김경종
29 KiB
scale factor, the solid/fluid density ratio, the linear convergence criterion, and the stiffness scale factor to control mesh motion and FSI stabilization.
The implicit algorithm uses the matrix-free, iteration method to solve the pseudo-elastic problem. The number of iterations and the linear convergence criterion control accuracy when solving the linear elasticity equations during the ALE process for FSI or deforming-mesh problems. Reducing the number of iterations or relaxing the linear convergence criterion can help reduce computational time. Similarly, increasing the number of iterations or the linear convergence criterion can help to ensure that the mesh quality remains good. The stiffness scale factor can be used to scale the elastic stiffness. Decreasing the elastic stiffness produces an ALE mesh with more local deformation.
When the explicit algorithm for mesh smoothing is used, you can specify the minimum number of mesh smoothing increments, the maximum number of mesh smoothing increments, the FSI penalty scale factor, the solid/fluid density ratio, and the stiffness scale factor to control the mesh motion and FSI stabilization.
The minimum and maximum number of mesh smoothing increments controls the number of mesh smoothing steps taken during the ALE process for FSI or deforming-mesh problems. Reducing the minimum and maximum number of mesh smoothing increments can help reduce computational time. Similarly, increasing the minimum/maximum number of smoothing increments helps to ensure that the mesh quality remains good and avoids potential element collapse during the evolution of a deformingmesh problem.
The FSI penalty scale factor is used to control FSI stabilization and has a default value of 1.0. Increasing this parameter in increments of 0.1 may be necessary for extremely flexible structures in highdensity fluids when the structural accelerations are high.
The solid/fluid density ratio is also used to control FSI stabilization. By default, the solid/fluid density ratio is ignored if its value is not specified. When multiple solid-fluid interfaces are present, you should choose the smallest solid/fluid density ratio.
Input File Usage: Use one of the following options to control the mesh smoothing or FSI stabilization:
*CONTROLS, TYPE=FSI, MESH SMOOTHING=IMPLICIT number of iterations before convergence check, maximum number of iterations, FSI penalty scale factor, solid/fluid density ratio, stiffness scale factor, linear convergence criterion
*CONTROLS, TYPE=FSI, MESH SMOOTHING=EXPLICIT minimum number of mesh smoothing increments, maximum number of mesh smoothing increments, FSI penalty scale factor, solid/fluid density ratio, stiffness scale factor
Abaqus/CAE Usage: Controlling FSI stabilization in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation is not supported in Abaqus/CAE.
Controlling mesh distortion
Similar to the distortion control used in Abaqus/Explicit (see “Section controls,” Section 27.1.4, for details), Abaqus/CFD offers distortion control to prevent elements from inverting or distorting
excessively in fluid mesh movement when the explicit mesh smoothing algorithm is used. By default, distortion control is turned off during the co-simulation and ignored if the implicit mesh smoothing algorithm is used.
Input File Usage: Use the following option to deactivate distortion control (default) when the implicit mesh smoothing algorithm is used:
*CONTROLS, TYPE=FSI, MESH SMOOTHING=EXPLICIT, DISTORTION CONTROL=OFF
Use the following option to activate distortion control:
*CONTROLS, TYPE=FSI, MESH SMOOTHING=EXPLICIT, DISTORTION CONTROL=ON
Abaqus/CAE Usage: Controlling mesh distortion in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation is not supported in Abaqus/CAE.
7.2.3 CONVERGENCE CRITERIA FOR NONLINEAR PROBLEMS
Products: Abaqus/Standard Abaqus/CAE
WARNING: The information in this section is provided for users who may wish to adjust the convergence criteria for the solution of nonlinear systems. In most cases these criteria need not be adjusted.
