Menu > PlotCtrls > Style > Contours > Uniform Contours

Enter 2 for Number of contours, and choose User specified for Contour Intervals. Enter Min contour value=-0.2E9, Max contour value=0.2E9, and Contour value incr=0.2E9. Click OK.

 

This plots the regions with positive and negative σ_θvalues in different colors. In the red region, 0<σ_θ<200MPa and in the blue region, -200MPa<σ_θ<0. So the boundary between the two colors is the neutral axis.

The FEA results indicate that the neutral axis is curved, contrary to the assumption in mechanics of materials theory.

Plot Radial Stress

In cylindrical coordinates, the radial stress is the SX stress component.

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

Select Stress from the left list, X-direction SX from the right list and click OK.

Change contour plot options back to original:

Utility Menu > PlotCtrls > Style > Contours > Uniform Contours

Enter 9 for Number of Contours, and choose Auto calculated for Contour Intervals. Click OK.

(Click Picture for Larger Image)

The radial stress is tensile over the entire cross-section.

Plot Deformed Shape

Main Menu > General Postproc > Plot Results > Deformed Shape

Select Def + undeformed and click OK.

This plots the deformed and undeformed shapes in the Graphics window. The maximum displacement DMX=0.230e-4 m.

 

Animate the deformation:

Utility Menu > PlotCtrls > Animate > Deformed Shape

Select Def + undeformed and click OK. Select Forward Only in the Animation Controller.

From the animation of the deformation of the cross-section, check that the following BCs are satisfied: u=0 at node A, w=0 along AB and CD. (Note that the z-direction is from right to left in the above view).

The radial stress is tensile, so the radial dimension becomes larger as expected. We saw that the circumferential stress is, respectively, tensile and compressive on the inner and outer portions of the cross-section. You can check that the stress SZ parallel to the axis of revolution is small. Therefore, the Poisson effect should cause the inner and outer portions, respectively, to contract and expand in the z-direction as is observed. Circumferential tension on the inner portion pulls material toward the center of curvature. Outer corners are more flexible than the central portion. So it makes sense that the outer, bottom corner moves inward with respect to central point A (Cook et al). Thus, the deformation we gets looks reasonable.

Animate the front view:

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

Utility Menu > PlotCtrls > Animate > Deformed Shape

Select Def + undeformed and click OK. Select Forward Only in the Animation Controller.

From this animation, check that the BCs for v on both faces are satisfied.

Save your work: Toolbar > SAVE_DB

Go to Step 9: Validate the results