Thick Beam

The purpose of this test is to check membrane elements. You will use 2D meshes.

Reference:

M. ZIENKIEWICKZ, The Finite Element Method, 4th edition, Vol. 1, p.386.
 

Specifications

Geometry Specifications

Length:
L = 10 m

Width =
W = 2 m

Thickness:
th = 0.001 m  

Analysis Specifications

Young Modulus (material):
E = 1500 MPa

Poisson's Ratio (material):
ν = 0.25

Mesh Specifications:

  • Mesh size: 4000 mm

  • Constrained points (using the points created in the CATPart)

  • Membrane elements

Restraints (User-defined):

  • On edge AD, Tx = 0

  • At point A, Tx = Ty = 0

Loads (Distributed force):

  • Case 1:
    FX = 1000 N at point B
    FX = -1000 N at point C

  • Case 2:
    Fy = 150 N at points B and C 
 

Results

  • The analytical solution is the vertical displacement at point B. The corresponding analytical solutions are:
    Case 1: Ty = 100.00 mm
    Case 2: Ty = 102.60 mm

  • The table below presents the analysis results.
    The results correspond to the vertical displacement at point B.
    The normalized results (computed results divided by analytical solution) are listed.

     

    Analytical solution [mm]

    Values

    Linear triangle
    (TR3)

    Parabolic triangle
    (TR6)

    Linear quadrangle
    (QD4)

    Parabolic quadrangle
    (QD8)

    Computed results
     [mm]

    Normalized results

    Computed results
     [mm]

    Normalized results

    Computed results
     [mm]

    Normalized results

    Computed results
     [mm]

    Normalized results

     Case 1

    100

    25.49

    0.255

    100

    1.000

    96.18

    0.962

    100

    1.000

     Case 2

    102.6

    29.78

    0.290

    101.54

    0.989

    98.05

    0.956

    102.8

    1.002

To Perform the Test:

The thick_beam_qd8.CATAnalysis document presents a complete analysis of this case, computed with a mesh formed of parabolic quadrangle elements (QD8).

To compute the case with other types of elements, proceed as follow:

  1. Open the CATAnalysis document.

  2. In the Advanced Meshing Tools workbench, change the mesh specifications as indicated above.

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