References
• “Convergence and time integration criteria: overview,” Section 7.2.1
• *CONTROLS
• “Customizing general solution controls,” Section 14.15.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
In nonlinear problems the governing balance equations must be solved iteratively. This section describes:
• the solution method for nonlinear problems (Newton’s method);
• the field equations that can be solved by Abaqus/Standard;
• the criteria used to establish convergence of each iteration during the solution;
• “severe discontinuity” iterations; and
• the line search algorithm, which can be used to improve the robustness of the Newton method.
Solution method
Where possible, Abaqus/Standard uses Newton’s method to solve nonlinear problems. In some cases it uses an exact implementation of Newton’s method, in the sense that the Jacobian of the system is defined exactly, and quadratic convergence is obtained when the estimate of the solution is within the radius of convergence of the algorithm. In other cases the Jacobian is approximated so that the iterative method is not an exact Newton method. For example, some material and surface interface models (such as nonassociated flow plasticity models or Coulomb friction) create a nonsymmetric Jacobian matrix, but you may choose to approximate this matrix by its symmetric part.
Many problems exhibit discontinuous behavior. A common example is contact: at a particular point on a surface, the contact constraint is either present or absent. Another (usually less severe) example is strain reversal in plasticity at a point where the material is yielding.
Specifying the quasi-Newton method
You can choose to use the quasi-Newton technique for a particular step (described in “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Guide) instead of the standard Newton method for solving nonlinear equations.
The quasi-Newton technique can save substantial computational cost in some cases by reducing the number of times the Jacobian matrix is factorized. Generally it is most successful when the system is large and many iterations are needed per increment or when the stiffness matrix is not changing much from iteration to iteration (such as in a dynamic analysis using implicit time integration or in a small-displacement analysis with local plasticity). It can be used only for symmetric systems of equations; therefore, it cannot be used when the unsymmetric solver is specified for a step (see “Defining an analysis,” Section 6.1.2), nor can it be used for procedures that always produce an unsymmetric system of equations, such as “Fully coupled thermal-stress analysis,” Section 6.5.3, and “Abaqus/Aqua analysis,” Section 6.11.1. In addition, it cannot be used for a static Riks procedure (see “Unstable collapse and postbuckling analysis,” Section 6.2.4).
The quasi-Newton method works well in combination with the line search method (see “Improving the efficiency of the solution by using the line search algorithm). Line searches help to prevent divergence of equilibrium iterations resulting from the inexact Jacobian produced by the quasi-Newton method. The line search method is activated by default for steps that use the quasi-Newton method. You can override this action by specifying line search controls.
You can specify the number of quasi-Newton iterations allowed before the kernel matrix is reformed. The default number of iterations is 8. Additional matrix reformations may occur automatically during the iteration process depending on the convergence behavior. Since quadratic convergence is not expected during quasi-Newton iterations, the logarithmic rate of convergence check is not applied during the time incrementation. Furthermore, the iteration count used in the time incrementation is a weighted sum of quasi-Newton iterations, with the weight factor depending on whether or not a kernel matrix has been reformed.
Input File Usage: *SOLUTION TECHNIQUE, TYPE=QUASI-NEWTON, REFORM KERNEL=n
Abaqus/CAE Usage: Step module: step editor: Other: Solution technique: Quasi-Newton, Number of iterations allowed before the kernel matrix is reformed: n
Specifying the separated method
Alternatively, you can choose to use the separated technique instead of the standard Newton method for solving nonlinear equations for fully coupled thermal-stress and coupled thermal-electrical procedures.
The separated technique (described in “Fully coupled thermal-stress analysis,” Section 6.5.3, and “Coupled thermal-electrical analysis,” Section 6.7.3) approximates the Jacobian by eliminating interfield coupling terms and can save substantial computational cost in cases where there is relatively weak coupling between the fields.
Input File Usage: *SOLUTION TECHNIQUE, TYPE=SEPARATED
Abaqus/CAE Usage: Step module: step editor: Other: Solution technique: Separated
Field equations
Field equations can be modeled separately or fully coupled. Some fields in Abaqus/Standard can only have linear response. Each field is discretized by using basic nodal variables (the degrees of freedom at
the nodes of the finite element model) such as the components of the displacement in a continuum stress analysis problem. Each field has a conjugate “flux.”
