Download Fem stress concepts and more Study notes Applied Mechanics in PDF only on Docsity!
3 Concepts of Stress Analysis
3.1 Introduction
Here the concepts of stress analysis will be stated in a finite element context. That means that the primary unknown will be the (generalized) displacements. All other items of interest will mainly depend on the gradient of the displacements and therefore will be less accurate than the displacements. Stress analysis covers several common special cases to be mentioned later. Here only two formulations will be considered initially. They are the solid continuum form and the shell form. Both are offered in SW Simulation. They differ in that the continuum form utilizes only displacement vectors, while the shell form utilizes displacement vectors and infinitesimal rotation vectors at the element nodes.
As illustrated in Figure 3 ‐1, the solid elements have three translational degrees of freedom (DOF) as nodal unknowns, for a total of 12 or 30 DOF. The shell elements have three translational degrees of freedom as well as three rotational degrees of freedom, for a total of 18 or 36 DOF. The difference in DOF types means that moments or couples can only be applied directly to shell models. Solid elements require that couples be indirectly applied by specifying a pair of equivalent pressure distributions, or an equivalent pair of equal and opposite forces at two nodes on the body.
Shell node Solid node Figure 3 ‐ 1 Nodal degrees of freedom for frames and shells; solids and trusses
Stress transfer takes place within, and on, the boundaries of a solid body. The displacement vector , u , at any point in the continuum body has the units of meters [m], and its components are the primary unknowns. The components of displacement are usually called u, v, and w in the x, y, and z‐directions, respectively. Therefore, they imply the existence of each other, u ↔ (u, v, w). All the displacement components vary over space. As in the heat transfer case (covered later), the gradients of those components are needed but only as an intermediate quantity. The displacement gradients have the units of [m/m], or are considered dimensionless. Unlike the heat transfer case where the gradient is used directly, in stress analysis the multiple components of the displacement gradients are combined into alternate forms called strains. The strains have geometrical interpretations that are summarized in Figure 3 ‐ 2 for 1D and 2D geometry.
In 1D, the normal strain is just the ratio of the change in length over the original length, εx = ∂u / ∂x. In 2D and 3D, both normal strains and shear strains exist. The normal strains involve only the part of the gradient terms parallel to the displacement component. In 2D they are εx = ∂u / ∂x and εy = ∂v / ∂y. As seen in Figure 3 ‐ 2 (b), they would cause a change in volume, but not a change in shape of the rectangular differential element. A shear strain causes a change in shape. The total angle change (from 90 degrees) is used as the engineering definition of the shear strain. The shear strains involve a combination of the components of the gradient that
are perpendicular to the displacement component. In 2D, the engineering shear strain is γ = (∂u / ∂y + ∂v / ∂x), as seen in Figure 3 ‐2(c). Strain has one component in 1D, three components in 2D, and six components in
3D. The 2D strains are commonly written as a column vector in finite element analysis, ε = (εx εy γ)T^.
Figure 3 ‐ 2 Geometry of normal strain (a) 1D, (b) 2D, and (c) 2D shear strain
Stress is a measure of the force per unit area acting on a plane passing through the point of interest in a body. The above geometrical data (the strains) will be multiplied by material properties to define a new physical quantity, the stress , which is directly proportional to the strains. This is known as Hooke’s Law : σ = E ε, (see Figure 3 ‐ 3 ) where the square material matrix , E , contains the elastic modulus, and Poisson’s ratio of the material. The 2D stresses are written as a corresponding column vector, σ = ( σ x σ y τ)T^. Unless stated otherwise, the applications illustrated here are assume to be in the linear range of a material property.
The 2D and 3D stress components are shown in Figure 3 ‐4. The normal and shear stresses represent the normal force per unit area and the tangential forces per unit area, respectively. They have the units of [N/m^2], or [Pa], but are usually given in [MPa]. The generalizations of the engineering strain definitions are seen in Figure 3 ‐5. The strain energy (or potential energy ) stored in the differential material element is half the scalar product of the stresses and the strains. Error estimates from stress studies are based on primarily on the strain energy (or strain energy density).
