김경종
26 KiB
Now
\mathbf {n} d A = \mathbf {k} \times \frac {\partial \mathbf {x}}{\partial g} t d g,
where \mathbf { k } = ( 0 , 0 , 1 ) is a unit vector out of the plane of the model, t is the thickness of the two-dimensional solid (which is assumed to be constant), and the surface parametric coordinate g is chosen to give the correct sign to n through the cross product. The external work is then given by
\delta W ^ {E} = \int_ {g} p \delta \mathbf {u} \cdot \mathbf {k} \times \frac {\partial \mathbf {x}}{\partial g} t d g,
and the load stiffness matrix is obtained from
- d \delta W ^ {E} = - \int_ {g} p \delta \mathbf {u} \cdot \mathbf {k} \times \frac {\partial d \mathbf {u}}{\partial g} t d g.
3.3 Infinite elements
3.3.1 Solid infinite elements
The stress analyst is often faced with problems defined in unbounded domains or problems in which the region of interest is small compared with the surrounding medium. The unbounded or infinite medium can be approximated by extending the finite element mesh to a far distance, where the influence of the surrounding medium on the region of interest is considered small enough to be neglected. This approach calls for experimentation with mesh sizes and assumed boundary conditions at the truncated edges of the mesh and is not always reliable. It is particularly of concern in dynamic analysis, when the boundary of the mesh may reflect energy back into the region being modeled. A better approach is to use "infinite elements": elements defined over semi-infinite domains with suitably chosen decay functions. ABAQUS provides first- and second-order infinite elements that are based on the work of Zienkiewicz et al. (1983) for static response and of Lysmer and Kuhlemeyer (1969) for dynamic response. The elements are used in conjunction with standard finite elements, which model the area around the region of interest, with the infinite elements modeling the far-field region.
Static analysis
The solution in the far field is assumed to be linear, so only linear behavior is provided in the infinite elements. The static behavior of the infinite elements is based on modeling the basic solution variable, u (in stress analysis u is a displacement component) with respect to spatial distance r measured from a "pole" of the solution, so that u \to 0 as r \infty . , and u \infty { \mathrm { a s } } r 0 . The interpolation provides terms of order 1 / r , 1 / r ^ { 2 } , and, when the solution variable is a stress-like variable (such as the pore liquid pressure in the analysis of flow through a porous medium), 1 / r ^ { 3 } as r \to 0 . The far-field behavior of many common cases, such as a point load on a half-space, is thereby included. This modeling is achieved by using standard quadratic or cubic interpolation for u ( s ) in - 1 \leq s \leq 1 , where s is a mapped coordinate that is chosen such that the mapping r ( s ) causes r \to \infty { \mathrm { a s ~ } } s \to 1 . We
Elements
obtain two- and three-dimensional models of domains that reach to infinity by combining this interpolation in the s-direction in a product form with standard linear or quadratic interpolation in orthogonal directions in the mapped space.
In using infinite elements for static analysis, the pole must be located so as to provide a reasonable far-field solution for the particular problem being modeled. The infinite elements in ABAQUS are written with nodes on the interface between the finite and infinite elements and, on each edge that stretches to infinity, a node that must be placed in the infinite direction such that the straight line from that node through the corresponding interface node passes through the pole for that ray at a distance on the other side of the interface from the infinite element equal to the distance between these nodes (Figure 3.3.1-1).
Figure 3.3.1-1 Pole node location for an infinite element.
text_image
r a a 1 2 3 r₀ r₁ r₂ r₃ ∞ 1 2 3 s = -1 s = 0 s = +1
The one-dimensional concept is, thus, based on a node (node 1) on the interface between the finite and infinite elements, distance r _ { 1 } = a from the pole and at s = - 1 in the mapped space, and node 2, at r _ { 2 } = 2 a from the pole (the pole is at r = 0 ) and at s = 0 is the mapped space. The r ( s ) mapping is chosen as
r = - \frac {2 s}{1 - s} r _ {1} + \frac {1 + s}{1 - s} r _ {2},
so that
r = \frac {2 a}{1 - s},
which inverts to give
s = 1 - \frac {2 a}{r}.