Available fields and their conjugate fluxes
The fields and conjugate fluxes available in Abaqus/Standard are as follows:
| Basic problem | Field | Conjugate flux |
| Stress analysis: force equilibrium | Displacement, u | Force, F |
| Stress analysis: moment equilibrium | Rotation, φ | Moment, M |
| Stress analysis: analysis containing beams with warping | Warping, w | Bimoment, W |
| Heat transfer analysis | Temperature, θ | Heat flux, q |
| Acoustic analysis (linear only) | Acoustic pressure, u | Rate of change of fluid volumetric flux |
| Pore liquid flow analysis | Pore liquid pressure, u | Pore liquid volumetric flux, q |
| Hydrostatic fluid modeling | Fluid pressure, p | Fluid volume, V |
| Mass diffusion analysis | Normalized concentration, φ | Mass concentration volumetric flux, Q |
| Piezoelectric analysis | Electrical potential, φ | Electrical charge, q |
| Electric conduction analysis | Electrical potential, φ | Electrical current, J |
| Mechanism analysis (connector elements with material flow degree of freedom) | Material flow | Material flux |
| Analysis containing C3D4H elements (all materials, except compressible hyperelastic elastomers and elastomeric foams). | Pressure Lagrange multiplier | Volumetric flux |
| Analysis containing C3D4H elements with compressible hyperelastic or hyperfoam materials. | Volumetric Lagrange multiplier | Pressure flux |
Constraint equations
In some cases the problem also involves constraint equations. In Abaqus/Standard the following constraints are included by using Lagrange multipliers:
| Problem | Constraint variable | Constraint |
| Hybrid solid (except C3D4H elements) | Pressure stress | Volumetric strain compatibility |
| Hybrid beam | Axial force | Axial strain compatibility |
| Hybrid beam | Transverse shear force | Transverse shear strain compatibility |
| Distributing coupling | Force | Coupling displacement compatibility |
| Distributing coupling | Moment | Coupling rotation compatibility |
| Contact | Normal pressure | Surface penetration |
| Contact with Lagrange friction | Shear stress | Relative shear sliding |
If the penalty method is used, the contact Lagrange multipliers may not be present.
Solving coupled field equations
In a general problem several (possibly nonlinear) coupled field equations of types \alpha = 1 , 2 , \ldots N must be solved and several different (possibly nonlinear) constraints of type j = 1 , 2 , \dots K must be satisfied simultaneously. For example, in a structural problem in which hybrid beam elements are used, \alpha = 1 might represent the displacement field and the equilibrium equations for the conjugate force and \alpha = 2 might represent the rotation field and the equilibrium equations for the conjugate moment, while j = 1 represents axial strain compatibility and j = 2 represents transverse shear strain compatibility.
Controlling the accuracy of the solution
The default solution control parameters defined in Abaqus/Standard are designed to provide reasonably optimal solution of complex problems involving combinations of nonlinearities as well as efficient solution of simpler nonlinear cases. However, the most important consideration in the choice of the control parameters is that any solution accepted as “converged” is a close approximation to the exact solution of the nonlinear equations. In this context “close approximation” is interpreted rather strictly by engineering standards when the default value is used, as described below.
You can reset many solution control parameters related to the tolerances used for field equations. If you define less strict convergence criteria, results may be accepted as converged when they are not sufficiently close to the exact solution of the system. Use caution when resetting solution control parameters. Lack of convergence is often due to modeling issues, which should be resolved before changing the accuracy controls.
You can select the type of equation for which the solution control parameters are being defined; for example, you can redefine the default controls for the displacement field and warping degree of freedom equilibrium equations only. By default, the solution control parameters will apply to all active fields in the model. See “Defining tolerances for field equations” in “Commonly used control parameters,” Section 7.2.2, for details.
