Harmonic Forced Vibration of a Simply-supported Thin Square Plate

This test lets you check analysis results for a simply-supported thin square plate, in the context of an harmonic dynamic response case. You will use 2D meshes.

This test proposed by NAFEMS is used to validate the following attributes:

  • 2D shell elements (i.e. the elementary stiffness and mass matrices)

  • Harmonic dynamic response solve algorithms.

Reference:

NAFEMS-Glasgow, Benchmark newsletter, Report No. E1261/R002, p.21, February 1989.
 

Specifications

Geometry Specifications

Length:
L = 10000 mm

Thickness:
th = 50 mm

Analysis Specifications

Young Modulus (material)
E = 200 GPa

Poisson's Ratio (material)
ν = 0.3

Density:
ρ = 8000 kg/m3

Restraints (User-defined):

Tx = Ty = Rz = 0 at all nodes
Tz = 0 along all four edges
Rx = 0 along edges x = 0 and x = 10000 mm
Ry = 0 along edges y = 0 and y = 10000 mm

  • Loads:
    F = F0 sin wt

    where:

    • F0 = 100 N/m2

    • w = 2 f

    • f = 0  to  4.16 Hz

  • Damping
    d = 2%     in all 16 modes used
 

Results

The results for different finite elements are presented in the table below.

The peak is the value at undamped natural frequency.
In this particular test, the undamped natural frequency is 2.377 Hz.

Type of values

Reference solution

Values

Linear triangle shell
(TR3)
64 x 64 elements

Parabolic triangle shell
(TR6)
32 x 32 elements

Linear quadrangle shell
(QD4)
32 x 32 elements

Parabolic quadrangle shell
(QD8)
16 x 16 elements

Computed Results

Error [%]

Computed Results

Error [%]

Computed Results

Error [%]

Computed Results

Error [%]

Peak displacement [mm]
at 2.377 Hz

45.420

45.430

0.023

45.430

0.022

45.477

0.125

45.429

0.020

Peak stress [MPa]

30.030

32.005

6.58

32.082

6.83

31.976

6.48

32.227

7.32

To Perform the Test:

The Harmonic_forced_vibration_of_a_simply_supported_thin_square_plate.CATAnalysis document presents a complete analysis of this case, computed with a mesh formed of linear quadrangle elements (QD4).

To compute the case with parabolic quadrangle (QD8), linear triangle (TR3) and parabolic triangle (TR6) elements, proceed as follow:

  1. Open the CATAnalysis document.

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

  3. In the Generative Structural Analysis workbench, compute the case.