Elements
When an element with 1 / r and 1 / r ^ { 2 } behavior is required, we combine this geometric mapping with standard quadratic interpolation of u with respect to s, written in terms of its values at node 1 and at node 2:
u = \frac {1}{2} s (s - 1) u _ {1} + (1 - s ^ {2}) u _ {2}
(this gives u = 0 at s = 1 , where r \infty ) . Using the inverted geometric mapping to define u ( r ) then gives
u = (- u _ {1} + 4 u _ {2}) \frac {a}{r} + (2 u _ {1} - 4 u _ {2}) \left(\frac {a}{r}\right) ^ {2},
which provides the desired behavior. Likewise, when 1 / r ^ { 3 } behavior is also required, we use cubic interpolation of u with respect to s, written in terms of its values at nodes 1 and 2 and at a third node, which we choose to place at \begin{array} { r } { s = \frac { 1 } { 2 } } \end{array} :
u = - \frac {1}{3} s (s - 1) (s - \frac {1}{2}) u _ {1} - 2 (1 - s ^ {2}) (s - \frac {1}{2}) u _ {2} + \frac {8}{3} s (1 - s ^ {2}) u _ {3}.
The inverted geometric mapping then provides
u = (\frac {1}{3} u _ {1} - 4 u _ {2} + \frac {3 2}{3} u _ {3}) \frac {a}{r} + (- 2 u _ {1} + 2 0 u _ {2} - 3 2 u _ {3}) \left(\frac {a}{r}\right) ^ {2} + (\frac {8}{3} u _ {1} - 1 6 u _ {2} + \frac {6 4}{3} u _ {3}) \left(\frac {a}{r}\right) ^ {3}.
The infinite elements in ABAQUS consist of two- and three-dimensional elements for uncoupled stress analysis that use quadratic interpolation for displacement components and two- and three-dimensional elements for coupled stress-pore liquid pressure elements, in which the displacements use quadratic interpolation and the pore liquid pressure uses cubic interpolation in the infinite direction. This higher-order interpolation is used for the pore liquid pressure for compatibility: since the displacement varies as 1 / r ^ { 2 } , the strain (and, therefore, the stress) may vary as 1 / r ^ { 3 } .
Dynamic response
The dynamic response of the infinite elements is based on consideration of plane body waves traveling orthogonally to the boundary. Again, we assume the response adjacent to the boundary is of small enough amplitude so that the medium responds in a linear elastic fashion.
The equilibrium equation is
- \rho \ddot {\mathbf {u}} + \frac {\partial}{\partial \mathbf {x}} \cdot \pmb {\sigma} = 0,
where \rho is the material's density, uÄ is the material particle acceleration, \pmb { \sigma } is the stress, and x is position.
We assume the material's response is isotropic, linear elastic, and--thus--can be written as
Elements
\boldsymbol {\sigma} = \lambda \mathbf {I} \mathbf {I}: \varepsilon + 2 G \varepsilon ,
where " is the strain and
\lambda = \frac {E \nu}{(1 + \nu) (1 - 2 \nu)}
and
G = \frac {E}{2 (1 + \nu)}
are Lamé's constants (E is Young's modulus and º is Poisson's ratio). Introducing this material response in the equilibrium equation, and assuming small strain:
\boldsymbol {\varepsilon} = \frac {1}{2} \left\{\frac {\partial \mathbf {u}}{\partial \mathbf {x}} + \left[ \frac {\partial \mathbf {u}}{\partial \mathbf {x}} \right] ^ {T} \right\},
provides the governing equation for the motion
\rho \ddot {u} _ {i} = G \frac {\partial^ {2} u _ {i}}{\partial x _ {j} \partial x _ {j}} + (\lambda + G) \frac {\partial^ {2} u _ {j}}{\partial x _ {i} \partial x _ {j}},
where index notation has been used for simplicity.
