김경종
29 KiB
2. Procedures
2.1 Overview
2.1.1 Procedures: overview and basic equations
ABAQUS is designed as a flexible tool for finite element modeling. An important aspect of this flexibility is the manner in which ABAQUS allows the user to step through the history to be analyzed. This is accomplished by defining analysis procedures.
A basic concept in ABAQUS is the division of the problem history into steps. A step is any convenient phase of the history--a thermal transient, a creep hold, a dynamic transient, etc. In its simplest form in ABAQUS/Standard, a "step" is just a static analysis of a load change from one magnitude to another.
In each "step" the user chooses a procedure, thus defining the type of analysis to be performed during the step: dynamic stress analysis, eigenvalue buckling, transient heat transfer analysis, etc. The procedure choice can be changed from step to step in any meaningful way. Since the state of the model (stresses, strains, temperatures, etc.) is updated throughout all analysis steps, the effects of previous history are always included in the response in each new step. Thus, for example, if natural frequency extraction is performed after a geometrically nonlinear static analysis step, the preload stiffness will be included.
ABAQUS/Standard provides both linear and nonlinear response options. The program is truly integrated, so linear analysis is always considered as linear perturbation analysis about the state at the time when the linear analysis procedure is introduced. This linear perturbation approach allows general application of linear analysis techniques in cases where the linear response depends on preloading or the nonlinear response history of the model.
In nonlinear problems the objective is to obtain a convergent solution at a minimum cost. The nonlinear procedures in ABAQUS/Standard offer two approaches to this. Direct user control of increment size is one choice, whereby the user specifies the incrementation scheme. Automatic control is the alternate approach: the user defines the step and specifies certain tolerances or error measures. ABAQUS/Standard then automatically selects the increments as it develops the response in the step. This approach is usually more efficient, because the user cannot predict the response ahead of time. Automatic control is particularly valuable in cases where the time or load increment varies widely through the step, as is often the case in diffusion type problems (such as creep, heat transfer, and consolidation).
In ABAQUS/Explicit the time incrementation is controlled by the stability limit of the central difference operator. The time incrementation scheme is, hence, fully automatic and requires no user intervention. User-specified time incrementation is not available because it would always be nonoptimal.
ABAQUS/Standard and ABAQUS/Explicit are separate program modules with different data structures; hence, the explicit dynamics procedure cannot be used in the same analysis as any of the procedures in ABAQUS/Standard. However, ABAQUS provides a capability to import a deformed mesh and associated material state from ABAQUS/Explicit into ABAQUS/Standard and vice versa.
This procedure is described in ``Transferring results between ABAQUS/Explicit and ABAQUS/Standard,'' Section 7.6.1 of the ABAQUS/Standard User's Manual.
In this chapter the basic equations for the most important analysis procedures in ABAQUS/Standard and ABAQUS/Explicit are described. In some sections specific aspects of an analysis procedure (i.e., damping, cavity radiation, etc.) are discussed.
Basic finite element equations
This section describes the basic equations for standard displacement-based finite element analysis. We begin with the equilibrium statement, written as the virtual work principle, Equation 1.5.1-6:
\int_ {V} \pmb {\sigma}: \delta \mathbf {D} d V = \int_ {S} \mathbf {t} ^ {T} \cdot \delta \mathbf {v} d S + \int_ {V} \mathbf {f} ^ {T} \cdot \delta \mathbf {v} d V.
Following the discussion in ``Equilibrium and virtual work,'' Section 1.5.1, the left-hand side of this equation (the internal virtual work rate term) is replaced with the integral over the reference volume of the virtual work rate per reference volume defined by any conjugate pairing of stress and strain:
Equation 2.1.1-1
\int_ {V ^ {0}} \pmb {\tau} ^ {c}: \delta \pmb {\varepsilon} d V ^ {0} = \int_ {S} \mathbf {t} ^ {T} \cdot \delta \mathbf {v} d S + \int_ {V} \mathbf {f} ^ {T} \cdot \delta \mathbf {v} d V,
where \pmb { \tau } ^ { c } and " are any conjugate pairing of material stress and strain measures. The particular choice of " depends on the individual element--see Chapter 3, "Elements."