Figure 3 ‐ 3 Hooke's Law for linear stress‐strain, σ = E ε
from zero at the support to a maximum of δ at the load point. That is, u (x) = x δ / L , so the axial strain is εx = ∂u
/ ∂x = δ / L , which is a constant. Likewise, the axial stress is everywhere constant, σ = E ε = E δ / L which in the
case simply reduces to σ = P / A. Like many other more complicated problems, the stress here does not depend on the material properties, but the displacement always does, ܣܧ ܮ ܲൌ ߜ⁄. You should always carefully check both the deflections and stresses when validating a finite element solution.
Since the assumed displacement is linear here, any finite element model would give exact deflection and the constant stress results. However, if the load had been the distributed bar weight the exact displacement would be quadratic in x and the stress would be linear in x. Then, a quadratic element mesh would give exact stresses and displacements everywhere, but a linear element mesh would not.
The elastic bar is often modeled as a linear spring. In introductory mechanics of materials the axial stiffness of a bar is defined as k = E A / L , where the bar has a length of L , an area A , and is constructed of a material elastic modulus of E. Then the above bar displacement can be written as ݇ܲൌ ߜ ⁄^ , like a linear spring.
σ = P / A, δ = P L / E A Figure 3 ‐ 6 A linearly elastic bar with an axial load
3.3 Structural mechanics
Modern structural analysis relies extensively on the finite element method. The most popular integral formulation, based on the variational calculus of Euler, is the Principle of Minimum Total Potential Energy. Basically, it states that the displacement field that satisfies the essential displacement boundary conditions and minimizes the total potential energy is the one that corresponds to the state of static equilibrium. This implies that displacements are our primary unknowns. They will be interpolated in space as will their derivatives, and the strains. The total potential energy, Π, is the strain energy, U, of the structure minus the mechanical work, W, done by the external forces. From introductory mechanics, the mechanical work, W, done by a force is the scalar dot product of the force vector, F , and the displacement vector, u , at its point of application.
The well‐known linear elastic spring will be reviewed to illustrate the concept of obtaining equilibrium equations from an energy formulation. Consider a linear spring, of stiffness k , that has an applied force, F , at the free (right) end, and is restrained from displacement at the other (left) end. The free end undergoes a displacement of Δ. The work done by the single force is
The spring stores potential energy due to its deformation (change in length). Here we call that strain energy. That stored energy is given by
Therefore, the total potential energy for the loaded spring is
∆ ௫ଶ^ െ ∆ ௫ ܨ௫
The equation of equilibrium is obtained by minimizing this total potential energy with respect to the unknown displacement, ∆ (^) ௫. That is,
߲߲ߎ ∆ (^) ௫
This simplifies to the common single scalar equation
k ∆௫ = F ,
which is the well‐known equilibrium equation for a linear spring. This example was slightly simplified, since we started with the condition that the left end of the spring had no displacement (an essential or Dirichlet boundary condition). Next we will consider a spring where either end can be fixed or free to move. This will require that you both minimize the total potential energy and impose the given displacement restraint.
Figure 3 ‐ 7 The classic and general linear spring element
Now the spring model has two end displacements, ∆ 1 and ∆ 2 , and two associated axial forces, F 1 and F 2. The
net deformation of the bar is δ = ∆ 2 ‐ ∆ 1. Denote the total vector of displacement components as
and the associated vector of forces as
Then the mechanical work done on the spring is
ܹ ൌ ሼ∆ሽ் ሼܨሽ ൌ ∆ 1 F 1 + ∆ 2 F 2
Then the spring's strain energy is
ଵ
ଶ ሼ∆ሽ்^ ሾ ݇ሿ ሼ∆ሽ ൌ^
ଵ
݇ଶ ߜ^
where the “spring stiffness matrix” is found to be
The total potential energy, Π, becomes
ଵ
ଶ ሼ∆ሽ்^ ሾ ݇ሿ ሼ∆ሽ െ^ ሼ∆ሽ்^ ሼܨሽ ൌ^
Note that each term has the units of energy, i.e. force times length. The matrix equations of equilibrium come from satisfying the displacement restraint and the minimization of the total potential energy with respect to
3.5 General equilibrium matrix partitions
The above small example gives insight to the most general form of the algebraic system resulting from only minimizing the total potential energy: a singular matrix system with more unknowns than equations. That is because there is not a unique equilibrium solution to the problem until you also apply the essential (Dirichlet) boundary conditions on the displacements. The algebraic system can be written in a general partitioned matrix form that more clearly defines what must be done to reduce the system to a solvable form by utilizing essential boundary conditions.
