
The purpose of this
test is to
check shell elements with double curvature. You will use 2D meshes. 

Reference:
MAC NEAL R.H., HARDER R.L., A Proposed Standard Set
of Problems to Test Finite Element Accuracy, Finite Element Design, Vol.1,
pp.320, 1985. 

Specifications
Geometry Specifications
Radius:
R = 10 m 

Angle:
θ
= 18 deg 
Thickness:
th=0.04 m 
Equation:
x^{2} + y^{2} + z^{2} = 100 

For symmetry reasons, only a quarter of the hemisphere
is modeled. The given results are the same for a quarter or for the
whole hemisphere. 
Analysis Specifications
Young Modulus (material):
E = 68.25 MPa 

Poisson's Ratio (material):
ν=
0.3 
Mesh Specifications:
See the values in the table of results. 
Restraints (Userdefined):

At point A: Tz=0

On edge AB: Ty=Rx=Rz=0

On edge CD: Tx=Ry=Rz=0

Loads (Distributed force):
F=1 (outward at A, inward
at D) 


Results

The analytical solution is:
At point A, xdisplacement is 94 mm.

The results correspond to the xdisplacements at point A.
The table below presents the analysis results.
The normalized results (computed results divided by analytical solution)
are listed.
Nodes 
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 
3 x 3 
105.9 
1.127 
99.97 
1.063 
71.17 
0.757 
23.00 
0.245 
5 x 5 
98.02 
1.043 
100.46 
1.069 
96.05 
1.022 
79.25 
0.843 
7 x 7 
95.76 
1.019 
101.95 
1.085 
96.47 
1.026 
94.75 
1.008 
9 x 9 
94.85 
1.009 
102.26 
1.088 
95.48 
1.016 
95.52 
1.016 
11 x 11 
94.97 
1.010 
103.75 
1.104 
94.80 
1.009 
94.52 
1.006 
13 x 13 
93.32 
0.993 
101.87 
1.084 
93.90 
0.999 
93.68 
0.997 


To Perform the Test:
The
hemispherical_shell_concentrated_loads_13nodes_tr6.CATAnalysis document
presents a complete analysis of this case, computed with a mesh formed of
parabolic triangle elements (TR6).
The
hemispherical_shell_concentrated_loads_13nodes_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 and number of nodes, proceed as follow:

Open one of the CATAnalysis documents.

Enter the Advanced Meshing Tools workbench.

In the specification tree, doubleclick on the mesh.
The Global Parameters dialog box appears.

Select the Linear element type.

Compute the case in the Generative Structural
Analysis workbench.