We consider plane waves traveling along the x-axis. Two body wave solutions of this form exist for this equation. One describes plane, longitudinal ("push") waves, which have the form
u _ {x} = f (x \pm c _ {p} t), \quad u _ {y} = u _ {z} = 0,
where, by substitution in the governing equation above, we find that the wave speed, c _ { p } { \mathrm { : } } , is
c _ {p} = \sqrt {\frac {\lambda + 2 G}{\rho}}.
The other solution of this form is the "shear" wave solution
u _ {y} = f (x \pm c _ {s} t), \quad u _ {x} = u _ {z} = 0
or
u _ {z} = f (x \pm c _ {s} t), \quad u _ {x} = u _ {y} = 0,
where--again by substitution in the governing equation--we obtain
Elements
c _ {s} = \sqrt {\frac {G}{\rho}}.
In each case the solution f ( x - c t ) represents waves moving in the direction of increasing x , while f ( x + c t ) represents waves moving in the direction of decreasing x.
Now consider a boundary at x = L of a medium modeled by finite elements in x < L . We introduce distributed damping on this boundary, such that
\sigma_ {x x} = - d _ {p} \dot {u} _ {x}
and
\sigma_ {x y} = - d _ {s} \dot {u} _ {y}
\sigma_ {x z} = - d _ {s} \dot {u} _ {z},
where we will now choose the damping constants d _ { p } and d _ { s } to avoid reflection of longitudinal and shear wave energy back into the medium in x < L . Plane, longitudinal waves approaching the boundary have the form u _ { x } = f _ { 1 } ( x - c _ { p } t ) , u _ { y } = u _ { z } = 0 . If they are reflected at all as plane, longitudinal waves, their reflection will travel away from the boundary in some form u _ { x } = f _ { 2 } ( x + c _ { p } t ) , u _ { y } = u _ { z } = 0 . Since the problem is linear, superposition provides the total displacement f _ { 1 } + f _ { 2 } , with corresponding stresses \sigma _ { x x } = ( \lambda + 2 G ) ( f _ { 1 } ^ { \prime } + f _ { 2 } ^ { \prime } ) , all other \sigma _ { i j } = 0 , and velocity \dot { u } _ { x } = - c _ { p } ( f _ { 1 } ^ { \prime } - f _ { 2 } ^ { \prime } ) . For this solution to satisfy the damping behavior introduced on the boundary at x = L requires
(\lambda + 2 G - d _ {p} c _ {p}) f _ {1} ^ {\prime} + (\lambda + 2 G + d _ {p} c _ {p}) f _ {2} ^ {\prime} = 0.
We can, therefore, ensure that f _ { 2 } = 0 (so that f _ { 2 } ^ { \prime } = 0 ) for any f _ { 1 } by choosing
d _ {p} = \frac {\lambda + 2 G}{c _ {p}} = \rho c _ {p}.
A similar argument for shear waves provides
d _ {s} = \rho c _ {s}.
These values of boundary damping are built into the infinite elements in ABAQUS. From the above discussion we see that they transmit all normally impinging plane body waves exactly (provided that the material behavior close to the boundary is linear elastic). General problems involve nonplane body waves that do not impinge on the boundary from an orthogonal direction and may also involve Rayleigh surface waves and Love waves. Nevertheless, these "quiet" boundaries work quite well even for such general cases, provided that they are arranged so that the dominant direction of wave propagation is orthogonal to the boundary or, at free surfaces and interfaces where Rayleigh or Love
Elements
waves are of concern, they are orthogonal to the surface (see, for example, Cohen and Jennings, 1983). As the boundaries are "quiet" rather than silent (perfect transmitters of all waveforms), and because the boundaries rely on the solution adjacent to them being linear elastic, they should be placed some reasonable distance from the region of main interest.