The finite element interpolator can be written in general as
\mathbf {u} = \mathbf {N} _ {N} u ^ {N},
where { \bf N } _ { N } are interpolation functions that depend on some material coordinate system, u ^ { N } are nodal variables, and the summation convention is adopted for the uppercase subscripts and superscripts that indicate nodal variables.
The virtual field, \delta \mathbf { v } , must be compatible with all kinematic constraints. Introducing the above interpolation constrains the displacement to have a certain spatial variation, so \delta \mathbf { v } must also have the same spatial form:
\delta \mathbf {v} = \mathbf {N} _ {N} \delta v ^ {N}.
The continuum variational statement Equation 2.1.1-1 is, thus, approximated by a variation over the finite set \delta v ^ { N } .
Now ±" is the virtual rate of material strain associated with \delta \mathbf { v } , and because it is a rate form, it must be linear in \delta \mathbf { v } . Hence, the interpolation assumption gives
\delta \pmb {\varepsilon} = \pmb {\beta} _ {N} \delta v ^ {N},
Procedures
where \beta _ { N } is a matrix that depends, in general, on the current position, x, of the material point being considered. The matrix \pmb { \beta } _ { N } that defines the strain variation from the variations of the kinematic variables is derivable immediately from the interpolation functions once the particular strain measure to be used is defined.
Without loss of generality we can write \pmb { \beta } _ { N } = \pmb { \beta } _ { N } ( \mathbf { x } , \ \mathbf { N } _ { N } ) , and--with this notation--the equilibrium equation is approximated as
\delta v ^ {N} \int_ {V ^ {0}} \pmb {\beta} _ {N}: \pmb {\tau} ^ {c} d V ^ {0} = \delta v ^ {N} \biggl [ \int_ {S} \mathbf {N} _ {N} ^ {T} \cdot \mathbf {t} d S + \int_ {V} \mathbf {N} _ {N} ^ {T} \cdot \mathbf {f} d V \biggr ];
since the \delta v ^ { N } are independent variables, we can choose each one to be nonzero and all others zero in turn, to arrive at a system of nonlinear equilibrium equations:
Equation 2.1.1-2
\int_ {V ^ {0}} \pmb {\beta} _ {N}: \pmb {\tau} ^ {c} d V ^ {0} = \int_ {S} \mathbf {N} _ {N} ^ {T} \cdot \mathbf {t} d S + \int_ {V} \mathbf {N} _ {N} ^ {T} \cdot \mathbf {f} d V.
This system of equations forms the basis for the (standard) assumed displacement finite element analysis procedure and is of the form
F ^ {N} (u ^ {M}) = 0
discussed above. The above equations are valid for static and dynamic analysis if the body force is assumed to contain the inertia contribution. In dynamic analysis, however, the inertia contribution is more commonly considered separately, leading to the equations
M ^ {N M} \ddot {u} ^ {M} + F ^ {N} (u ^ {M}) = 0.
