Application of Boundary Conditions to Obtain Better FEA Results

Application of Boundary Conditions
to Obtain Better FEA Results
Kee H. Lee, P.E. (kee007.lee@samsung.com)
Design & Structural QC Group
Civil Design Team
November 20, 2015

1
Contents
I. Finite Element Method
II. Pre-requisition for Structural Analysis
III. Typical Boundary Conditions (B.C.)
IV. Element Mesh Generation
V. FE Analysis Boundary Based on Structural Behavior
VI. Examples of B.C. Applications

2
Contents - cont.
Application of Boundary
Conditions
1. Finite Element
Method
Purpose
Fundamental Concepts
Discretization
Pre/Post-Processing
Advantages & Disadvantages
2. Pre-requisition for
Structural Analysis
3. Typical Boundary
Conditions (B.C.)
4. Element Mesh
Generation
5. FE Analysis
Boundary Based on
Structural Behavior
6. Examples of B.C.
Applications
Types of Structural Analysis
Element Types
Degree of Freedom
Element Coordinate Systems & Output Data
Connection types of Frame Structure
Connecting Different Kinds of Elements
Structural Symmetry
Loading Condition for
Underground Tunnel Modeling
Boundary Condition for Bored Pile
Subgrade Modeling Using Solid Elements
Bottom-up Method
Geometrical Modeling Method
Basic Tips of Geometrical Modeling Method
Modeling Method Using CAD Model
Plane Stress and Plane Strain Modeling
Modeling for Vessel Foundation
Foundation Analysis Programs
Linear & Nonlinear System Modeling
Isolation Plan with Expansion Joints
Global FE Model (Preliminary)
Structural Component for FE Modeling
and Analysis
Thermal Structural Analysis Using
Nonlinear Frictional Contact
Maximum Spacing of Expansion Joint
B.C. Effects in Thermal Structural Analysis
Constraint Equation
Application of Boundary Conditions
to Obtain Better FEA Results

3
FEA Modeling & Analysis
FE Model Generation
Structural Analysis
for Component
Isolation Plan
Structural Analysis
with Symmetric
Boundary Condition
Example 1: Structure with Single
Component
Example 2: Structure with Multi
Components
Example 3: FE Analysis for Global
Structural Behavior
Example 5: Thermal Structural
Analysis Using Linear Horizontal
Supports
Example 4: Thermal Structural
Analysis Using Nonlinear
Frictional Contact
Example 6: Local Detail Thermal
Structural Analysis (Plane Strain)
Example 7: Evaluation of
Structural Integrity (Tower Crane
Foundation)
Example 8: Evaluation of Concrete
Crack (Equipment Foundation)
Example 9: Thermal Analysis
(Temperature Distribution)
Contents - cont.
Examples of
Finite Element Modeling & Analysis

4
1. Finite Element Method (FEM)

5
 Purpose
 To solve problems with complicated geometries, loadings, and material
properties where analytical solutions cannot be obtained
 To understand the physical behaviors of a complex object (strength,
heat transfer capability, fluid flow, etc.)
 To predict the performance and behavior of the design;
to calculate the safety margin; and to identify the weakness of the
design accurately
 To identify the optimal design with confidence

6
FEM
approximate
 Fundamental Concepts
 Many engineering phenomena can be expressed by “governing
equations” and “boundary conditions”
Elastic problems
Thermal problems
Fluid flow
Electrostatics
etc.
Governing Equation
(Differential Equation)
𝐿 𝜙 + 𝑓 = 0
Boundary Conditions
𝐵 𝜙 + 𝑔 = 0
𝑲 𝒖 = 𝑭
A Set of Simultaneous
Algebraic Equation

7
 Fundamental Concepts – cont.
Property [K] Behavior {u} Action {F}
Elastic stiffness displacement force
Thermal conductivity temperature heat source
Fluid viscosity velocity body force
Electrostatic permittivity electric potential charge
𝑲 𝒖 = 𝑭 𝒖 = 𝑲 −𝟏
𝑭

8
𝑲 𝒖 = 𝑭
: Stiffness matrix for one linear Spring element
 One type of degree of freedom
 Symmetric (forces areequal and oppositeto equilibrium, -f1=f2)
 Singular (boundary condition is required, u1=0)

