김경종
251 lines
19 KiB
Markdown
251 lines
19 KiB
Markdown
<!-- source-page: 931 -->
|
|
|
|
ramping up of strains is desirable so that the response of history-dependent materials can be integrated gradually.
|
|
|
|
Subsequent to the end of the reactivation step, the strains in reactivated elements correspond to the displacements of their nodes from their initial configuration, rather than to their displacements since the moment of reactivation. This is appropriate, for example, in the refueling of a nuclear reactor, where the new fuel assembly must conform to the distortion of its old neighbors.
|
|
|
|
This reactivation scheme does not work for the rotations of shell elements that have five degrees of freedom per node because a total rotation is not stored at those nodes. Consequently, reactivation with strain is not allowed for these elements.
|
|
|
|
If an element is reactivated with strain after having been previously reactivated strain free, the strains are based on the displacements from the configuration in which the element was reactivated strain free (because this defined the new initial configuration for the element). In this case the $u ^ { g }$ in the formula above should be interpreted as the displacement of the node relative to the position in which the element was reactivated strain free.
|
|
|
|
Input File Usage: Use the following option to reactivate elements with strain:
|
|
|
|
\*MODEL CHANGE, ADD=WITH STRAIN
|
|
|
|
Abaqus/CAE Usage: Interaction module: Create Interaction: Model Change: Definition:
|
|
|
|
Region, Activation state of region elements: Reactivated in this step; toggle on Reactivated elements with strain (when applicable)
|
|
|
|
# Reactivating elements with rebar
|
|
|
|
Rebars are reactivated strain free or with strain exactly like the element in which they are defined. The annealing that takes place upon reactivation is also applied to rebars in the model. Reactivation of rebars can also be done in a nonvirgin state.
|
|
|
|
# Reactivating other element types
|
|
|
|
During reactivation of all element types other than stress/displacement elements, substructures, and contact elements, the nodal forces caused by stress in the element and by distributed loads are scaled by a value that ramps from zero to one during the reactivation step. (The nodal fluxes are scaled similarly for heat transfer elements.) In effect this scaling ramps the element stiffness up from zero during the step; for elements with mass or damping this scaling also ramps up the mass or damping during the step.
|
|
|
|
During the reactivation step the thermal conductivity of heat transfer elements and the permeability of pore pressure elements are ramped up from zero over the step.
|
|
|
|
User-defined elements can be removed and reactivated. User subroutine UEL is not called in steps in which the element is being removed or has already been removed.
|
|
|
|
Input File Usage: \*MODEL CHANGE, ADD
|
|
|
|
Abaqus/CAE Usage: Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Reactivated in this step
|
|
|
|
<!-- source-page: 932 -->
|
|
|
|
# Removing and reactivating contact pairs
|
|
|
|
You can remove specified slave and master surfaces from the model in a general analysis step. Contact pair removal and reactivation is explained in “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 36.3.1.
|
|
|
|
Input File Usage: \*MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE or ADD
|
|
|
|
Abaqus/CAE Usage: Use the following option to remove contact pairs:
|
|
|
|
Interaction module: Create Interaction: Surface-to-surface contact (Standard) or Self-contact (Standard): toggle off Active in this step
|
|
|
|
Use the following option to reactivate contact pairs:
|
|
|
|
Interaction module: Create Interaction: Surface-to-surface contact (Standard) or Self-contact (Standard): toggle on Active in this step
|
|
|
|
# Removing and reactivating contact elements
|
|
|
|
Contact elements are removed and reactivated by Abaqus/Standard in the same way as contact pairs, as described in “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 36.3.1.
|
|
|
|
Input File Usage: \*MODEL CHANGE, TYPE=ELEMENT, REMOVE or ADD
|
|
|
|
Abaqus/CAE Usage: Use the following option to remove contact elements:
|
|
|
|
Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Deactivated in this step
|
|
|
|
Use the following option to reactivate contact elements:
|
|
|
|
Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Reactivated in this step
|
|
|
|
# Modeling issues
|
|
|
|
In some cases element removal/reactivation may cause numerical problems. The following guidelines can be used to reduce the chance of difficulty:
|
|
|
|
• If elements are removed in a static stress analysis and this removal leaves a region of the model with an unconstrained rigid body mode, solver problems will occur and the analysis most likely will fail to converge. Therefore, ensure that the remainder of the model is constrained sufficiently.
|
|
• If elements that are connected to a contact pair are removed, the contact pair should also be removed to avoid solver problems.
|
|
• If all elements attached to a node constrained with a multi-point constraint or a linear constraint equation are being removed, this node should be the dependent node of the multi-point constraint or linear constraint equation.