During dynamic response analysis following static preload (as is common in geotechnical applications), the traction provided by the infinite elements to the boundary of the finite element mesh consists of the constant stress obtained from the static response with the quiet boundary damping stress added. Since the elements have no stiffness during dynamic analysis, they allow a net rigid body motion to occur, which is usually not a significant effect.
3.4 Membrane and truss elements
3.4.1 Membrane elements
Membrane elements are sheets in space that can carry membrane force but do not have any bending or transverse shear stiffness, so the only nonzero stress components in the membrane are those components parallel to the middle surface of the membrane: the membrane is in a state of plane stress.
At any time we use a local orthonormal basis system \mathbf { e } _ { i } , where \mathbf { e } _ { 1 } and \mathbf { e } _ { 2 } are in the surface of the membrane and \mathbf { e } _ { 3 } is normal to the membrane. The basis system is defined by the standard convention used in ABAQUS for a basis on a surface in space. In this section Greek indices take the range 1, 2, and Latin indices take the range 1, 2, 3. Greek indices are used to refer to components in the first two directions of the local orthonormal basis (in the surface of the membrane).
Equilibrium
The virtual work contribution from the internal forces in a membrane element is
Equation 3.4.1-1
\delta W ^ {I} = \int_ {V} \pmb {\sigma}: \delta \pmb {\varepsilon} d V,
where \pmb { \sigma } is the Cauchy stress, \delta \pmb { \varepsilon } = \operatorname { s y m } ( \delta \mathbf { L } ) is the virtual rate of deformation ( \delta \mathbf { L } = \partial \delta \mathbf { u } / \partial \mathbf { x } , where ±u is the virtual velocity field), and V is the current volume of the membrane.
We assume that only the membrane stress components in the surface of the membrane are nonzero: \sigma _ { 3 i } = 0 . Then Equation 3.4.1-1 simplifies to
\begin{array}{l} \delta W ^ {I} = \int_ {V} \sigma_ {\alpha \beta} \delta \varepsilon_ {\alpha \beta} d V \\ = \int_ {V} \sigma_ {\alpha \beta} \delta L _ {\alpha \beta} d V \quad (\mathrm{since} \pmb {\sigma} \mathrm{issymmetric}), \\ \end{array}
where
\delta L _ {\alpha \beta} = \mathbf {e} _ {\alpha} \frac {\partial \delta \mathbf {u}}{\partial \mathbf {x}} \cdot \mathbf {e} _ {\beta} = \mathbf {e} _ {\alpha} \frac {\partial \delta \mathbf {u}}{\partial x _ {\beta}}
and d V = t d A , where t is the current thickness of the element and A is its current area.
Jacobian
The consistent Jacobian contribution from the element is
d \delta W ^ {I} = \int_ {A} t \left(\delta \pmb {\varepsilon}: \mathbf {D}: d \pmb {\varepsilon} + \pmb {\sigma}: \left(\delta \mathbf {L} ^ {T} \cdot d \mathbf {L} - 2 \delta \pmb {\varepsilon} \cdot d \pmb {\varepsilon}\right)\right) d A.
Since we assume that \sigma _ { 3 i } = 0 , the first term in the integrand is
\delta \varepsilon_ {\alpha \beta} D _ {\alpha \beta \gamma \delta} d \varepsilon_ {\gamma \delta}.
