Introduction to the Finite Element Method (3)
Petr Kabele Czech Technical University in Prague Faculty of Civil Engineering Czech Republic
[email protected] ∗ people.fsv.cvut.cz/~pkabele
1
Outline Types of finite element programs Practical aspects of finite element analysis Examples of FE modeling
2
Finite element programs – classification and structure FEM programs ➢general purpose ● simulation of general physical problems (statics, dynamics, heat/mass transport, magnetism, ... , coupled problems) ● more complex problem definition/input (choice from many options) ● user must perfectly understand the mathematical and physical essence of analyzed problem ● e.g DIANA, ADINA, ABAQUS ➢specialized, engineering ● simulation of specific engineering problems (e.g. elastic truss structure) ● user-friendly input (mouse-click, predefined material models, structural members, cross-sections etc., close linkage to design codes) ● use in engineering practice (structural design) ● e.g. SAP 3
Structure of finite element programs Preprocesor graphical interface for data input
Computational core FE program itself
Postprocesor graphical interface for processing and visualization of results
4
Practical aspects of finite element analysis General consideration: “Finite element analysis is essentially an approximate method for calculating the behavior of real structures by performing an algebraic solution of a set of equations describing idealized structures”
Physical reality
Finite element model
5
Selection of analysis type Consider what physical phenomena should be analyzed. stress analysis stability static mechanical
dynamic
heat transport
... ...
mass transport fluid
... ...
linear nonlinear
modal analysis transient analysis ... ...
linear nonlinear
magnetism coupled, interaction ... ...
6
Selection of modeling hypotheses “The most difficult part” Geometry and morphology (model scope and detail, structural form, internal composition, connections between the structural elements,…) Material models and properties Actions (mechanical, physical, chemical…) Existing alterations and damage (cracks, constructional mistakes, disconnections, crushing, leanings, …) The interaction of the structure with its surroundings (soil, fluids, other structural parts,...)
7
To this end: Clarify what result is anticipated (e.g. overall deformation of a large structure vs. crack propagation at a detail). Consider, what information about the analyzed structure is available (geometry, material, surroundings/supports, loading). Think of suitable simplification, reduction of dimension, substructuring, decomposition, use of symmetry. Select suitable kinematic assumptions and dimension (truss, beam, 2D solid, plate, shell, 3-D solid). Bear in mind the complexity of model, solution time, postprocessing time and visualization of results. In complex problems, combining various kinematic assumptions may be efficient (e.g. beam + plate). However, proper linkage of all DOF’s must be ensured.
8
Pre-analysis Make a rough estimation of the expected result (e.g. simplified calculation by hand). Estimate locations of strain concentration and locations of uniform strain – use denser mesh in locations with steeper gradients. Run a pilot analysis with coarser mesh compare results with the rough estimate use the results to identify further locations of strain concentration Refinement and analysis Refine the hypotheses and FE mesh as necessary based on the previous step and run the analysis
9
Preliminary results check Always check after analysis – plot magnified displacement of the model, display the stresses (generalized stresses), reactions Compare results with the rough estimate. Check that loading and kinematic boundary conditions act as expected (stress under loading must correspond to imposed distributed load, outer reactions must be in equilibrium with imposed loading). Check for possible discontinuities due to improper meshing (overlaps of mesh, unexpected stress concentrations) If check fails, find and correct mistakes in input and return to “Refinement and analysis”.
10
Example:
11
Rigorous results check Analysis verification: “Is the mathematical formulation solved correctly?” Check error/accuracy/convergence messages. Check mesh quality criteria. ... ... Analysis validation “Does the mathematical model correctly represent the physical reality?” Validation of modeling hypotheses ... see SA2 Lecture 1.
12
Results processing and presentation FE analysis usually produces huge amount of data. These must be sorted out and presented in an easy-to-understand way. Some examples: plot of deformed configuration contour plots of field variables (displacement, stress, strain, components or principal values, ...) vector plots (displacements, principal stress, strain, ...) line plots of field variables along line, section time history plots/tables of values in given points extreme values of field variables ... ...
(see iDiana intro for examples)
13
Example 1
Perform analysis of a slab. Uniform distributed load 8 kN/m2 (incl. self weight) Thickness: 0.15 m Plan: 2 x 3 m
Material (R/C): E = 30 GPa ν = 0.2
Supports allow free sliding and rotation but no vertical movement (up or down)
14
Model 1 : plate elements mesh 1 3-node plate elements 6 DOF/node (3 translations + 3 rotations) mesh 2
15
Model 1 : plate elements Boundary conditions
u, v, ϕx, ϕy, ϕz ... free w ... fixed
ϕx, ϕy, ϕz ... free u, v, w ... fixed u, v, ϕx, ϕy, ϕz ... free w ... fixed v, ϕx, ϕy, ϕz ... free u, w ... fixed u, v, ϕx, ϕy, ϕz ... free w ... fixed
Note: these point BC are imposed to prevent rigid body movement in slab plane.