|
|
|
|
<!-- source-page: 933 -->
|
|
|
|
In some cases element removal may cause Abaqus/Standard to report extra unconnected regions in the message file. These messages can be safely ignored.
|
|
|
|
# Removing or reactivating elements and contact pairs in a restart analysis
|
|
|
|
Elements or contact pairs can be removed or reactivated in a restart analysis (“Restarting an analysis,” Section 9.1.1) only if elements or contact pairs were removed or reactivated in the original analysis. In situations where it is expected that the addition or removal of elements or contact pairs will be required in a restart analysis, but there is no such need in the original analysis, you must activate element or contact pair removal/reactivation in the original analysis. Activating this capability does not add or remove any elements or contact pairs; it only prepares Abaqus/Standard to allow for these changes in a subsequent restart analysis.
|
|
|
|
Input File Usage: Use the following option to activate element or contact pair removal/reactivation:
|
|
|
|
\*MODEL CHANGE, ACTIVATE
|
|
|
|
Abaqus/CAE Usage: Interaction module: Create Interaction: Model Change: Definition: Restart
|
|
|
|
# Procedures
|
|
|
|
Elements or contact pairs cannot be removed or reactivated in a linear perturbation step (see “General and linear perturbation procedures,” Section 6.1.3) or in a static Riks step (see “Unstable collapse and postbuckling analysis,” Section 6.2.4). For elements to be absent in such steps, they must have been inactive at the end of the previous general analysis (nonperturbation) step.
|
|
|
|
# Initial conditions
|
|
|
|
When elements are added back into the model, they are usually assumed to be “annealed”; that is, they have zero plastic strain, creep strain, etc. and zero stress at the start of the step in which they are reactivated. It is possible to reactivate an element so that it starts with a nonzero stress, equivalent plastic strain, and, if relevant, backstress (in a nonvirgin state).
|
|
|
|
# Reactivation in a nonvirgin state
|
|
|
|
To reactivate elements with nonzero stress, define initial stress conditions (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) to specify the required stress in the model definition. Then the elements must be removed in the first step of the analysis. When reactivated, they will have the initial stress specified. The reactivation is done immediately, so the initial stress (which is applied in full during the first increment) must be self-equilibrating to avoid convergence issues.
|
|
|
|
If the elements were not removed in the first step, if they were removed again after the first step, or if initial conditions were not specified for them, they will have zero stresses when reactivated.
|
|
|
|
In a similar manner a material can be reactivated with a nonzero initial equivalent plastic strain and, if relevant, backstress.
|
|
|
|
<!-- source-page: 934 -->
|
|
|
|
When elements are reactivated, any applied initial stress is not displayed in the zero increment frame.
|
|
|
|
<table><tr><td>Input File Usage:</td><td>Use the following option to specify initial stress conditions:*INITIAL CONDITIONS, TYPE=STRESSUse the following option to specify initial equivalent plastic strain and backstress:*INITIAL CONDITIONS, TYPE=HARDENING</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Use the following options to specify the initial stress conditions:Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Stress for the Types for Selected StepUse the following options to specify the initial equivalent plastic strain and backstress:Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step</td></tr></table>
|
|
|
|
# Boundary conditions
|
|
|
|
The nodal variables of removed elements are not changed when the elements are removed. You can reset these variables by defining a boundary condition while the elements are inactive (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1).
|
|
|
|
# Loads
|
|
|
|
Distributed and concentrated loads that are applied in an area where elements are removed or reactivated may need to be modified.
|
|
|
|
# Distributed loads
|
|
|
|
Any distributed loads, fluxes, flows, and foundations specified for inactive elements are also inactive. However, unless you explicitly remove them, records of these loads are still kept and are listed in the data (.dat) file as though the elements were still present. Continuation of loads across steps is not affected by removal; on element reactivation unremoved distributed loads are also reactivated.
|
|
|
|
By default, if a distributed load is applied to an element that is being reactivated in a step, the distributed load magnitude is scaled up linearly from zero to its end-of-step value during the step. If such a load is applied with an amplitude reference, the magnitude value given by the amplitude reference is scaled again by a value that ramps from zero to one throughout the step. This scheme ensures that reactivation has a smooth effect on the solution, even in cases where a distributed load with an amplitude reference on a reactivated element is carried over from a previous step.
