김경종
19 KiB
Input File Usage: *INERTIA RELIEF, FIXED
Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Inertia relief for the Types for Selected Step: Method: Fix at current loading
Removing inertia relief loads
You can specify that the inertia relief loads that were applied in the previous general analysis step should be removed in the current step.
Input File Usage: *INERTIA RELIEF, REMOVE
Abaqus/CAE Usage: Load module: Load Manager: Deactivate
Predefined fields
User-defined field variables can be specified in the same way as in static and dynamic analyses without inertia relief loads. See “Predefined fields,” Section 34.6.1.
Material options
Any of the mechanical constitutive models that are available in Abaqus/Standard for use in static, dynamic, or buckling analyses can be used with inertia relief (see Part V, “Materials,” for details on the material models available in Abaqus/Standard). Since inertia relief loading is calculated using the inertia properties of the model, the density must be specified (see “Density,” Section 21.2.1) to define the model’s inertia properties.
Elements
Most of the stress/displacement elements that are available in Abaqus/Standard for use in static, dynamic, and buckling analyses (including mass and rotary inertia elements and user elements) can be used. A warning will be issued when the model contains elements that do not have associated mass or inertia (for example, hydrostatic fluid elements and pore pressure elements). An error will be issued if the model contains elements that do not allow finite boundaries (for example, infinite elements and elastic element foundations). Although five degree of freedom shell elements can be used in a step with inertia relief loads, they may cause convergence difficulties if the model has no boundary conditions or insufficient boundary conditions. To improve convergence, these elements should be replaced with other conventional shell elements.
In the case of a substructure you must generate a reduced mass matrix for the substructure (see “Generating a reduced structural damping matrix for a substructure” in “Defining substructures,” Section 10.1.2). The reduced mass matrix is included in the global mass matrix of the entire model to compute rigid body accelerations and inertia relief loads. Inertia relief can be used only with substructures in a geometrically linear analysis. An error message is issued if inertia relief is used with substructures in a geometrically nonlinear analysis.
Output
In addition to the usual output variables available in Abaqus/Standard (see “Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables are provided specifically for inertia relief:
Variables for the entire model:
| IRX | Current coordinates of the reference point. |
| IRXn | Coordinate n of the reference point (n = 1, 2, 3). |
| IRA | Equivalent rigid body acceleration components. |
| IRAn | Component n of the equivalent rigid body acceleration (n = 1, 2, 3). |
| IRARn | Component n of the equivalent rigid body angular acceleration with respect to the reference point (n = 1, 2, 3). |
| IRF | Inertia relief load corresponding to the equivalent rigid body acceleration. |
| IRFn | Component n of the inertia relief load corresponding to the equivalent rigid body acceleration (n = 1, 2, 3). |
| IRMn | Component n of the inertia relief moment corresponding to the equivalent rigid body angular acceleration with respect to the reference point (n = 1, 2, 3). |
| IRRI | Rotary inertia about the reference point. |
| IRRIij | ij-component of the rotary inertia about the reference point (i ≤ j ≤ 3). |
| IRMASS | Whole model mass. |
For most cases inertia relief loads correspond to the product of “rigid body inertia” and the equivalent rigid body acceleration vector. However, when only a few rigid body directions are chosen as free directions for inertia relief, inertia relief loads are computed in all rigid body directions for output purposes, but equivalent rigid body accelerations are computed in only the free directions with the equivalent rigid body angular accelerations computed from the diagonal entries of the “rigid body inertia.”
Limitations
You need to be aware of limitations that may be encountered in analyses with inertia relief loads.
Internal boundary conditions and convergence in geometrically linear and nonlinear analysis
In a model containing internal boundary conditions that generate unbalanced internal forces or moments, such as is possible from certain elements (for example, SPRING1, DASHPOT1, SPRING2, DASHPOT2, or GAPUNI elements) or kinematic constraints (for example, coupling constraints, linear constraint equations, multi-point constraints, or surface-based tie constraints), inertia relief loads will not balance these internal forces or moments. If the model contains sufficient boundary conditions, these internal forces or moments will appear as nonzero reaction forces or moments. If the model does not contain sufficient boundary conditions, these internal forces or moments will appear as unconverged residual fluxes in the message file for geometrically linear as well as nonlinear analyses. The model
should be treated as having internal boundary conditions, with the unconverged residuals representing the reaction forces or moments needed to impose the internal boundary conditions. Ideally, the internal boundary conditions should be removed or sufficient boundary conditions should be added to the model.