For an elastic system of any size, the full, symmetric matrix equations obtained by minimizing the energy can always be rearranged into the following partitioned matrix form:
where ∆ u represents the unknown nodal displacements, and ∆ g represents the given essential boundary values
(restraints, or fixtures) of the other displacements. The stiffness sub‐matrices Kuu and Kgg are square, whereas Kug and Kgu are rectangular. In a finite element formulation all of the coefficients in the K matrices are known. The resultant applied nodal loads are in sub‐vector F (^) g and the Fu terms represent the unknown generalized reactions forces associated with essential boundary conditions. This means that after the enforcement of the
essential boundary conditions the actual remaining unknowns are ∆ u and F u. Only then does the net number
of unknowns correspond to the number of equations. But, they must be re‐arranged before all the remaining unknowns can be computed.
Here, for simplicity, it has been assumed that the equations have been numbered in a manner that places rows associated with the given displacements (essential boundary conditions) at the end of the system equations. The above matrix relations can be rewritten as two sets of matrix identities:
The first identity can be solved for the unknown displacements, ࢛∆ , by putting it in the standard linear
equation form by moving the known product ࢛ࡷࢍ ∆ ࢍ to the right side. Most books on numerical analysis
assume that you have reduced the system to this smaller, nonsingular form (࢛࢛ࡷ ) before trying to solve the
system. Inverting the smaller non‐singular square matrix yields the unique equilibrium displacement field:
࢛∆ ି࢛࢛ࡷ ൌ ^ ࡲ൫ ࢍ ࢛ࡷ െࢍ ∆ࢍ ൯.
The remaining reaction forces can then be recovered, if desired, from the second matrix identity:
࢛ࡲ ࡷ ൌ࢛ࢍ ࢛∆ ࡷ ࢍࢍ ∆ࢍ.
In most applications, these reaction data have physical meanings that are important in their own right, or useful in validating the solution. However, this part of the calculation is optional.
3.6 Structural Component Failure
Structural components can be determined to fail by various modes determined by buckling, deflection, natural frequency, strain, or stress. Strain or stress failure criteria are different depending on whether they are considered as brittle or ductile materials. The difference between brittle and ductile material behaviors is determined by their response to a uniaxial stress‐strain test, as in Figure 3 ‐8. You need to know what class of material is being used. SW Simulation, and most finite element systems, default to assuming a ductile material
and display the distortional energy failure theory which is usually called the Von Mises stress, or effective stress, even though it is actually a scalar. A brittle material requires the use of a higher factor of safety.
Figure 3 ‐ 8 Axial stress‐strain experimental results
3.7 Factor of Safety
All aspects of a design have some degree of uncertainty, as does how the design will actually be utilized. For all the reasons cited above, you must always employ a Factor of Safety (FOS). Some designers refer to it as the factor of ignorance. Remember that a FOS of unity means that failure is eminent; it does not mean that a part or assembly is safe. In practice you should try to justify 1 < FOS < 8. Several consistent approaches for computing a FOS are given in mechanical design books [9]. They should be supplemented with the additional uncertainties that come from a FEA. Many authors suggest that the factor of safety should be computed as the product of terms that are all 1. There is a factor for the certainty of the restraint location and type; the certainty of the load region, type, and value; a material factor; a dynamic loading factor; a cyclic (fatigue) load factor; and an additional factor if failure is likely to result in human injury. Various professional organizations and standards organizations set minimum values for the factor of safety. For example, the standard for lifting hoists and elevators require a minimum FOS of 4, because their failure would involve the clear risk of injuring or killing people. As a guide, consider the FOS as a product of factors: ൌ ܱܵܨ ∏^ ୀଵ ܨܨ ൌଵ ܨଶ ܨଷ ܨ …. A set of typical factors is given inTable 3 ‐1.
