On different FE elements for beam bending

This post presents a comparison between different hexahedral FEM element formulations in a pure bending cantilever beam problem.
FEM analysis results are post-processed within the CAE-Viewer, iChrome tool for CAE models and results visualization. Extracted results are then compared with the analytical solution with Grapheme, the iChrome data visualization and Analysis tool.
FEM Analysis are performed with the free structural finite element package CalculiX.

Contents

This post is organized as it follows:

  1. Geometry and FEM model
  2. Load and Boundary Conditions
  3. Results
  4. Conclussions

Geometry and FEM model

A steel cantilever beam with a squared cross section is considered. Beam dimensions are reported in following table.

Beam Geometry

Beam Geometry within the CAE-Viewer

Beam dimensions
Rectangular Section Dimension
Beam length
b (mm) h (mm) L (mm)
100 100 1500

Hexahedral elements have been used. Different meshes have been generated by taking into account the following refinement strategies:

  • p-refinement: strategy aimed at improving the results by increasing the displacement field accuracy in each element. This method refers to increasing the degree of the highest complete polynomial (p) within an element without changing the number of elements used. In the test case herein discussed, linear hexahedral elements (C3D8/C3D8I in CalculiX) and quadratic hexahedral elements (C3D20 in CalculiX) are used.
  • h-refinement: strategy aimed at improving the results by decreasing the element size while maintaining the same element formulation. This strategy is usually implemented by dividing each existing element into two or more elements, without changing the original aspect ratio. For this test case, four different mesh (A, B, C and D) have been generated via h-refinement. Details for each mesh are reported in the following table.
FEM Models – Number of elements
Mesh
Number of elements
b h Length
A 1 1 15
B 2 2 30
C 4 4 60
D 8 8 120

Mesh A

Mesh A

Mesh B

Mesh B

Mesh C

Mesh C

Mesh D

Mesh D

Loads and Boundary conditions

The cantilever beam is clamped at one end and free at the other. On the free end a static load of 1000 N, along z-positive direction, has been applied.

A static analysis has been performed for each mesh and for each element formulation.

Results

Following tables report the results obtained for each Mesh and for each element formulation. Results are indicated in terms of percent error with respect to the analytical solution.

FEM Analysis results – C3D8 Elements
MESH Vertical displacement error at free end (%) Stress error at 700 mm from the clamped end (%)
A 36.78 23.93
B 13.29 3.13
C 3.97 -1.90
D 1.21 -1.89
FEM Analysis results – C3D8I Elements
MESH Vertical displacement error at free end (%) Stress error at 700 mm from the clamped end (%)
A 0.73 0.00
B 0.70 0.00
C 0.42 0.00
D 0.28 0.00
FEM Analysis results – C3D20 Elements
MESH Vertical displacement error at free end (%) Stress error at 700 mm from the clamped end (%)
A 1.30 0.00
B 0.51 0.00
C 0.30 0.00
D 0.23 0.00

As expected, linear hexahedral elements (C3D8 elements) generally lead to incorrect results in stress distribution and free-end deflection. However the error can be reduced by increasing the number of elements along the beam axis. At least four elements along the height (mesh C) need to be used in order to reach a good level of accuracy. For bending dominated problems, enhanced strain formulations (C3D8I) or quadratic shape functions elements (C3D20) lead to good results even with a single element along the height.


The incompatible mode eight-node brick element C3D8I is an improved version of the C3D8-element. In particular, shear locking is removed and volumetric locking is much reduced with respect to the standard formulation. This is obtained by supplementing the standard shape functions with so-called bubble functions, which have a zero value at all nodes and nonzero values in between. The C3D8I element should be used in all instances, in which linear elements are subject to bending.

Although the quality of the C3D8I element is far better than the C3D8 element, the best results are obtained with quadratic elements (C3D20).


displacement C3D8 elements

FEM Results visualized within the CAE-Viewer

Following images show the vertical displacement and stress contour for each solution.

displacement C3D8 elements

Comparison between the different meshes with C3D8 elements – Vertical displacement contour

displacement C3D8 elements

Comparison between the different meshes with C3D8 elements – Normal Stress contour

displacement C3D8I elements

Comparison between the different meshes with C3D8I elements – Vertical displacement contour

displacement C3D8I elements

Comparison between the different meshes with C3D8I elements – Normal Stress contour

displacement C3D20 elements

Comparison between the different meshes with C3D20 elements – Vertical displacement contour

displacement C3D20 elements

Comparison between the different meshes with C3D20 elements – Normal Stress contour

Following images report the Vertical displacement error against the position along beam axis created within Grapheme.

C3D8_ERROR

C3D8 elements – Vertical displacement error vs position along beam axis

C3D8I_ERROR

C3D8I elements – Vertical displacement error vs position along beam axis

C3D20_ERROR

C3D20 elements – Vertical displacement error vs position along beam axisr

Conclusions

In this post we have used the CAE Viewer to post-process CalculiX results of a pure bending problem. The analytic results (displacement and stresses) have been compared with the finite element solutions using Grapheme. The comparison with analytic results shows that, for bending dominated problems, the quadratic shape functions (C3D20) or enhanced strain formulations elements (C3D8I) are best suited to avoid shear locking phenomena, which lead to incorrect results for both stress and displacement.

Leave a Reply