Input File Usage: *CONTROLS, PARAMETERS=FIELD, FIELD=field
R _ {n} ^ {\alpha}, C _ {n} ^ {\alpha}, \tilde {q} _ {0} ^ {\alpha}, \tilde {q} _ {u} ^ {\alpha}, R _ {P} ^ {\alpha}, \epsilon^ {\alpha}, C _ {\epsilon} ^ {\alpha}, R _ {l} ^ {\alpha}
C _ {f}, \epsilon_ {l} ^ {\alpha}, \epsilon_ {d} ^ {\alpha}
Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle
on Specify: Field Equations: Apply to all applicable fields
or Specify individual fields: field
Terminology
Each field, , that is active in the problem is tested for convergence of the field equations. The following measures are used in deciding if an increment has converged:
rQ r _ { \mathrm { m a x } } ^ { \alpha } The largest residual in the balance equation for field \alpha .
\Delta u _ { \mathrm { m a x } } ^ { \alpha } The largest change in a nodal variable of type in the increment.
c _ { \mathrm { m a x } } ^ { \alpha } The largest correction to any nodal variable of type provided by the current Newton iteration.
e ^ { j } The largest error in a constraint of type j .
\bar { q } ^ { \alpha } ( t ) The instantaneous magnitude of the flux for field at time \mathbf { \Delta } _ { t , \tiny { \Psi } } averaged over the entire model (spatial average flux). This average is by default defined by the fluxes that the elements apply to their nodes and any externally defined fluxes:
\bar {q} ^ {\alpha} (t) \stackrel {\mathrm{def}} {=} \frac {1}{\sum_ {e = 1} ^ {E} \sum_ {n _ {e} = 1} ^ {N _ {e}} N _ {n _ {e}} ^ {\alpha} + N _ {e f} ^ {\alpha}} \left(\sum_ {e = 1} ^ {E} \sum_ {n _ {e} = 1} ^ {N _ {E}} \sum_ {i = 1} ^ {N _ {n _ {e}} ^ {\alpha}} | q | _ {i, n _ {e}} ^ {\alpha} + \sum_ {i = 1} ^ {N _ {e f} ^ {\alpha}} | q | _ {i} ^ {\alpha , e f}\right).
Here, E is the number of elements in the model, N _ { e } is the number of nodes in element e , N _ { n _ { \epsilon } } ^ { \alpha } is the number of degrees of freedom of type at node n _ { e } of element e, q | _ { i , n _ { e } } ^ { \alpha } is the magnitude of the total flux component that element e applies at its ith degree of freedom of type at its n _ { e } th node at time t, N _ { e f } ^ { \alpha } is the number of external fluxes for field \alpha (depends on element type, loading type, and number of loads applied to an element), and q | _ { i } ^ { \alpha , e f } is the magnitude of the ith external flux for field .
\tilde { q } ^ { \alpha } ( t ) An overall time-averaged value of the typical flux for field \alpha so far during this step including the current increment. Normally, \tilde { q } ^ { \alpha } ( t ) is defined as \bar { q } ^ { \alpha } averaged over all the increments in the step in which \bar { q } ^ { \alpha } is nonzero. The \bar { q } ^ { \alpha } for the current increment is recalculated after every iteration of the current increment.
\tilde {q} ^ {\alpha} (t) \stackrel {\mathrm{def}} {=} \frac {1}{N _ {t}} \sum_ {i = 1} ^ {N _ {t}} \bar {q} ^ {\alpha} (t | _ {i}),
where N _ { t } is the total number of increments so far in the step, including the current increment, in which \bar { q } ^ { \alpha } ( t | _ { i } ) > \epsilon ^ { \alpha } \tilde { q } ^ { \alpha } ( t | _ { i } ) . Here \bar { q } ^ { \alpha } ( t | _ { i } ) is the value of \overline { { q } } ^ { \alpha } at increment i and \epsilon ^ { \alpha } is a small number. The default for \epsilon ^ { \alpha } is 1 0 ^ { - 5 } , but in rare cases, you can change this default.