We also assume that there is no transverse shear strain of the element: \varepsilon _ { 3 i } = 0 , and, hence, \delta \varepsilon _ { \alpha i } d \varepsilon _ { i \beta } = \delta \varepsilon _ { \alpha \gamma } d \varepsilon _ { \gamma \beta } . Thus, the second term in the integrand is
\sigma_ {\alpha \beta} \left(\frac {\partial \mathbf {u}}{\partial x _ {\alpha}} \cdot \frac {\partial \mathbf {u}}{\partial x _ {\beta}} - \frac {1}{2} \left(\mathbf {e} _ {\gamma} \cdot \frac {\partial \mathbf {u}}{\partial x _ {\alpha}} + \mathbf {e} _ {\alpha} \cdot \frac {\partial \mathbf {u}}{\partial x _ {\gamma}}\right) \left(\mathbf {e} _ {\gamma} \cdot \frac {\partial \mathbf {u}}{\partial x _ {\beta}} + \mathbf {e} _ {\beta} \cdot \frac {\partial \mathbf {u}}{\partial x _ {\gamma}}\right)\right).
We can write this out as
\begin{array}{l} \sigma_ {1 1} \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} + \sigma_ {2 2} \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} + \sigma_ {1 2} \left(\frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} + \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}}\right) \\ - 2 \sigma_ {1 1} \mathbf {e} _ {1} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \mathbf {e} _ {1} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} - 2 \sigma_ {2 2} \mathbf {e} _ {2} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \mathbf {e} _ {2} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} \\ - \frac {1}{2} (\sigma_ {1 1} + \sigma_ {2 2}) \bigg (\mathbf {e} _ {2} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \mathbf {e} _ {2} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} + \mathbf {e} _ {1} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \mathbf {e} _ {1} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} + \mathbf {e} _ {1} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \mathbf {e} _ {2} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} + \mathbf {e} _ {2} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \mathbf {e} _ {1} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} \bigg) \\ - \sigma_ {1 2} \left(\mathbf {e} _ {1} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \mathbf {e} _ {1} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} + \mathbf {e} _ {2} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \mathbf {e} _ {2} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} + \mathbf {e} _ {1} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \mathbf {e} _ {1} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} + \mathbf {e} _ {2} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \mathbf {e} _ {2} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} \right. \\ + \mathbf {e} _ {1} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \mathbf {e} _ {2} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} + \mathbf {e} _ {2} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \mathbf {e} _ {1} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} + \mathbf {e} _ {1} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {1}} \mathbf {e} _ {2} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {1}} + \mathbf {e} _ {2} \cdot \frac {\partial \delta \mathbf {u}}{\partial x _ {2}} \mathbf {e} _ {1} \cdot \frac {\partial d \mathbf {u}}{\partial x _ {2}} \Bigg) \\ \end{array}
Thickness change
In geometrically nonlinear analyses the cross-section thickness changes as a function of the membrane strain with a user-defined "effective section Poisson's ratio," º.
In plane stress \sigma _ { 3 3 } = 0 ; ; linear elasticity gives
\epsilon_ {3 3} = - \frac {\nu}{1 - \nu} (\epsilon_ {1 1} + \epsilon_ {2 2}).
Treating these as logarithmic strains,
Elements
\ln \left(\frac {t}{t _ {0}}\right) = - \frac {\nu}{1 - \nu} \left(\ln \left(\frac {l _ {1}}{l _ {1} ^ {0}}\right) + \ln \left(\frac {l _ {2}}{l _ {2} ^ {0}}\right)\right) = - \frac {\nu}{1 - \nu} \ln \left(\frac {A}{A ^ {0}}\right),
where A is the area on the membrane's reference surface. This nonlinear analogy with linear elasticity leads to the thickness change relationship:
{\frac {t}{t _ {0}}} = \left({\frac {A}{A _ {0}}}\right) ^ {- {\frac {\nu}{1 - \nu}}}.
For \nu = 0 . 5 the material is incompressible; for \nu = 0 the section thickness does not change.