|
|
|
|
# Concentrated loads
|
|
|
|
Concentrated loads or fluxes are not removed when the surrounding elements are removed; therefore, you must ensure that any concentrated loads or fluxes that are carried solely by removed elements are
|
|
|
|
<!-- source-page: 935 -->
|
|
|
|
also removed. Otherwise, a solver problem will occur during the removal step (a force is applied to a degree of freedom with zero stiffness). Concentrated loads or fluxes should be ramped up when they are reintroduced along with reactivated elements.
|
|
|
|
# Predefined fields
|
|
|
|
The nodal variables of removed elements are not changed directly when the elements are removed. You can reset these variables by defining temperature or other predefined field variables while the elements are inactive (see “Predefined fields,” Section 34.6.1). For example, elements that are removed in a stress/displacement analysis can be reintroduced at a different temperature by setting the temperatures at the nodes on these elements to the desired value while the elements are inactive due to removal.
|
|
|
|
# Temperatures
|
|
|
|
The temperatures at the start of the reactivation step become the initial temperatures for reactivated elements; thermal strains (and, thus, also the thermal stresses) are based on the temperature change subsequent to the instant of reactivation (see “Thermal expansion,” Section 26.1.2).
|
|
|
|
# Material options
|
|
|
|
On annealing, compaction-related quantities—such as the yield stress in hydrostatic compression, $p _ { c } ,$ , in crushable foam plasticity (“Crushable foam plasticity models,” Section 23.3.5); the yield stress in hydrostatic compression, , in cap plasticity (“Modified Drucker-Prager/Cap model,” Section 23.3.2); and the void volume fraction, f, in porous metal plasticity (“Porous metal plasticity,” Section 23.2.9)—are reset to the values they had at the start of the analysis.
|
|
|
|
For porous materials the porosity, n, is reset to its initial value and the saturation, s, retains its value from the instant of removal (see “Pore fluid flow properties,” Section 26.6.1).
|
|
|
|
Elements with a user-defined material type can be removed and reactivated; user subroutines UMAT and UMATHT are not called while the elements are inactive. On reactivation the stresses and strains in user subroutine UMAT are set to zero, and conductivity and heat fluxes defined in user subroutine UMATHT are ramped up from zero during the reactivation step. Solution-dependent state variables must be reset in user subroutine UMAT, UMATHT, or SDVINI, which will be called on reactivation.
|
|
|
|
# Elements
|
|
|
|
Removal is not currently supported for rigid, cohesive, gasket, and piezoelectric elements. All other element types in Abaqus/Standard can be removed and reactivated. See “Choosing the appropriate element for an analysis type,” Section 27.1.3.
|
|
|
|
# Output
|
|
|
|
Output is not available for elements or contact surfaces that have been removed. Inactive elements and contact surfaces are visible in Abaqus/CAE.
|
|
|
|
<!-- source-page: 936 -->
|
|
|
|
Input file template
|
|
```txt
|
|
*HEADING
|
|
...
|
|
*STEP
|
|
*STATIC
|
|
...
|
|
** Remove all elements in element set SIDE
|
|
*MODEL CHANGE, REMOVE
|
|
SIDE,
|
|
** Remove contact pair (SLAVE1, MASTER1)
|
|
*MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE
|
|
SLAVE1, MASTER1
|
|
...
|
|
*END STEP
|
|
**
|
|
*STEP
|
|
*STATIC
|
|
...
|
|
** Reactivate elements in element set SIDE
|
|
*MODEL CHANGE, ADD=STRAIN FREE
|
|
SIDE,
|
|
** Reactivate contact pair (SLAVE1, MASTER1)
|
|
*MODEL CHANGE, TYPE=CONTACT PAIR, ADD
|
|
SLAVE1, MASTER1
|
|
...
|
|
*END STEP
|
|
```
|
|
|
|
<!-- source-page: 937 -->
|
|
|
|
# 11.3 Geometric imperfections
|
|
|
|
• “Introducing a geometric imperfection into a model,” Section 11.3.1
|
|
|
|
<!-- source-page: 938 -->
|
|
|
|
<!-- source-page: 939 -->
|
|
|
|
# 11.3.1 INTRODUCING A GEOMETRIC IMPERFECTION INTO A MODEL
|
|
|
|
Products: Abaqus/Standard Abaqus/Explicit
|
|
|
|
# References
|
|
|
|
• “Unstable collapse and postbuckling analysis,” Section 6.2.4
|
|
• \*IMPERFECTION
|
|
|
|
# Overview
|
|
|
|
A geometric imperfection pattern:
|
|
|
|
• is generally introduced in a model for a postbuckling load-displacement analysis;
|
|
• can be defined as a linear superposition of buckling eigenmodes obtained from a previous eigenvalue buckling prediction or eigenfrequency extraction analysis performed with Abaqus/Standard;
|
|
• can be based on the solution obtained from a previous static analysis performed with Abaqus/Standard; or
|
|
• can be specified directly.