For the Newton algorithm (or for the linear perturbation procedure) used in ABAQUS/Standard, we need the Jacobian of the finite element equilibrium equations. To develop the Jacobian, we begin by taking the variation of Equation 2.1.1-1, giving
Equation 2.1.1-3
\begin{array}{l} \int_ {V ^ {0}} (d \pmb {\tau} ^ {c}: \delta \pmb {\varepsilon} + \pmb {\tau} ^ {c}: d \delta \pmb {\varepsilon}) d V ^ {0} - \int_ {S} d \mathbf {t} ^ {T} \cdot \delta \mathbf {v} d S - \int_ {S} \mathbf {t} ^ {T} \cdot \delta \mathbf {v} d A _ {r} \frac {1}{A _ {r}} d S \\ - \int_ {V} d \mathbf {f} ^ {T} \cdot \delta \mathbf {v} d V - \int_ {V} \mathbf {f} ^ {T} \cdot \delta \mathbf {v} d J \frac {1}{J} d V = 0, \\ \end{array}
where d( ) represents the linear variation of the quantity ( ) with respect to the basic variables (the degrees of freedom of the finite element model). In the above expression J = | d V / d V ^ { 0 } | is the volume change between the reference and the current volume occupied by a piece of the structure and, likewise, A _ { r } = | d S / d S ^ { 0 } | is the surface area ratio between the reference and the current configuration. The Jacobian matrix is obtained by restricting the above variation, allowing variations in the nodal
Procedures
variables, u ^ { N } , only. Let such a restricted variation be indicated by \partial _ { N } = \partial / \partial { u } ^ { N } . Examining Equation 2.1.1-3 term by term with this in mind, we proceed as follows. The first term contains d \tau ^ { c } . We now assume that the constitutive theory allows us to write
d \pmb {\tau} ^ {c} = \mathbf {H}: d \pmb {\varepsilon} + \mathbf {g},
where H and g are defined in terms of the current state, direction of straining, etc., and on the kinematic assumptions used to form the generalized strains. See Chapter 4, "Mechanical Constitutive Theories," for a detailed discussion of forming H and g for the material models currently available in ABAQUS. From the choice of generalized strain measure and interpolation function,
\partial_ {N} \pmb {\varepsilon} = \frac {\partial \pmb {\varepsilon}}{\partial u ^ {N}} = \pmb {\beta} _ {N}.
From the above constitutive assumption,
\partial_ {N} \pmb {\tau} ^ {c} = \mathbf {H}: \pmb {\beta} _ {N}.
Now, since ±" is the first variation of " with respect to nodal variables,
\delta \pmb {\varepsilon} = \partial_ {M} \pmb {\varepsilon} \delta u ^ {M} = \pmb {\beta} _ {M} \delta u ^ {M}.
Thus, the first term in the Jacobian matrix is
\int_ {V ^ {0}} \pmb {\beta} _ {M}: \mathbf {H}: \pmb {\beta} _ {N} d V ^ {0},
the usual "small-displacement stiffness matrix," except that, since the strain measure " will always be nonlinear in displacement, the \beta _ { N } in this term will be a function of displacement.
The second term in Equation 2.1.1-3 is
\int_ {V ^ {0}} \pmb {\tau} ^ {c}: d \delta \pmb {\varepsilon} d V ^ {0}.
This is rewritten as
\int_ {V ^ {0}} \pmb {\tau} ^ {c}: \partial_ {N} \delta \pmb {\varepsilon} d V ^ {0},
which is
\int_ {V ^ {0}} \pmb {\tau} ^ {c}: \partial_ {N} \pmb {\beta} _ {M} d V ^ {0}.
This term contributes to the Jacobian and is the "initial stress matrix."
Procedures
The external load rate terms in Equation 2.1.1-3 are considered next. In general, these load vectors can be written
\mathbf {t} = \mathbf {t} (\lambda , \mathbf {x}) \text { and } \mathbf {f} = \mathbf {f} (\lambda , \mathbf {x}),
where ¸ represents the externally prescribed loading parameters. Whether the load depends on position or not depends on the particular load type, but common types of loading (pressure, centrifugal load) do depend on position--for example, if t is caused by pressure on the surface, t depends on the pressure magnitude, on the direction of the normal to the surface, and on the current surface area: the latter two are functions of the current position of points on the surface. The variation of the load vector with nodal variables can then be written symbolically as
\partial_ {N} \mathbf {t} + \mathbf {t} \frac {1}{A _ {r}} \partial_ {N} A _ {r} = \mathbf {Q} _ {N} ^ {S},
\partial_ {N} \mathbf {f} + \mathbf {f} \frac {1}{J} \partial_ {N} J = \mathbf {Q} _ {N} ^ {V},
and then writing
\delta \mathbf {v} = \mathbf {N} _ {M} \delta v ^ {M},
where { \bf N } _ { M } is obtained directly from the interpolation functions, we can write the Jacobian terms pertaining to the last four terms of Equation 2.1.1-3 as
- \int_ {S} \mathbf {N} _ {M} ^ {T} \cdot \mathbf {Q} _ {N} ^ {S} d S - \int_ {V} \mathbf {N} _ {M} ^ {T} \cdot \mathbf {Q} _ {N} ^ {V} d V.
