Cantilever Thin Square Plate

The purpose of this test is to check the distorted meshes. You will use 2D meshes formed of parabolic quadrangle elements (QD8).

Reference:

NAFEMS-Glasgow, Benchmark newsletter, April 1989, p.19.

 

Specifications

Geometry Specifications

Length:
L = 10 m   

Width:
W = 10 m
Thickness:
th = 0.05 m  


Analysis Specifications

Young Modulus (material):
E = 200 GPa

Poisson's Ratio (material):
ν = 0.3

Mesh Specifications:

  • Parabolic quadrangle elements (QD8)   

  • Constrained points

    • For tests 1 and 3: regular

    • For tests 2 and 4:
      Point 1: x = 4.0 and y = 4.0
      Point 2: x = 2.25 and y = 2.25
      Point 3: x = 4.75 and y = 2.5
      Point 4: x = 7.25 and y = 2.75
      Point 5: x = 7.5 and y = 4.75
      Point 6: x = 7.75 and y = 7.25
      Point 7: x = 5.25 and y = 7.25
      Point 8: x = 2.25 and y = 7.25
      Point 9: x = 2.5 and y = 4.75

Restraints (User-defined):

Along y axis, Tx = Ty = Tz =  Ry = 0  

 

Results

The results are given in the table below.
Normalized results (computed results divided by the reference solution) are listed.

Mode 

Reference 

Test 1

Test 2

Test 3

Test 4

Computed  results
[Hz]

Normalized  results

Computed  results
[Hz]

Normalized  results

Computed  results
[Hz]

Normalized  results

Computed  results
[Hz]

Normalized  results

1

0.421

0.419

0.995

0.420

0.998

0.419

0.995

0.420

0.998

2

1.029

1.023

0.994

1.032

1.003

1.024

0.995

1.028

0.999

3

2.582

2.576

0.998

2.606

1.009

2.697

1.045

2.703

1.047

4

3.306

3.295

0.997

3.317

1.003

3.420

1.034

3.540

1.071

5

3.753

3.733

0.995

3.930

1.047

3.900

1.039

3.993

1.064

6

6.555

6.841

1.044

6.799

1.037

6.677

1.019

6.844

1.044

To Perform the Test:

The cantilever_thin_square_plate_test2.CATAnalysis document presents a complete analysis of the test 2, computed with an irregular mesh formed of parabolic quadrangle elements (QD8).

To compute the three other tests, with other nodes of distribution, 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.