9
𝑲 𝒖 = 𝑭

10
 Assembling Element Equations to Obtain Global Equation
𝑲 𝒖 = 𝑭
𝑲 𝑬
𝒖 𝑬
= 𝑭 𝑬
𝑲 𝑬
𝒖 𝑬
= 𝑭 𝑬
𝑲 𝑬 𝒖 𝑬 = 𝑭 𝑬
𝑲 𝑬
𝒖 𝑬
= 𝑭 𝑬
1. Obtain the algebraic equations for each element
2. Put all the element equations together

11
 Assembling Element Equations to Obtain Global Equation

12
Real
Structure
Simplified
Physical Model
 Discretization
 FEM cuts a structure into several
elements (pieces of the structure).
 Then reconnects elements at “nodes” as
if nodes were pins or drops of glue that
hold elements together.
 This process results in a set of
simultaneous algebraic equations.
Discretized
Model (mesh)

13
 Pre-Processing
 Discretize Continuum (Modeling)
 Impose Boundary Conditions
 Impose External Forces
 Solution (Internal Processing)
 Find Element Stiffness Matrix
 Assemble Element Stiffness Matrix (System Stiffness Matrix)
 Solve Displacements
 Convert Displacement into Force, or Stress
 Post-Processing
 Sort, Print, and Plot Selected Results from Finite Element Solution

14
 Advantages
 Can readily handle very complex geometry
 Can handle a wide variety of engineering problems;
Solid mechanics - Dynamics - Heat problems - Fluids - Electrostatic problems
 Can handle complex loading;
Nodal load, Element load, Time or frequency dependent loading
 Disadvantages
 The FEM obtains only "approximate" solutions.
 The FEM has "inherent" errors.

15
2. Pre-requisition for Structural Analysis

16
Static Analysis Modal Analysis
Harmonic Analysis
Transient Dynamic Analysis
Spectrum Analysis
Buckling Analysis Explicit Dynamic Analysis
Available only
in Linear Analysis ←Linear B.C. Required
Typical applications
 Droptests
 Impact and Penetration
 Types of Structural Analysis
𝑴 𝒖 + 𝑪 𝒖 + 𝑲 𝒖 = 𝑭(𝒕)
General Equationof Motion
𝑴 𝒖 + 𝑲 𝒖 = 𝟎
Linear Equationof Motion
for Free, Un-dampedVibration

17
 Nonlinear Structural Analysis
 Geometric Nonlinearities:
If a structure experiences large
deformations, its changing
geometric configuration can
cause nonlinear behavior.
 Material Nonlinearities:
A nonlinear stress-strain
relationship, such as metal
plasticity shown on the right,
is another source of
nonlinearities.
 Boundary Condition (Contact) :
“changing status” nonlinearity,
where an abrupt change in
stiffness may occur when
bodies come into or out of
contact with each other.
← compress only spring included
Source: ANSYS Mechanical Introduction to Structural Nonlinearities

18
 Element Types

19
Element Type
Translation Rotation
Required Data
X Y Z X Y Z
Truss Yes Yes Yes Area
Beam Yes Yes Yes Yes Yes Yes Area
2D Solid Yes Yes
Membrane Yes Yes Yes Thickness
Plate Yes Yes Yes Yes* Yes* Thickness
Solid Yes Yes Yes
 Degree of Freedom of Each Element Type

20
Element Coordinate Systems of Shell andBeamElements
 Element Coordinate Systems

21
 Element Output Data
SignConventionof Shell Element Forces
X Directional Stress due toMoment (Mx)
Source: STAAD.Pro – Technical Reference Manual

22
 Element Output Data – cont.
Three Directional Stresses of SolidElement
Solid element can simulate shear deformation and
nonlinear stress distribution in thick members.

