Transcript Presentazione di PowerPoint

FE analysis with plane stress and plane
strain elements
E. Tarallo, G. Mastinu
POLITECNICO DI MILANO, Dipartimento di Meccanica
Summary
2
Subjects covered in this tutorial
 An introduction to plane stress and plane strain elements
 An introduction to convergence theory
 A guided example to evaluate a simple structure through
the use of FEM
 Comparison analytical vs numerical solutions
 Other few exercises (to include in exercises-book)
Es02
Es-03
Plane element – topic
3
 Plane stress elements can be used when the thickness of a body is small
relative to its lateral (in-plane) dimensions. The stresses are functions of
planar coordinates alone, and the out-of-plane normal and shear stresses
are equal to zero. Plane stress elements must be defined in the X–Y plane,
and all loading and deformation are also restricted to this plane
 Plane strain elements can be used when it can be assumed that the
strains in a loaded body are functions of planar coordinates alone and the
out-of-plane normal and shear strains are equal to zero.
 DOF active:
1, 2 (translation of each node)
 Output request:
S11, S22, S33, S12
Es02
Es-03
Convergence theory
4
The Convergence Curve
The formal method of establishing mesh convergence requires a curve of a
critical result parameter (typically some kind of stress) in a specific location,
to be plotted against some measure of mesh density. At least three
convergence runs will be required to plot a curve which can then be used to
indicate when convergence is achieved or, how far away the most refined
mesh is from full convergence.
Local Mesh Refinement
All elements in the model should be split in all directions. It is not necessary
to carry this out on the whole model: St Venant's Principle implies that local
stresses in one region of a structure do not affect the stresses elsewhere.
From a physical standpoint then, we should be able to test convergence of a
model by refining the mesh only in the regions of interest, and retain the
unrefined (and probably unconverged) mesh elsewhere. We should also
have transition regions, from coarse to fine meshes, suitably distant from the
region of interest
Es02
Es-03
Convergence – example
5
Es02
Es-03
Exercise 1
6
Part: 3D shell planar
Material: E=210 GPa, ν=0.3
B
Solution Type:
1kN
Thickness=10mm
A
1. Beam elements (no consider fillet)
2. Plane elements (plane-stress or plane-strain?)
2.1 Tri linear
2.2 Tri quadratic
2.3 Quad linear
2.4 Quad quadratic
A. Fine mesh (dimension 10mm)
B. Coarse mesh (dimension 120mm)
3-Analytical solution
For each configuration find:
Max S22 in A
Max displacement in B
(magnitude & U2)
Es02
Es-03
Exercise 1 - results
7
Solution Type
Max S22
Coarse
Max S22
Fine
Max Disp
Coarse
Max Disp
Fine
Beam Elements
20 MPa
20.63 MPa
Mag=1.28 mm
U2=0.97 mm
Mag=1.28 mm
U2=0.97 mm
Plane Tri-Lin
7.28 MPa
18.72 MPa
Mag=0.49 mm
U2=0.34 mm
Mag=1.24 mm
U2=0.83 mm
Plane Tri-Quad
20.62MPa
23.25 MPa
Mag=1.20 mm
U2=0.81 mm
Mag=1.26 mm
U2=0.85 mm
Plane Quad-Lin
13.02 MPa
19.26 MPa
Mag=1.67 mm
U2=1.11 mm
Mag=1.27 mm
U2=0.86 mm
Plane Quad-Quad 20.24 MPa
24.68 MPa
Mag=1.26 mm
U2=0.84mm
Mag=1.26 mm
U2=0.85mm
Analytical
21.66 MPa
Es02
Es-03
U2=0.97 mm
Exercise 2
8
Material: E=210 GPa, ν=0.3
Thickness=10mm
Load: 1 kN (as ex1)
Element: Quad quadratic
Fine mesh
Find Max Mises Stress
Es02
Es-03
Exercise 2 - modeling
9
1- Make 3 different Parts:
2- Insert them as 3 instances
in Assembly
3- Use Translate Command
(leave a gap between the
faces)
Es02
Es-03
Exercise 2 - interaction
10
4- Tie Connections
5- In the assembly fill the gap
with translator command
Es02
Es-03
Exercise 2 - results
11
Es02
Es-03
Exercise 3
12
Part: 3D shell planar
Material: E=210 GPa, ν=0.3
Load: σ0=1 Mpa
Solution Type: plane elements Quad
quadratic
Goal:
1. Find the stress filed around the hole
and compare it with the analytical
solution
2. Find the number of elements that
gives convergence
Coarse and finer mesh, quadrilateral elements
Es02
Es-03
Exercise 3 – analytical solution
The analytical solution of the problem considering
a circular hole in an infinite thin plate:

 0  a 2   0  3a 4 4a 2 
1  2  
1  4  2  cos 2
 r 
2
r
2
r
r 





 0  a 2   0  3a 4 

1  2  
1  4  cos 2
  
2  r  2 
r 


 3a 4 2a 2 

0
 r   1 
 2 sen2
4

2 
r
r 

Concentration coefficient
Analyzing the trend of σθ on the contour of a hole with
the radius a gives the maximum values in
correspondence of π / 2 and 3π / 2.
  ,max  3 0  Kt 
  ,max
3
0
Es02
Es-03
13
Appendix – visualize different field output
Displaying the results
VISUALIZE, is the module that allows you to analyze the results of the analysis
Es02
Es-03
14
Appendix – create a path
15
Create path, defines a set of nodes from
which you can extract the values of the
magnitude of the desired output (stress,
strain, temperature, etc.)
Es02
Es-03
Appendix – create XY data and plot
16
XY Data from path, plots the magnitudes of
chosen parameters according to the
previously selected nodes on the path
Save the data of the plot:
Using >Report>XY save
the data in a report file
Es02
Es-03
Visualize directly the plot