Table 3 ‐ 1 Factors to consider when evaluating a design (each )
k Type Comments
1 Consequences Will loss be okay, critical or fatal
2 Environment Room‐ambient or harsh chemicals present
3 Failure theory Is a part clearly brittle, ductile, or unknown 4 Fatigue Does the design experience more that ten cycles of use
5 Geometry of Part Not uncertain, if from a CAD system
FEA Concepts
Draft
3.9 SW S The symbols u Figure 3 ‐10. T element solut represents the are often refe displacement enough restra
N
Al
For simplicity That is, they the type of re frequently en understand s
s: SW Simula
13.0. Copyri
Simulation used in SW Sim The symbols fo ions are based e mechanical w rred to as gene DOF’s for the s ints to prevent
Node of solid l three displa
F
y many finite enforce an Im estraint, as w ncounter the symmetry pla
Displaceme Figu
ation Overview
ght 2009. All
Figure 3
Fixture an mulation to repr r the correspo d on work‐ener work done at th eralized displac solid nodes (to t any model fro
or truss elem acements are
Figure 3 ‐ 10 Fix
element exam mmovable co well as where t common con ane restraints
ent ure 3 ‐ 11 Single
w
l rights reserv
‐ 9 Overlappin
nd Load Sy resent a single nding forces a rgy relations, th he point. Whe cements. The op) and shell no om undergoing
ment: zero.
xed restraint sy
mples incorre ondition for so the part is re nditions of sym for solids an
Force e component s
ved.
ng valid ranges
ymbols e translational a nd moment lo he above word en a model can SW Simulation odes are seen g a rigid body t
ymbols for sol
ectly apply co olids or a Fixe strained is of mmetry or an d shells.
Rot symbols for res
s of element ty
and rotational adings are sho d “correspondi n involve either n nodal symbo in Figure 3 ‐11. translation or
Node of f All three di ro ids (top) and s
omplete restr ed condition f ften the most nti‐symmetry
tation straints (fixtur
ypes
DOF at a node own pink in tha ng” means tha r translations o ls for the unkn
. You almost a rigid body rota
frame or shel splacements otations are ze shell nodes
aints at a face for shells. Ac t difficult part y restraints. Y
Coup res) and loads
J
e are shown gr at figure. Since at their dot pro or rotations as nown generaliz always must su ation.
ll element: and all three ero.
e, edge or no tually determ t of an analys You should un
le
.E. Akin
reen in e finite oduct DOF they zed upply
ode. mining is. You nder
3.10 Symmetry DOF on a Plane
A plane of symmetry is flat and has mirror image geometry, material properties, loading, and restraints. Symmetry restraints\i are very common for solids and for shells. Figure 3 ‐ 12 shows that for both solids and shells, the displacement perpendicular to the symmetry plane is zero. Shells have the additional condition that the in‐plane component of its rotation vector is zero. Of course, the flat symmetry plane conditions can be stated in a different way. For a solid element translational displacements parallel to the symmetry plane are allowed. For a shell element rotation is allowed about an axis perpendicular to the symmetry plane and its translational displacements parallel to the symmetry plane are also allowed.
Node of a solid or truss element: Displacement normal to the symmetry plane is zero.
Node of a frame or shell element: Displacement normal to the symmetry plane and two rotations parallel to it are zero. Figure 3 ‐ 12 Symmetry requires zero normal displacement, and zero in‐plane rotation
3.11 Available Loading (Source) Options
Most finite element systems have a wide range of mechanical loads (or sources) that can be applied to points, curves, surfaces, and volumes. The mechanical loading terminology used in SW Simulation is in Table 3 ‐2. Most of those loading options are utilized in later example applications.