These are commonly called the "load stiffness matrix." The actual form of the load stiffness is very much dependent on the type of load being considered--see Chapter 3, "Elements," and Hibbitt (1979) for examples.
The complete Jacobian matrix is then
Equation 2.1.1-4
K _ {M N} = \int_ {V ^ {0}} \pmb {\beta} _ {M}: \mathbf {H}: \pmb {\beta} _ {N} d V ^ {0} + \int_ {V ^ {0}} \pmb {\tau} ^ {c}: \partial_ {N} \pmb {\beta} _ {M} d V ^ {0} - \int_ {S} \mathbf {N} _ {M} ^ {T} \cdot \mathbf {Q} _ {N} ^ {S} d S - \int_ {V} \mathbf {N} _ {M} ^ {T} \cdot \mathbf {Q} _ {N} ^ {V} d V.
Thus, Equation 2.1.1-2 and Equation 2.1.1-4 provide the basis for the Newton incremental solution, given specification of the interpolation function and constitutive theories to be used.
2.2 Nonlinear solution methods
2.2.1 Nonlinear solution methods in ABAQUS/Standard
Procedures
The finite element models generated in ABAQUS are usually nonlinear and can involve from a few to thousands of variables. In terms of these variables the equilibrium equations obtained by discretizing the virtual work equation can be written symbolically as
Equation 2.2.1-1
F ^ {N} (u ^ {M}) = 0,
where F ^ { N } is the force component conjugate to the N ^ { \mathrm { t h } } variable in the problem and u ^ { M } is the value of the M ^ { \mathrm { t h } } variable. The basic problem is to solve Equation 2.2.1-1 for the u ^ { M } throughout the history of interest.
Many of the problems to which ABAQUS will be applied are history-dependent, so the solution must be developed by a series of "small" increments. Two issues arise: how the discrete equilibrium statement Equation 2.2.1-1 is to be solved at each increment, and how the increment size is chosen.
ABAQUS/Standard generally uses Newton's method as a numerical technique for solving the nonlinear equilibrium equations. The motivation for this choice is primarily the convergence rate obtained by using Newton's method compared to the convergence rates exhibited by alternate methods (usually modified Newton or quasi-Newton methods) for the types of nonlinear problems most often studied with ABAQUS. The basic formalism of Newton's method is as follows. Assume that, after an iteration i, an approximation u _ { i } ^ { M } , to the solution has been obtained. Let c _ { i + } ^ { M } 1 be the difference between this solution and the exact solution to the discrete equilibrium equation Equation 2.2.1-1. This means that
F ^ {N} (u _ {i} ^ {M} + c _ {i + 1} ^ {M}) = 0.
Expanding the left-hand side of this equation in a Taylor series about the approximate solution u _ { i } ^ { M } then gives
\begin{array}{l} F ^ {N} (u _ {i} ^ {M}) + \frac {\partial F ^ {N}}{\partial u ^ {P}} (u _ {i} ^ {M}) c _ {i + 1} ^ {P} \\ + \frac {\partial^ {2} F ^ {N}}{\partial u ^ {P} \partial u ^ {Q}} (u _ {i} ^ {M}) c _ {i + 1} ^ {P} c _ {i + 1} ^ {Q} + \ldots = 0. \\ \end{array}
If u _ { i } ^ { M } is a close approximation to the solution, the magnitude of each c _ { i + 1 } ^ { M } will be small, and so all but the first two terms above can be neglected giving a linear system of equations:
Equation 2.2.1-2
K _ {i} ^ {N P} c _ {i + 1} ^ {P} = - F _ {i} ^ {N},
where
K _ {i} ^ {N P} = \frac {\partial F ^ {N}}{\partial u ^ {P}} (u _ {i} ^ {M})
is the Jacobian matrix and
F _ {i} ^ {N} = F ^ {N} (u _ {i} ^ {M}).