23
 Calculation of Design Moments
 Shell Element
 Solid Element
𝑴 𝑼𝑿 = 𝑴 𝑿 + 𝑨𝑩𝑺 𝑴 𝑿𝒀 ∗ 𝑺𝑮𝑵(𝑴 𝑿)
𝑴 𝑼𝒀 = 𝑴 𝒀 + 𝑨𝑩𝑺 𝑴 𝑿𝒀 ∗ 𝑺𝑮𝑵(𝑴 𝒀)
𝑴 𝑼𝑿 = (𝒛𝒊 − 𝒛 𝒄) × (𝝈 𝑿𝒊 − 𝝈 𝑿)𝑨𝒊
𝑴 𝑼𝒀 = (𝒛𝒊 − 𝒛 𝒄) × (𝝈 𝒀𝒊 − 𝝈 𝒀)𝑨𝒊 𝝈 𝑿𝒊

24
 Nonlinear Behaviors of Real Structure
Concrete Cracked-elastic Stresses Stage Ultimate Stresses Stage
Euler-Bernoulli vs Timoshenko
Shear Deformation

25
3. Typical Boundary Conditions

26
Moment ConnectionsShear Connections
 Connection types of Frame Structure

27
All connections have a certain amount of rigidity
Simple connections (A above) have some rigidity,
but are assumed to be free to rotate
Partially-Restrained moment connections (B and C
above) are designed to be semi-rigid
Fully-Restrained moment connections (D and E
above) are designed to be fully rigid
 Rigidity of Each Connection Type
Source: AISC Teaching Aids - Connections and Bracing Configurations

28
 Result Changes due to Boundary Conditions
Displacement (Y Direction) Moment (Z Direction)

29
 Connecting Different Kinds of Elements
Connecting Shell toSolid (NoMoment Transferred) Connecting BeamtoShell (NoTorque Transferred)

30
Connecting beamelement toplane elements:
(a) no moment is transferred, (b) moment is transferred
 Connecting Different Kinds of Elements – cont.

31
Different Types of Structural Symmetry
 Structural Symmetry

32
 Applied Structural Symmetry
Modelling a cubic block with two planes of symmetry Problem reduction using axes of symmetry applied to
a plate with a hole subjected to tensile force

33
 Applied Structural Symmetry – cont.
Simply supported symmetric beam structure Simply supported anti-symmetric beam structure

34
 Rigid Corner of Frame Structure
Coupling, Offset, RigidMember, etc.
Source: Finite element design of concrete structures

35
 Constraint Equation
Every node tied togetherhas the same value for degree of freedom

36
 Loading Condition for Underground Tunnel Modeling
(Plus Dynamic Earth Pressure)

37
 Loading Condition for Underground Tunnel Modeling(Flooding)

38
 Result Changes due to Boundary Conditions
1. Fixed Condition
2. Vertical Springs
3. Compression-only VerticalSprings
3
2
1

39
 Horizontal Boundary Condition for Pile Modeling
FE Model and Distribution of Subgrade ReactionModulus
for Horizontal Force at Pile Head
 Piles can be modelled by linear-elastic supported beam
elements.
 The bedding modulus ks and the stiffness of the
horizontalsprings may vary along the length of the pile
and its circumference.
 Exponent n should be chosen as follows;
n Soil Condition
0 cohesive soilundersmall tomediumloads
0.5
mediumcohesive soil andnon-cohesivesoil
above groundwaterlevel
1
non-cohesive soil below groundwaterlevel
or undergreaterloads
1.5 to 2 loose non-cohesive soil underveryhighloads
𝒌 𝒔 𝒛 = 𝒌 𝒔 × 𝒅 × (𝒛/𝒅) 𝒏
Source: Finite element design of concrete structures

40
 Influence on Analysis Results by Stiffness of Vertical Spring
Bending moment distribution in pile
(horizontal load: 870 kN at column head)
Horizontal deformation of pile
(horizontal load: 870 kN at column head)

41
Pile Model with Strut-and-Tie - Foundation of Bridge Pier
Strut-and-tie Model for Pile Cap
 Strut-and-tie Model for Pile Cap