Alternatively, you can define a value for the average flux in the step, \tilde { q } _ { u } ^ { \alpha } . In this case, \tilde { q } ^ { \alpha } ( t ) = \tilde { q } _ { u } ^ { \alpha } throughout the step.
At the start of the step, \tilde { q } ^ { \alpha } is normally the value from the previous step (except for Step 1, when \tilde { q } ^ { \alpha } \ = \ 1 0 ^ { - 2 } by default). Alternatively, you can define an initial value for the time average flux, \tilde { q } _ { 0 } ^ { \alpha } , as described in “Modifying the initial time average flux” in “Commonly used control parameters,” Section 7.2.2. \tilde { q } ^ { \alpha } retains its initial value until an iteration is completed for which \bar { q } ^ { \alpha } > \epsilon ^ { \alpha } \tilde { q } ^ { \alpha } , at which time we redefine \tilde { q } ^ { \alpha } = \bar { q } ^ { \alpha } . (If \tilde { q } _ { u } ^ { \alpha } is defined, the value defined for \tilde { q } _ { 0 } ^ { \alpha } is ignored.)
\tilde { q } _ { \mathrm { m a x } } ^ { \alpha } The time-averaged value of the largest flux corresponding to the field during this step, excluding the current increment.
q _ { \mathrm { m a x } } ^ { \alpha } The largest flux corresponding to the field during the current iteration.
Average flux
The time-averaged value of the flux ( \tilde { q } ^ { \alpha } ( t ) ) is computed from the spatial average of the flux ( \overline { { q } } ^ { \alpha } ( t ) ) a t various instants in time. In some situations where only a small part of the model is active (the fluxes over the rest of the model are zero or very small), the spatial average of a flux over the entire model can be very small when compared to the spatial average over the active part of the model. Over a period of time this can result in a small value for the time-averaged value of the flux and in turn may lead to a convergence criterion that is very strict by engineering standards. To avoid such an excessively strict convergence criterion, Abaqus/Standard uses an algorithm to determine the active parts of a model at any given instant.
During an iteration any flux q _ { i } ^ { \alpha } ( t ) | < \epsilon _ { l } ^ { \alpha } \tilde { q } _ { \mathrm { m a x } } ^ { \alpha } is treated as inactive, and the corresponding degree of freedom is also marked inactive. \tilde { q } _ { \mathrm { m a x } } ^ { \alpha } is the time-averaged value of the largest flux in the model during the current step. The default value of \epsilon _ { l } ^ { \alpha } is 1 0 ^ { - 5 } ; you can redefine this parameter.
At the end of an iteration the largest flux in the model during the current iteration ( q _ { \mathrm { m a x } } ^ { \alpha } ) is compared with the time-averaged value of the largest flux ( \tilde { q } _ { \mathrm { m a x } } ^ { \alpha } ) . If q _ { \mathrm { m a x } } ^ { \alpha } ~ \ge ~ 0 . 1 \tilde { q } _ { \mathrm { m a x } } ^ { \alpha } , the spatial average is computed over only the active parts of the model; if q _ { \mathrm { m a x } } ^ { \alpha } < 0 . 1 \tilde { q } _ { \mathrm { m a x } } ^ { \alpha } , all inactive parts of the model are reclassified as active and the spatial average is computed over the entire model. The appropriate spatial average of the flux obtained in this manner is then used to compute the time-averaged flux \tilde { q } ^ { \alpha } ( t ) （204号 that is used in the convergence criterion. Setting \epsilon _ { l } ^ { \alpha } = 0 forces the spatial averages of a flux to be always computed over the entire model.
