Bonded Blades in Compression

This test lets you check the bending/extension coupling in non-symmetric stack composite plates and the traverse shear behavior in a thick plate.

For this test, the reference is the mesh formed of linear hexahedron elements (HE8). You will use 2D meshes.

Reference:

3D Model with HE8 element, computed with CATIA.
 

Specifications

Geometry Specifications

Length:
L = 10 000 mm

Width:
b = 1 000 mm

Thickness:
h = 400 mm divided in two layers  


Analysis Specifications

Material 1:

  • Young Modulus (material):
    E = 100 MPa

  • Poisson's Ratio:
    ν = 0.3

Material 2:

  • Young Modulus (material):
    E = 10 MPa

  • Poisson's Ratio:
    ν = 0.2

Mesh Specifications:

  • 10 x 2 elements for linear quadrangle (QD4) and parabolic quadrangle (QD8) elements

  • 10 x 2 x 1 elements for linear hexahedron elements (HE8)

Restraints:
Clamp on End 1

Loads:
Force density Fx = -30 N on End 2
 

Results

The static analysis results correspond to the displacements Tx and Tz at End 2.

The buckling analysis is performed for this 30 N load case. The buckling coefficients for the lowest two modes, computed with CATIA, are presented in the table below:

Analysis Case

 Quantity

Reference
 Linear Hexahedron 
(HE8)

Computed Results

 Linear Quadrangle 
(QD4)

 Parabolic Quadrangle
(QD8)

Static Case

Tx max [mm]

-0.027

-0.0277

-0.0281

Tz max [mm]

-0.834

-0.834

-0.835

Buckling Case

Coefficient 1

121.634

121.197

120.743

Coefficient 2

1126.56

1095.34

1079.94

To Perform the Test:

The Bonded_blades_compression_QD8.CATAnalysis document presents a complete analysis of this case, computed with a mesh formed of parabolic quadrangle elements (QD8).

The Bonded_blades_compression_HE8.CATAnalysis document presents a complete analysis of this case, computed with a mesh formed of linear hexahedron elements (HE8).

To compute the mesh with linear quadrangle elements (QD4), proceed as follow:

  1. Open the Bonded_blades_compression_QD8.CATAnalysis document.

  2. Enter the Advanced Meshing Tools workbench.

  3. In the specification tree, double-click the mesh part. The Global Parameters dialog box appears.

  4. Select Linear as element type.

  5. Compute the case in the Generative Structural Analysis workbench.