42
 Subgrade Modeling Using Solid Elements

43
X
Y
Z
B.C.:
SYMMETRIC
B.C.: UY=0
B.C.: UX=0
SUBGRADE ELEMENTS
CONCRETE ELEMENTS
L2 = 7.5 m
L1 = 5.0 m
FE Model for Parametric Study
Case Contact B.C. Load σx_top σx_bottom Moment Axial Force Remark
1 None Thermal ≒0 ≒0 ≒0 ≒0 No stress w/o constraint
2 Fixed
Gravity
Thermal
-2683.06 2673.64 446.39 ≒0
w/o Subgrade Elements
No axial force
3 Friction
Gravity
Thermal
-1310.53 1284.77 216.28 12.88
4 w/o Friction
Gravity
Thermal
-1316.63 1317.22 219.49 ≒0 No axial force
5 Merged
Gravity
Thermal
-2129.38 1730.25 321.64 -199.57
Parametric Study Results
 B.C. Effects in Thermal Structural Analysis

44
Case 1. w/ogravity,w/oFriction(σx) Case 2. w/gravity,w/oFriction(σx,FixedB.C.)
Case 3. w/gravity,w/Friction(σx) Case 4. w/gravity,w/oFriction(σx) Case 5. w/gravity,sharednodesonthe interface
surface of soil andconcrete (σx)
 B.C. Effects in Thermal Structural Analysis

46
Make nodes
Build elements by assigning connectivity
Apply boundary conditions and loads
4. Element Mesh Generation
 Bottom-up Method for Element Generation

47
 Geometrical Modeling Method for Element Generation
Geometrical Modeling
(a) Physical Geometry of Structural Parts
(b) Geometry Created in FE Model

48
 Basic Tips of Geometrical Modeling Method

49
It is important to remember that a finite element solution is an approximation:
• CAD geometry is an idealization of the physical model.
• The mesh is a combination of discreet “elements” representing the geometry.
• The accuracy of answers is determined by various factors, one of which is the mesh density.
 Modeling Method Using CAD Model
3D CAD Model Finite Element Model

50
 Modeling Method Using CAD Model – cont.
3D CAD Model Finite Element Model
Left View Right View

51
Navisworks Screenshotof FrameworksModel (Partof PDSModel)
X
Y
Z
3D IsometricViewof 3D Frame Model (STAAD.Prov8i)
3D RenderedIsometricViews (STAAD.Prov8i)

52
Automated Structural Analysis System
 Build 3D CAD Model
 Convert 3D CAD Model to Finite Element Model
 Generate Input Data Based on Load Database
 Under Development of Different Modules Specialized for Each
Structure

53
3D Shell Element Mesh Imported into FEA Program
Steel Concrete
Composite Column
Members
Steel Beam and
Girder Members

54
5. FE Analysis Boundary
Based on Structural Behavior

55
5. FE Analysis Boundary Based on Structural Behavior
 Plane Stress / Plane Strain Problems
Plane strain problems:
(a) dam subjected to horizontal loading
(b) pipe subjected to a vertical load
Plane stress problems:
(a) plate with hole; (b) plate with fillet
Source: A FIRST COURSE IN THE FINITE ELEMENT METHOD (Daryl L. Logan)

56
 Plane Stress / Plane Strain Problems – cont.
Plot of minimum principal stress with largest absolute value of 1.86 MPa located
on back side of dam subjected to both hydrostatic and self-weight loading
Mohr’s Circle for Plane Strain

57
Seepage Analysis – Potential Problem
Boundary Condition (left) and Hydraulic Head Contour (right)

58
Seepage Analysis – Potential Problem
Flow Velocity Vector (left) and Equipotential Lines (right)

59
 Modeling for Vessel Foundation
Shell FoundationModel
w/o Pedestal Stiffness
Shell FoundationModel
withSolidPedestal
SolidFoundationModel withSolidPedestal

60
+
Compression-only Soil Spring
Fixed B.C. for Shell Foundation
(or Hinge B.C. for Solid Foundation)
Shell Elements
Foundation
Beam Elements
Support Frame
LinearSystemforDynamicAnalysis
NonlinearSystemforStaticAnalysis
Rigid Link
Vessel Mass
 Linear & Nonlinear System Modeling

61
 Linear & Nonlinear System Modeling – cont. (Super-structure)
Stack +AB (Modal-05)
TYPE MASS (1000 kg)
1 680.891 Stack Shell
2 20.077 Stack Beam
3 524794.000 AB Shell
4 1618.620 AB Beam
527113.588
DecouplingCriteriaforSubsystems U.S.NRCSPR 3.7.2
 If Rm < 0.01, decouplingcanbe done forany Rf.
 If 0.01 < Rm < 0.1, decouplingcanbe done if 0.8 > Rf > 1.25.
 If Rm > 0.1, a subsystemmodelshouldbe includedinthe primarysystem
model.
Rm = Total massof supportedsubsystem/Dominantmassof supporting system
Rf = Total mass of supportedsubsystem/Dominantmassof supportingsystem