If you specify a value for the average flux in the step, \tilde { q } _ { u } ^ { \alpha } , \tilde { q } ^ { \alpha } ( t ) = \tilde { q } _ { u } ^ { \alpha } throughout the step.
Residuals
Most nonlinear engineering calculations will be sufficiently accurate if the error in the residuals is less than \frac { 1 } { 2 } \% . Therefore, Abaqus/Standard normally uses
r _ {\mathrm{max}} ^ {\alpha} \leq R _ {n} ^ {\alpha} \tilde {q} ^ {\alpha}
as the residual check, where you can define R _ { n } ^ { \alpha } (it is 0.005 by default). If this inequality is satisfied, largest incremental change in the corresponding solution variable, convergence is accepted if the largest correction to the solution, c _ { \mathrm { m a x } } ^ { \alpha } \Delta u _ { \mathrm { m a x } } ^ { \alpha } , is also small compared to the ,
c _ {\mathrm{max}} ^ {\alpha} \leq C _ {n} ^ {\alpha} \Delta u _ {\mathrm{max}} ^ {\alpha},
or if the magnitude of the largest correction to the solution that would occur with one more iteration, estimated as
c _ {e s t} ^ {\alpha} = \frac {\left(r _ {\max} ^ {\alpha}\right) ^ {i}}{\min \left(\left(r _ {\max} ^ {\alpha}\right) ^ {i - 1} , \left(r _ {\max} ^ {\alpha}\right) ^ {i - 2}\right)} c _ {\max} ^ {\alpha},
satisfies the same criterion:
c _ {e s t} ^ {\alpha} \leq C _ {n} ^ {\alpha} \Delta u _ {\mathrm{max}} ^ {\alpha}.
You can define C _ { n } ^ { \alpha . } the default value is 1 0 ^ { - 2 } .
The superscripts i , i - 1 , and refer to the iteration number, and \left( r _ { \operatorname* { m a x } } ^ { \alpha } \right) ^ { 0 } refers to the largest residual in field \alpha at the start of the first iteration of the increment. See “Commonly used control parameters,” Section 7.2.2, for more details on specifying C _ { n } ^ { \alpha } .
Zero flux
In some cases there may be zero flux in the equations of type anywhere in the model during some increments. Zero flux is defined as \bar { q } ^ { \alpha } \leq \epsilon ^ { \alpha } \tilde { q } ^ { \alpha } , where, as discussed earlier, \epsilon ^ { \alpha } has a default value of 1 0 ^ { - 5 } and the solution for field is accepted if r _ { \mathrm { m a x } } ^ { \alpha } \leq \epsilon ^ { \alpha } \tilde { q } ^ { \alpha } . If not, c _ { \mathrm { m a x } } ^ { \alpha } is compared to \Delta u _ { \mathrm { m a x } } ^ { \alpha } , and convergence for field is accepted when c _ { \mathrm { m a x } } ^ { \alpha } \leq C _ { \epsilon } ^ { \alpha } \Delta u _ { \mathrm { m a x } } . The default value of C _ { \epsilon } ^ { \alpha } is 1 0 ^ { - 3 } ; ; you can redefine this parameter.
Negligible response in some fields
Cases may arise where more than one field is active in the model yet there is negligible response in some of the fields in some increments. If some type of physical conversion factor, f _ { \beta } ^ { \alpha } , exists between active fields \alpha and \beta , \tilde { q } ^ { \alpha } in the above paragraph can be replaced by f _ { \beta } ^ { \alpha } C _ { f } \tilde { q } ^ { \beta } for those particular increments where \tilde { q } ^ { \alpha } is deemed too small ( \bar { q } ^ { \alpha } \leq \tilde { q } ^ { \alpha } < f _ { \beta } ^ { \alpha } C _ { f } \tilde { q } ^ { \beta } ) to be used realistically as part of the convergence criteria for field \alpha . . An example of f _ { \beta } ^ { \alpha } is a characteristic length to convert between force and moment.