Total deformation
The deformation gradient is \mathbf { F } = \partial \mathbf { x } / \partial \mathbf { X } . Since we take \mathbf { e } _ { 3 } normal to the current membrane surface and assume no transverse shear of the membrane,
F _ {3 \alpha} = \mathbf {e} _ {3} \cdot \frac {\partial \mathbf {x}}{\partial X _ {\alpha}} = 0 \quad \text {and} \quad F _ {\alpha 3} = \mathbf {e} _ {\alpha} \cdot \frac {\partial \mathbf {x}}{\partial X _ {3}} = 0.
By the thickness change assumption above, the direct out-of-plane component of the deformation gradient is
F _ {3 3} = \frac {1}{\left(F _ {1 1} F _ {2 2} - F _ {1 2} F _ {2 1}\right) ^ {\frac {\nu}{1 - \nu}}}.
To calculate the deformation gradient at the end of the increment, first we calculate the two tangent vectors at the end of the increment defined by the derivative of the position with respect to the reference coordinates:
\frac {\partial \mathbf {x} ^ {n + 1}}{\partial X _ {\beta}} = \frac {\partial \mathbf {x} ^ {n + 1}}{\partial \xi_ {\alpha}} \frac {\partial \xi_ {\alpha}}{\partial X _ {\beta}},
where \partial \mathbf x ^ { n + 1 } / \partial \xi _ { \alpha } is obtained by interpolation with the shape function derivatives from the nodal coordinates and the change of coordinate transformation \partial \xi _ { \alpha } / \partial X _ { \beta } is based on the reference geometry. The deformation gradient components are defined
F _ {\alpha \beta} = \mathbf {e} _ {\alpha} ^ {n + 1} \cdot \frac {\partial \mathbf {x} ^ {n + 1}}{\partial X _ {\beta}}.
To choose the element basis directions \mathbf { e } _ { \alpha } ^ { n + 1 } , we do the following. Find any pair of in-plane orthonormal vectors \hat { \mathbf { e } } _ { \alpha } ^ { n + 1 } (by the standard ABAQUS projection). Then find the angle \Delta \psi such that the element basis vectors \mathbf { e } _ { \alpha } ^ { n + 1 } , defined
Elements
\mathbf {e} _ {1} ^ {n + 1} = \cos (\Delta \psi) \hat {\mathbf {e}} _ {1} ^ {n + 1} + \sin (\Delta \psi) \hat {\mathbf {e}} _ {2} ^ {n + 1}
\mathbf {e} _ {2} ^ {n + 1} = - \sin (\Delta \psi) \hat {\mathbf {e}} _ {1} ^ {n + 1} + \cos (\Delta \psi) \hat {\mathbf {e}} _ {2} ^ {n + 1},
satisfy the symmetry condition
F _ {\alpha \beta} = \mathbf {e} _ {\alpha} ^ {n + 1} \cdot \frac {\partial \mathbf {x} ^ {n + 1}}{\partial X _ {\beta}} = F _ {\beta \alpha}.
Using the definitions of \mathbf { e } _ { \alpha } ^ { n + 1 } in terms of \hat { \mathbf { e } } _ { \alpha } ^ { n + 1 } in the above equation, the rotation angle \Delta \psi is found to be
\Delta \psi = \tan^ {- 1} \left[ \frac {\hat {F} _ {2 1} - \hat {F} _ {1 2}}{\hat {F} _ {1 1} + \hat {F} _ {2 2}} \right],
where
\hat {F} _ {\alpha \beta} \stackrel {\mathrm{def}} {=} \hat {\mathbf {e}} _ {\alpha} ^ {n + 1} \cdot \frac {\partial \mathbf {x} ^ {n + 1}}{\partial X _ {\beta}}.
The deformation gradient then follows immediately.