Table 3 ‐ 2 Mechanical loads (sources) that apply to the active structural study
Load Type Description Bearing Load Non‐uniform bearing load on a cylindrical face
Centrifugal Force Radial centrifugal body forces for the angular velocity and/or tangential body forces from the angular acceleration about an axis
Force Resultant force, or moment, at a vertex, curve, or surface
Gravity Gravity, or linear acceleration vector, body force loading
Pressure A pressure having normal and/or tangential components acting on a selected surface
Remote Load / Mass
Allows loads or masses remote from the part to be applied to the part by treating the omitted material as rigid
Temperature Temperature change at selected curves, surfaces, or bodies (see thermal studies for more realistic temperature transfers)
3.12 Available Material Inputs for Stress Studies
Most applications involve the use of isotropic (direction independent) materials. The available mechanical properties for them in SW Simulation are listed in Table 3 ‐3. It is becoming more common to have designs utilizing anisotropic (direction dependent) materials. The most common special case of anisotropic materials is the orthotropic material. Any anisotropic material has its properties input relative to the principal directions of the material. That means you must construct the principal material directions reference plane or coordinate axes before entering orthotropic data. Mechanical orthotropic properties are subject to some theoretical
Figure 3 ‐ 13 Example of a four‐ply laminate material
3.13 Stress Study Outputs
A successful run of a study will create a large amount of additional output results that can be displayed and/or listed in the post‐processing phase. Displacements are the primary unknown in a SW Simulation stress study. The available displacement vector components are cited in Table 3 ‐ 5 and Table 3 ‐6, along with the reactions they create if the displacement is used as a restraint. The displacements can be plotted as vector displays, or contour values. They can also be transformed to cylindrical or spherical components.
Table 3 ‐ 5 Output results for solids, shells, and trusses Symbol Label Item Symbol Label Item Ux UX Displacement (X direction) Rx RFX Reaction force (X direction) Uy UY Displacement (Y direction) Ry RFY: Reaction force (Y direction) Uz UZ Displacement (Z direction) Rz RFZ Reaction force (Z direction) Ur URES: Resultant displacement magnitude
Rr RFRES Resultant reaction force magnitude
Table 3 ‐ 6 Additional primary results for beams, plates, and shells Symbol Label Item Symbol Label Item θ x RX Rotation (X direction) Mx RMX: Reaction moment (X direction) θ y RY Rotation (Y direction) My RMY Reaction moment (Y direction) θ z RZ Rotation (Z direction) Mz RMZ: Reaction moment (Z direction) Mr MRESR Resultant reaction moment magnitude
The strains and stresses are computed from the displacements. The stress components available at an element centroid or averaged at a node are given in Table 3 ‐7. The six components listed on the left in that table give the general stress at a point (i.e., a node or an element centroid). Those six values are illustrated on the left of Figure 3 ‐14. They can be used to compute the scalar von Mises failure criterion. They can also be used to solve an eigenvalue problem for the principal normal stresses and their directions, which are shown on the right of Figure 3 ‐14. The maximum shear stress occurs on a plane whose normal is 45 degrees from the direction of P1. The principal normal stresses can also be used to compute the scalar von Mises failure criterion.
The von Mises effective stress is compared to the material yield stress for ductile materials. Failure is predicted to occur (based on the distortional energy stored in the material) when the von Mises value reaches the yield stress. The maximum shear stress is predicted to cause failure when it reaches half the yield stress. SW Simulation uses the shear stress intensity which is also compared to the yield stress to determine failure
(because it is twice the maximum shear stress). The first four values on the right side of Table 3 ‐ 7 are often represented graphically in mechanics as a 3D Mohr’s circle (seen in Figure 3 ‐15).
Table 3 ‐7: Nodal and element stress results Symbol Label Item Symbol Label Item σ x SX Normal stress parallel to x‐axis σ 1 P1 1st principal normal stress σ y SY Normal stress parallel to y‐axis σ 2 P2 2nd principal normal stress σ z SZ Normal stress parallel to z‐axis σ 3 P3 3rd principal normal stress τ xy TXY Shear in Y direction on plane normal to x‐axis
τI INT Stress intensity (P1‐P3), twice the maximum shear stress τ xz TXZ Shear in Z direction on plane normal to x‐axis τ yz TYZ Shear in Z direction on plane normal to z‐axis
σ vm VON von Mises stress (distortional energy failure criterion)
Figure 3 ‐ 14 The stress tensor (left) and its principal normal values
Figure 3 ‐ 15 The three‐dimensional Mohr's circle of stress yield the principal stresses
Table 3 ‐ 9 Additional element centroid stress related results Label Item ERR Element error measured in the strain energy norm CP Contract pressure developed on a contact surface