The next approximation to the solution is then
u _ {i + 1} ^ {M} = u _ {i} ^ {M} + c _ {i + 1} ^ {M},
and the iteration continues.
Convergence of Newton's method is best measured by ensuring that all entries in F _ { i } ^ { N } and all entries in c _ { i + \cdot } ^ { N } 1 are sufficiently small. Both these criteria are checked by default in an ABAQUS/Standard solution. ABAQUS/Standard also prints peak values in the force residuals, incremental displacements, and corrections to the incremental displacements at each iteration so that the user can check for these contingencies himself.
Newton's method is usually avoided in large finite element codes, apparently for two reasons. First, the complete Jacobian matrix is sometimes difficult to formulate; and for some problems it can be impossible to obtain this matrix in closed form, so it must be calculated numerically--an expensive (and not always reliable) process. Secondly, the method is expensive per iteration, because the Jacobian must be formed and solved at each iteration. The most commonly used alternative to Newton is the modified Newton method, in which the Jacobian in Equation 2.2.1-2 is recalculated only occasionally (or not at all, as in the initial strain method of simple contained plasticity problems). This method is attractive for mildly nonlinear problems involving softening behavior (such as contained plasticity with monotonic straining) but is not suitable for severely nonlinear cases. (In some cases ABAQUS/Standard uses an approximate Newton method if it is either not able to compute the exact Jacobian matrix or if an approximation would result in a quicker total solution time. For example, several of the models in ABAQUS/Standard result in a nonsymmetric Jacobian matrix, but the user is allowed to choose a symmetric approximation to the Jacobian on the grounds that the resulting modified Newton method converges quite well and that the extra cost of solving the full nonsymmetric system does not justify the savings in iteration achieved by the quadratic convergence of the full Newton method. In other cases the user is allowed to drop interfield coupling terms in coupled procedures for similar reasons.)
Another alternative is the quasi-Newton method, in which Equation 2.2.1-2 is symbolically rewritten
c _ {i + 1} ^ {P} = - [ K _ {i} ^ {N P} ] ^ {- 1} F _ {i} ^ {N}
and the inverse Jacobian is obtained by an iteration process.
There are a wide range of quasi-Newton methods. The more appropriate methods for structural applications appear to be reasonably well behaved in all but the most extremely nonlinear cases--the trade-off is that more iterations are required to converge, compared to Newton. While the savings in forming and solving the Jacobian might seem large, the savings might be offset by the additional arithmetic involved in the residual evaluations (that is, in calculating the Fi), and in the cascading vector transformations associated with the quasi-Newton iterations. Thus, for some practical cases quasi-Newton methods are more economic than full Newton, but in other cases they are more
Procedures
expensive. ABAQUS/Standard offers the "BFGS" quasi-Newton method: it is described in `Quasi-Newton solution technique,'' Section 2.2.2.
When any iterative algorithm is applied to a history-dependent problem, the intermediate, nonconverged solutions obtained during the iteration process are usually not on the actual solution path; thus, the integration of history-dependent variables must be performed completely over the increment at each iteration and not obtained as the sum of integrations associated with each Newton iteration, c _ { i } . . In ABAQUS/Standard this is done by assuming that the basic nodal variables, u , vary linearly over the increment, so that
u (\tau) = \big (1 - \frac {\tau}{\Delta t} \big) u (t) + \frac {\tau}{\Delta t} u (t + \Delta t),
where 0 \leq \tau \leq \Delta t represents "time" during the increment. Then, for any history-dependent variable, g ( t ) , we compute
g (t + \Delta t) = g (t) + \int_ {t} ^ {t + \Delta t} \frac {d g}{d \tau} (\tau) d \tau
at each iteration.