Here, f _ { \beta } ^ { \alpha } is a factor calculated by Abaqus/Standard based on the problem definition and the fields involved and C _ { f } is a field conversion ratio that you can define. The default value for C _ { f } is 1.0. Currently, this concept is used only for converting between the fields associated with forces and moments, when f _ { \beta } ^ { \alpha } represents a characteristic element length.
Linear increments
Linear cases do not require more than one equilibrium iteration per increment. If
r _ {\mathrm{max}} ^ {\alpha} \leq R _ {l} ^ {\alpha} \tilde {q} ^ {\alpha}
for all \alpha , the increment is considered to be linear.
You can define R _ { l } ^ { \alpha } ; it is intended to be very small. The default value of R _ { l } ^ { \alpha } is 1 0 ^ { - 8 } . Any case that passes such a stringent comparison of the largest residual with the average flux magnitude in each field is considered linear and does not require further iteration. If this requirement is satisfied at some iteration after the first, the solution is accepted without any check on the size of the correction to the solution.
Nonquadratic convergence
In some cases quadratic convergence of the iterations is not possible because the Jacobian of the Newton scheme is approximated. If after I _ { P } iterations the convergence rate is only linear, Abaqus/Standard uses a looser tolerance,
r _ {\mathrm{max}} ^ {\alpha} \leq R _ {p} ^ {\alpha} \tilde {q} ^ {\alpha},
as the residual check. This tolerance modification is not applied when the quasi-Newton method is used, since it is normal for this method to require a larger number of iterations to converge.
You can define R _ { p } ^ { \alpha } , which is 2 \times 1 0 ^ { - 2 } by default. You can also define I _ { P } (by default, I _ { P } = 9 ; see “Controlling iteration”).
Convergence also requires that
c _ {\mathrm{max}} ^ {\alpha} \leq C _ {n} ^ {\alpha} \Delta u _ {\mathrm{max}} ^ {\alpha}.
Iteration continues until both criteria are satisfied for all active fields or the increment is abandoned.
When the active field is the displacement, the convergence criterion requiring the largest displacement correction to be small relative to the maximum displacement increment ( c _ { \mathrm { m a x } } ^ { \alpha } ~ \leq C _ { n } ^ { \alpha } \Delta u _ { \mathrm { m a x } } ^ { \alpha } ) is ignored when the maximum displacement increment itself is very small, as defined by △umax \Delta u _ { m a x } ^ { \alpha } \ : < \ : \epsilon _ { d } ^ { \alpha } f _ { \beta } ^ { \alpha } , where f _ { \beta } ^ { \alpha } is the characteristic element length. The default value for \epsilon _ { d } ^ { \alpha } is 1 0 ^ { - 8 } ; you can redefine this parameter.
Controlling iteration
Each increment of a nonlinear solution will usually be solved by multiple equilibrium iterations. The number of iterations may become excessive, in which case the increment size should be reduced and the increment attempted again. On the other hand, if successive increments are solved with a minimum number of iterations, the increment size may be increased. You can specify a number of time incrementation control parameters; some of them are described in this section, while the remainder are described in “Time integration accuracy in transient problems,” Section 7.2.4.
Input File Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION
I _ {0}, I _ {R}, I _ {P}, I _ {C}, I _ {L}, I _ {G}, I _ {S}, I _ {A}, I _ {J}, I _ {T}, I _ {S} ^ {c}, I _ {J} ^ {c}, I _ {A} ^ {c}
D _ {f}, D _ {C}, D _ {B}, D _ {A}, D _ {S}, D _ {H}, D _ {D}, W _ {G}
D _ {G}, D _ {M}, D _ {M} ^ {d y n}, D _ {M} ^ {d i f f}, D _ {L}, D _ {E}, D _ {R}, D _ {F}
D _ {T}
Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation; click More to see additional data tables