Transient 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 a transient dynamic response case. You will use 2D meshes.

This test is used to validate the following attributes:

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

  • Transient 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:

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:
    F0 = 100 N/m2     over whole plate

  • Damping:
    d = 2 % in all 16 modes used

  • Time step:
    t = 0.002 s

 

Results

You will find here the results for different finite elements:

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

Values

Error
[%]

Values

Error
[%]

Values

Error
[%]

Values

Error
[%]

Peak displacement [mm]
at t=0.210s

3.523

3.444

2.24

3.445

2.21

3.451

2.04

3.446

2.19

Peak stress [MPa]

2.484

2.221

10.59

2.217

10.75

2.251

9.38

2.234

10.06

Static displacement [mm]

1.817

1.774

2.37

1.775

2.31

1.776

2.26

1.775

2.31

To Perform the Test:

The Transient_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.