62
 Linear & Nonlinear System Modeling – cont. (Foundation)
ModelingConcept
 SelectedSolidElementstoConsiderVarious
ThicknessChanges
 AppliedCompression-onlySpringforSimulating
Uplifting
 CoupledSuper-structure withZeroDensitytoUse
ItsStiffness
NonlinearSystemforStaticAnalysis

63
6. Examples of B.C. Applications

64
Analysis Models and B.C. Application
Based on Structural Behaviors

65
 Global FE Model (Preliminary)
 To Check Stability and Structural Behavior
 Compress-only Springs Used to Consider
Buoyancy
 Loading Condition:
Self-weight, Soil Pressure, Buoyancy

66
2D Model (2 EA)
Plane Strain Behavior
3D Model (9 EA)
3D Structural Behavior
 Structural Component
for FE Modeling and Analysis (Design Purpose)
Each structural component should be isolated to match actual structural behaviors to
the assumed in splitting the entire structure. In this case, expansion joints are arranged
for the purpose.

67

68
Thermal Structural Analysis
Using Nonlinear Frictional Contact

69
 Thermal Structural Analysis to Determine
MaximumSpacing between Expansion Joints
 Analysis Boundary: Separated Bay (Orange-colored)
 Seasonal Change in Temperature (Case 1) :
T0 (ref. temp)=27.5℃, △T= -22.5℃ (Ambient Air)
 Daily Change in Temperature (Case 2):
T0 (ref. temp)=40.0℃, △T= +22.5℃ (Solar Radiation)
 Boundary Condition:
Accounts for Friction Effects between Concrete and
Subgrade

70
Type of Building Outside Temperature Variations Maximum Joint Spacing (ft)
Heated
Up to 70°F
Above 70°F
600 (182.88 m)
400-500 (121.92 ~152.4 m)
Unheated
Up to 70°F
Above 70°F
300 (91.44 m)
200 (60.96 m)
Mark Fintel, Section 4.10.2, "Spacing of Expansion Joints", Handbook of Concrete
Engineering, pp. 129-130.
ACI Report: Building Movements and Joints, EB086.01B.
Buildings of more than 600 ft (183 m) have been constructed and performed satisfactorily withoutexpansion
joints. The possible need for thermalexpansion jointsin long buildings may be determined initially using the
empiricalapproach described in the following section. Previously developed empiricalrulesfor expansion joint
spacing are not necessarily compatible with modern construction. Therefore, effectsof thermaland other volume
changesshould be determined aspartof the structuralanalysis.If results of the empiricalapproach indicate an
expansion jointmay be needed, a more comprehensive analysiscan be done to determine if use of expansion
joints can be avoided.
 Maximum Spacing between Expansion Joints

71
Thermal Loading Condition due to Solar Radiation
Temperature Distribution through Cross Section of Aeration Channel
Temperature Distribution through Aeration Channel
 Design Temperature Condition

72
Nonlinear Frictional Contact between Concrete and Subgrade Parts
 Nonlinear Contact Boundary Condition

73
 Model Verification
Total Deformation under Thermal Load only (ISO View)
This condition cannot occur in the real loading cases under gravity, but it has to be
checked to verify nonlinear contact boundary condition.

74
 Analysis Results
Total Deformation under Thermal Load and Self-weight

75
Normal Stress in Global Z Direction
Normal Stress in Global Z Direction (Upside Down)
 Analysis Results

Application of Boundary Conditions to Obtain Better FEA Results

Recomendados

Recomendados

Mais conteúdo relacionado

Mais procurados

Mais procurados (20)

Semelhante a Application of Boundary Conditions to Obtain Better FEA Results

Semelhante a Application of Boundary Conditions to Obtain Better FEA Results (20)

Último

Último (20)

Application of Boundary Conditions to Obtain Better FEA Results