
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:

Restraints (Userdefined):

On edge AD, Tx = 0

At point A, Tx = Ty = 0


Loads (Distributed force):



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:

Open the CATAnalysis document.

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

Compute the case in the Generative Structural
Analysis workbench.