For elastomers we work directly in terms of B _ { \alpha \beta } = F _ { \alpha \gamma } F _ { \beta \gamma } and B _ { 3 3 } = ( F _ { 3 3 } ) ^ { 2 } . For inelastic material models we need measures of incremental strain and average material rotation, which we compute from \Delta \mathbf { F } defined by \mathbf { F } = \Delta \mathbf { F } \cdot \mathbf { F } ^ { n } , where \mathbf { F } ^ { n } is the deformation gradient at the start of the current increment (at increment " n " ) :
(F ^ {n}) _ {\alpha \beta} = (\mathbf {e} ^ {n}) _ {\alpha} \cdot \frac {\partial \mathbf {x} ^ {n}}{\partial X _ {\beta}}.
We can define the components of \Delta \mathbf { F } ^ { - 1 } by
(\Delta F ^ {- 1}) _ {\alpha \beta} = (\mathbf {e} ^ {n}) _ {\alpha} \cdot \frac {\partial \mathbf {x} ^ {n}}{\partial x _ {\beta}}
and, hence, define \Delta F _ { \alpha \beta } by inversion.
The incremental strain and rotation are then defined from the polar decomposition \Delta \mathbf { F } = \Delta \mathbf { V } \cdot \Delta \mathbf { R } , where \Delta \mathbf { R } is a rotation matrix and \Delta { \bf V } is a pure stretch:
\Delta \mathbf {V} = \sum_ {I = 1} ^ {3} \Delta \lambda_ {I} \mathbf {a} ^ {I} \mathbf {a} ^ {I}
(see ``Deformation,'' Section 1.4.1). We find the \Delta \lambda _ { I } and the corresponding eigenvectors { \bf a } _ { I } by solving the eigenproblem for
Elements
\Delta \mathbf {F} \cdot \Delta \mathbf {F} ^ {T} = \Delta \mathbf {V} \cdot \Delta \mathbf {V} = \sum_ {I = 1} ^ {3} (\Delta \lambda_ {I}) ^ {2} \mathbf {a} ^ {I} \mathbf {a} ^ {I}.
Since we assume no transverse shear in the membrane, the normal direction (along e3) is always a principal direction, so the eigenproblem is the 2 £ 2 problem
\Delta F _ {\alpha \gamma} F _ {\beta \gamma} = \sum_ {I = 1} ^ {2} (\Delta \lambda) ^ {2} a _ {\alpha} ^ {I} a _ {\beta} ^ {I}.
The logarithmic strain increment is then
\Delta \varepsilon_ {\alpha \beta} = \sum_ {I = 1} ^ {2} \ln (\Delta \lambda_ {I}) a _ {\alpha} ^ {I} a _ {\beta} ^ {I},
and the average material rotation increment is defined from the polar decomposition of the increment:
\Delta R _ {\alpha \beta} = \sum_ {I = 1} ^ {2} \frac {1}{\Delta \lambda_ {I}} a _ {\alpha} ^ {I} a _ {\gamma} ^ {I} \Delta F _ {\gamma \beta}.
Due to the choice of the element basis directions, we can assume that
\Delta R _ {\alpha \beta} \approx \delta_ {\alpha \beta}.
3.4.2 Truss elements
Truss elements are one-dimensional bars or rods that are assumed to deform by axial stretching only. They are pin jointed at their nodes, and so only translational displacements and the initial position vector at each node are used in the discretization. When the strains are large, the formulation is simplified by assuming that the trusses are made of incompressible material.
There are two truss elements in ABAQUS: a 2-node linear interpolation truss and a 3-node quadratic interpolation truss. The quadratic interpolation version is in the library mainly for compatibility with the quadratic interpolation elements of other types, such as shell element S8R5. The same interpolation functions are used for both the Cartesian displacement components and for the Cartesian components of the initial position vector, so these elements are the simplest form of isoparametric elements.
The elements are one-dimensional: a single material (isoparametric) coordinate, g, is defined along the element, with - 1 \leq g \leq 1 in the element. In a 2-node element node 1 is at g = ¡1 and node 2 is at g = + 1 . In the 3-node version node 1 is at g = ¡1, node 2 is at g = 0, and node 3 is at g = +1.
Interpolation
The interpolation for the 2-node element is