|
|
|
|
# General postbuckling analysis
|
|
|
|
In Abaqus/Standard the Riks method (“Unstable collapse and postbuckling analysis,” Section 6.2.4) can be used to solve postbuckling problems, both with stable and unstable postbuckling behavior. However, the exact postbuckling problem often cannot be analyzed directly due to the discontinuous response (bifurcation) at the point of buckling. To analyze a postbuckling problem, you must turn it into a problem with continuous response instead of bifurcation, which can be accomplished by introducing a geometric imperfection pattern in the “perfect” geometry so that there is some response in the buckling mode before the critical load is reached.
|
|
|
|
# Introducing geometric imperfections
|
|
|
|
Imperfections are usually introduced by perturbations in the geometry. Abaqus offers three ways to define an imperfection: as a linear superposition of buckling eigenmodes, from the displacements of a static analysis, or by specifying the node number and imperfection values directly. Only the translational degrees of freedom are modified. Abaqus will then calculate the normals using the usual algorithm based on the perturbed coordinates. Unless the precise shape of an imperfection is known, an imperfection consisting of multiple superimposed buckling modes can be introduced (“Eigenvalue buckling prediction,” Section 6.2.3).
|
|
|
|
The usual approach involves two analysis runs with the same model definition, using Abaqus/Standard to establish the probable collapse modes and either Abaqus/Standard or Abaqus/Explicit to perform the postbuckling analysis:
|
|
|
|
<!-- source-page: 940 -->
|
|
|
|
1. In the first analysis run perform an eigenvalue buckling analysis with Abaqus/Standard on the “perfect” structure to establish probable collapse modes and to verify that the mesh discretizes those modes accurately. Write the eigenmodes in the default global system to the results file as nodal data (“Output to the data and results files,” Section 4.1.2).
|
|
2. In the second analysis run use Abaqus/Standard or Abaqus/Explicit to introduce an imperfection in the geometry by adding these buckling modes to the “perfect” geometry. The lowest buckling modes are frequently assumed to provide the most critical imperfections, so usually these are scaled and added to the perfect geometry to create the perturbed mesh. The imperfection thus has the form
|
|
|
|
$$
|
|
\Delta \pmb {x} _ {i} = \sum_ {i = 1} ^ {M} w _ {i} \phi_ {i},
|
|
$$
|
|
|
|
where $\phi _ { i }$ is the $i ^ { t h }$ mode shape and $w _ { i }$ is the associated scale factor.
|
|
|
|
You must choose the scale factors of the various modes; usually (if the structure is not imperfection sensitive) the lowest buckling mode should have the largest factor. The magnitudes of the perturbations used are typically a few percent of a relative structural dimension such as a beam cross-section or shell thickness.
|
|
|
|
3. Use either Abaqus/Standard or Abaqus/Explicit to perform the postbuckling analysis.
|
|
|
|
• In Abaqus/Standard perform a geometrically nonlinear load-displacement analysis of the structure containing the imperfection using the Riks method. In this way the Riks method can be used to perform postbuckling analyses of “stiff” structures that show linear behavior prior to buckling, if perfect. By performing a load-displacement analysis, other important nonlinear effects, such as material inelasticity or contact, can be included.
|
|
• In Abaqus/Explicit perform a postbuckling analysis on the perturbed structure.
|
|
|
|
Abaqus imports imperfection data through the user node labels. Abaqus does not check model compatibility between both analysis runs. Node set definitions in the original model and the model with the imperfection may be different. Care must be taken for models in which Abaqus generates additional nodes (for example, the nodes generated for contact surfaces on 20-node brick elements). In such cases you have to ensure that the models for both analysis runs are identical and that the nodal information for the generated nodes is written to the results file.
|
|
|
|
If the model is defined in terms of an assembly of part instances, the part (.prt) file from the original analysis is required to read the eigenmodes from the results file. Both the original model and the subsequent model must be defined consistently in terms of an assembly of part instances.
|
|
|
|
# Defining an imperfection based on eigenmode data
|
|
|
|
To define an imperfection based on the superposition of weighted mode shapes, specify the results file and step from a previous eigenfrequency extraction or eigenvalue buckling prediction analysis. Optionally, you can import eigenmode data for a specified node set.
|
|
|
|
Input File Usage: \*IMPERFECTION, FILE=results\_file, STEP=step, NSET=name
|