16
Model 1 : plate elements - results Deflection
17
Model 1 : plate elements - results Bending moment intensities Mesh 1: Element 59
mx Int point 1 Int point 2 Int point 3 Average:
-9.24586E-04 -4.27317E-04 -7.25490E-04 -6.92464E-4
my -5.78145E-03 -5.93220E-03 -5.66659E-03 -0.00579341
Mesh 2: Element 431
mx Int point 1 Int point 2 Int point 3 Average
-5.05462E-05 -5.62267E-04 -3.10636E-04 -9.23449e-4
my -5.63296E-03 -5.64567E-03 -5.64596E-03 -0.00564153
18
Model 1 : plate elements - results Stress ... may be not directly accessible, calculated from σ y , ext = ±
6 my 2 h
σy,ext = ±1.54491 MPa
σy,ext = ±1.50441 MPa
19
Model 1 : plate elements - results Deformed shape and reactions (notice corner forces)
20
Model 1 : plate elements - results Deformed shape and reactions (notice corner forces)
21
Model 2 : solid elements
mesh 1
20-node isoparametric solid elements 3 DOF/node (3 translations) mesh 2
mesh 3
22
Model 2 : solid elements Boundary conditions
u, v ... free w ... fixed
z, w
x, u
u, v, w ... fixed u, v ... free w ... fixed
u, w ... fixed
y, v
u, v ... free w ... fixed
Note: these point BC are imposed to prevent rigid body movement in slab plane.
23
Model 2 : solid elements - results Deflection
24
Model 2 : solid elements - results Deformed shape and reactions (notice corner forces)
25
Model 2 : solid elements - results Bending stress σy
26
Models 1, 2, 3: comparison
Deflection
y-axis
27
Models 1, 2, 3: comparison
Model
Extreme stress (MPa)
Plate 1
±1.54
Plate 2
±1.50
Solid 1
±1.64*)
Solid 2
±1.57*)
Solid 3
±1.59*)
*)
extrapolated values
28
Example 2 Perform a stress analysis of a wall exposed to uniform load, self-weight and foundation settlement. Identify the locations and magnitudes of maximum tension.
29
Initial calculation 4-node isoparematric quarilateral plane stress elements (Q4)
30
Deformed mesh
31
Principal stresses
32
Maximum principal stress
33
Maximum principal stress – smoothed plot
34
Convergence study – meshes Q4 elements
Q9 elements
35
Convergence of extreme displacement
Convergence of max. princ. stress 3.0
-7.008E-03 -7.010E-03
2.5
-7.014E-03
Q4
-7.016E-03
Q9
-7.018E-03
Q9a
sig_max
u_ext
-7.012E-03 Q4
2.0
Q9
1.5
Q9a
1.0
-7.020E-03 -7.022E-03
0.5
-7.024E-03
0.0
-7.026E-03 100
1000
10000
100000
100
1000
DOF
Mesh 1 2 3 4 5 6 4r
El. type Q4 Q4 Q4 Q9 Q9 Q9 Q9
10000
100000
DOF
# of elem 106 408 1616 106 408 1616 378
# of DOF 262 914 3426 946 3458 13314 3114
u_ext -7.0239E-03 -7.0148E-03 -7.0107E-03 -7.0128E-03 -7.0095E-03 -7.0090E-03 -7.0097E-03
sig_max 1.671 2.328 2.631 2.346 2.606 2.760 2.782
36
Maximum principal stress
Q4 elements
Q9 elements
37
Maximum principal stress
Q4 elements
Q9 elements
38
Maximum principal stress
Q4 elements
Q9 elements
39
Local refinement
40
41
Convergence of extreme displacement
Convergence of max. princ. stress 3.0
-7.008E-03 -7.010E-03
2.5
-7.014E-03
Q4
-7.016E-03
Q9
-7.018E-03
Q9a
sig_max
u_ext
-7.012E-03 Q4
2.0
Q9
1.5
Q9a
1.0
-7.020E-03 -7.022E-03
0.5
-7.024E-03
0.0
-7.026E-03 100
1000
10000 DOF
100000
100
1000
10000
100000
DOF
42
References K.J. Bathe: Finite Element Procedures, Prentice Hall, Inc., 1996 ADINA R&D, Inc.: Theory and modeling guide, Volume I: ADINA, November 2006 TNO DIANA BV.: DIANA User's Manual -- Release 9.3 -- Teacher Edition, 2008,
43
Remark This document is designated solely as a teaching aid for students of CTU in Prague, Faculty of Civil Engineering, course Numerické metody v inženýrských úlohách. This document is being continuously updated and corrected by the author. Despite author’s utmost effort, it may contain inaccuracies and errors. Limitation on Liability. Except to the extent required by applicable law, in no event will the author be liable to any user of this document on any legal theory for any special, incidental, consequential, punitive or exemplary damages arising out of the use of the work, even if author has been advised of the possibility of such damages. This is a copyrighted document © Petr Kabele, 2007 – 2012
Last modified: 28.11.2012
44