# Buckling of a Straight Beam (Out-of-Plane Buckling) This test lets you compare analysis results for the buckling of a straight beam in CATIA with the Beam Theory. In other words, you will study the quality of distorted shell elements in a buckling analysis. You will use 2D meshes. Reference:

Beam Theory.

## Specifications

### Geometry Specifications

 Length: L = 100 mm Width: W = 12 mm Thickness: th = 1 mm

### Analysis Specifications

 Young Modulus (material): E = 1e+09 N_m2 = 1000 MPa Poisson's Ratio (material): ν = 0 Mesh Specifications: Constrained points (using the points created in the CATPart) Shell elements Restraints (User-defined): At point B: Tx = 0 At edge AB: Ty = Tz = Rx = 0 Loads: The line forced density at edge CD is: Ty = -83.333 N_m

## Results

The critical load is given by column Buckling theory: In this particular case, the result is Nc = 0.2467 N.

The table below presents the results of the solver computation and the percentage of error compared with the results of the Beam Theory.

 Linear triangle shell (TR3) Parabolic triangle shell (TR6) Linear quadrangle shell (QD4) Parabolic quadrangle shell (QD8)    Mesh Regular Irregular Regular Irregular Regular Irregular Regular Irregular Computed buckling factor [N] 0.2488 0.2491 0.2463 0.2470 0.2467 0.2479 0.2467 0.2471 Error [%] 0.9 1 0.2 0.1 0 0.5 0 0.2 To Perform the Test:

The Straight_Beam.CATAnalysis document presents the complete analysis of the buckling case, computed with an irregular mesh formed of parabolic triangle elements (TR6).

To compute the case with linear triangle (TR3), linear quadrangle (QD4) and parabolic quadrangle (QD8) elements, open the Straight_Beam.CATPart document and proceed as follow:

1. Define the mesh using the Surface Meshing workshop in the Advanced Meshing Tools workbench.

2. In Generative Structural Analysis workbench, define analysis specifications as shown above.

3. Insert and compute buckling case solution in Generative Structural Analysis workbench. To create an irregular mesh, use the Add/Remove Constraints icon in the Local Specifications toolbar, then select the points on the part. 