The issue of choosing suitable time steps is a difficult problem to resolve. First of all, the considerations are quite different in static, dynamic, or diffusion cases. It is always necessary to model the response as a function of time to some acceptable level of accuracy. In the case of dynamic or diffusion problems time is a physical dimension for the problem and the time stepping scheme must provide suitable steps to allow accurate modeling in this dimension. Even if the problem is linear, this accuracy requirement imposes restrictions on the choice of time step. In contrast, most static problems have no imposed time scale, and the only criterion involved in time step choice is accuracy in modeling nonlinear effects. In dynamic and diffusion problems it is exceptional to encounter discontinuities in the time history, because inertia or viscous effects provide smoothing in the solution. (One of the exceptions is impact. The technique used in ABAQUS/Standard for this is discussed in ``Intermittent contact/impact,'' Section 2.4.2.) However, in static cases sharp discontinuities (such as bifurcations caused by buckling) are common. Softening systems, or unconstrained systems, require special consideration in static cases but are handled naturally in dynamic or diffusion cases. Thus, the considerations upon which time step choice is made are quite different for the three different problem classes.
ABAQUS provides both "automatic" time step choice and direct user control for all classes of problems. Direct user control can be useful in cases where the problem behavior is well understood (as might occur when the user is carrying out a series of parameter studies) or in cases where the automatic algorithms do not handle the problem well. However, the automatic schemes in ABAQUS are based on extensive experience with a wide range of problems and, therefore, generally provide a reliable approach.
For static problems a number of schemes have been suggested for automatic step control (see, for example, Bergan et al., 1978). ABAQUS/Standard uses a scheme based predominantly on the
maximum force residuals following each iteration. By comparing consecutive values of these quantities, ABAQUS/Standard determines whether convergence is likely in a reasonable number of iterations. If convergence is deemed unlikely, ABAQUS/Standard adjusts the load increment; if convergence is deemed likely, ABAQUS/Standard continues with the iteration process. In this way excessive iteration is eliminated in cases where convergence is unlikely, and an increment that appears to be converging is not aborted because it needed a few more iterations. One other ingredient in this algorithm is that a minimum increment size is specified, which prevents excessive computation in cases where buckling, limit load, or some modeling error causes the solution to stall. This control is handled internally, with user override if needed. Several other controls are built into the algorithm; for example, it will cut back the increment size if an element inverts due to excessively large geometry changes. These detailed controls are based on empirical testing. The full algorithm is described in detail in ``Convergence criteria for nonlinear problems,'' Section 8.3.3 of the ABAQUS/Standard User's Manual.
In dynamic analysis when implicit integration is used, the automatic time stepping is based on the concept of half-step residuals (Hibbitt and Karlsson, 1979). The basic idea is that the time stepping operator defines the velocities and accelerations at the end of the step ( t + \Delta t ) in terms of displacement at the end of the step and conditions at the beginning of the step. Equilibrium is then established at ( t + \Delta t ) ; which ensures an equilibrium solution at the end of each time step and, thus, at the beginning and end of any individual time step. However, these equilibrium solutions do not guarantee equilibrium throughout the step. The time step control is based on measuring the equilibrium error (the force residuals) at some point during the time step, by using the integration operator, together with the solution obtained at ( t + \Delta t ) , to interpolate within the time step. The evaluation is performed at the half step ( t + \Delta t / 2 ) . If the maximum entry in this residual vector--the maximum "half-step residual"--is greater than a user-specified tolerance, the time step is considered to be too big and is reduced by an appropriate factor. If the maximum half-step residual is sufficiently below the user-specified tolerance, the time step can be increased by an appropriate factor for the next increment. Otherwise, the time step is deemed adequate. The algorithm is somewhat more complicated at traumatic events such as impact. Here, the time step can also be adjusted based on the magnitude of residuals in the first or second iteration following such events. Clearly, if these residuals are several orders of magnitude greater than those permitted, convergence is unlikely and the time step is altered immediately to avoid unproductive iteration. These algorithms are discussed in more detail in ``Intermittent contact/impact,'' Section 2.4.2, as well as in ``Convergence criteria for nonlinear problems,'' Section 8.3.3 of the ABAQUS/Standard User's Manual, and ``Time integration accuracy in transient problems,'' Section 8.3.4 of the ABAQUS/Standard User's Manual. They are products of experience and many numerical experiments and have been shown to be effective in several problem areas of interest.
2.2.2 Quasi-Newton solution technique
A major contribution to the computational effort involved in nonlinear analysis is the solution of the nonlinear equations (Equation 2.2.1-1). In most cases ABAQUS/Standard uses Newton's method to solve these equations, as described in ``Nonlinear solution methods in ABAQUS/Standard,'' Section 2.2.1. The principal advantage of Newton's method is its quadratic convergence rate when the approximation at iteration i is within the "radius of convergence"--that is, when the gradients defined
Procedures
by KNMi K _ { i } ^ { N M } provide an improvement to the solution. The method has two major disadvantages: the Jacobian matrix has to be calculated, and this same matrix has to be solved. The calculation of the Jacobian matrix is a problem because, in many important cases, it is difficult to derive the form of the matrix algebraically. The solution of the Jacobian is a problem because of the computational effort involved: as the problem size increases, the direct solution of the linear equations can dominate the entire computational effort.
There are a number of important nonlinear applications where the Jacobian is symmetric, is fairly well conditioned, and does not change greatly from one iteration to the next. Examples are implicit dynamic time integration with small time increments relative to the periods of the natural vibrations that participate in the response or small-displacement elastic-plastic analysis where the yielding is confined (such as occurs in many practical fracture mechanics applications). In such cases, especially when the problem is large, it can be less expensive to use an alternative to the Newton approach to the solution of the nonlinear equations. The "quasi-Newton" methods are such an approach; and Matthies and Strang (1979) have shown that, for systems of equations with a symmetric Jacobian matrix, the BFGS (Broyden, Fletcher, Goldfarb, Shanno) method can be written in a simple form that is especially effective on the computer and is successful in such applications. This method is implemented in ABAQUS/Standard and is described in this section. The user must select this method by using the *SOLUTION TECHNIQUE option: by default, ABAQUS/Standard uses the standard Newton method.
The basis of quasi-Newton methods is to obtain a series of improved approximations to the Jacobian matrix, \widetilde { K } _ { i } ^ { N M } , that satisfy the secant condition:
Equation 2.2.2-1
F ^ {N} (u _ {i} ^ {M}) - F ^ {N} (u _ {i - 1} ^ {M}) = \widetilde {K} _ {i} ^ {N M} \left(u _ {i} ^ {M} - u _ {i - 1} ^ {M}\right),
so that \widetilde { K } _ { i } ^ { N M } approaches K _ { i } ^ { N M } as the iterations proceed. Equation 2.2.2-1 is the basic quasi-Newton equation.
For convenience we define the change in the residual from one iteration to the next as
\gamma_ {i} ^ {N} = F _ {i} ^ {N} - F _ {i - 1} ^ {N},
so that Equation 2.2.2-1 can be written
Equation 2.2.2-2
\gamma_ {i} ^ {N} = \widetilde {K} _ {i} ^ {N M} c _ {i} ^ {M},
where c _ { i } ^ { - M } is the correction to the solution from the previous iteration, defined in ``Nonlinear solution methods in ABAQUS/Standard,'' Section 2.2.1.
Matthies and Strang's implementation of the BFGS method is a computationally inexpensive method of creating a series of approximations to \left[ \widetilde { K } _ { i } ^ { N M } \right] ^ { - 1 } that satisfy Equation 2.2.2-1 and retain the symmetry and positive definiteness of \widetilde { K } _ { i } ^ { N M } . They accomplish this by updating \left[ \widetilde { K } _ { i - 1 } ^ { N M } \right] ^ { - 1 } to