Unconnected regions and analyses with contact
Inertia relief is not supported for models consisting of multiple unconnected regions, even if contact is defined between them. An exception is when tied contact is defined between the regions. In this case it is the user’s responsibility to ensure that different parts are tied in such a way that no rigid body motion is possible between them.
In addition, models involving contact with inertia relief loads may show poor convergence or fail to converge in cases when the surfaces are not in contact or when contact stabilization is used.
Mass and stiffness defined using matrices
Mass and stiffness cannot be defined using matrices in analyses with inertia relief loads.
Assembly loads
An analysis with inertia relief and assembly loads (see “Prescribed assembly loads,” Section 34.5.1) may experience poor convergence or no convergence if the model is not properly constrained by boundary conditions.
Input file template
*HEADING
...
*DENSITY
Data line to specify material density
*BOUNDARY
Data lines to specify zero-valued boundary conditions
**
*STEP (, NLGEOM) (, PERTURBATION)
Use the NLGEOM parameter to include nonlinear geometric effects;
it will remain active in all subsequent steps.
*STATIC (or *DYNAMIC)
...
*CLOAD and/or *DLOAD
Data lines to specify loads
*INERTIA RELIEF, ORIENTATION=orientation_name
Data lines to specify global (or local, if the ORIENTATION parameter is used) degrees of freedom that define free directions and to provide coordinates of a reference point
*END STEP
**
*STEP
*STATIC(or *DYNAMIC)
*INERTIA RELIEF, FIXED or REMOVE
Include the FIXED parameter to keep inertia relief loads fixed at their current values from the beginning of the step; include the REMOVE parameter to remove inertia relief loads from the beginning of the step.
*END STEP
11.2 Mesh modification or replacement
• “Element and contact pair removal and reactivation,” Section 11.2.1
11.2.1 ELEMENT AND CONTACT PAIR REMOVAL AND REACTIVATION
Products: Abaqus/Standard Abaqus/CAE
References
• “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 36.3.1
• *MODEL CHANGE
• “Defining a model change interaction,” Section 15.13.13 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
Element and contact pair removal/reactivation:
• can be used to simulate removal of part of the model, either temporarily or for the remainder of the analysis;
• allows reactivation of elements strain-free or with strain;
• can be used to save computational time when a contact pair is not needed;
• can be used only in general analysis steps; and
• can be used in a restart analysis only if it was used or activated in the original analysis.
Removing elements
You can remove specified elements from the model in a general analysis step. Just prior to the removal step, Abaqus/Standard stores the forces/fluxes that the region to be removed is exerting on the remaining part of the model at the nodes on the boundary between them. These forces are ramped down to zero during the removal step; therefore, the effect of the removed region on the rest of the model is completely absent only at the end of the removal step. The forces are ramped down gradually to ensure that element removal has a smooth effect on the model.
No further element calculations are performed for elements being removed, starting from the beginning of the step in which they are removed. The removed elements remain inactive in subsequent steps unless you reactivate them as described below.
Input File Usage: Use the following option to remove elements from the model:
*MODEL CHANGE, TYPE=ELEMENT, REMOVE
Abaqus/CAE Usage: Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Deactivated in this step
Removing elements in transient procedures
Care must be taken in removing elements in transient procedures. The nodal flux that the removed elements apply at the boundary with the rest of the model is ramped down over the step. In transient heat transfer, fully coupled temperature-displacement, or fully coupled thermal-electrical-structural analysis if the fluxes are high and the step is long, this ramping down may have the effect of cooling down or heating up the rest of the body. In dynamic analysis if the forces are high and the step is long, kinetic energy can be imparted to the remaining portion of the model. This problem can be avoided by removing the elements in a very short transient step prior to the rest of the analysis. This step can be done in a single increment.
Reactivating stress/displacement elements
Two distinct types of reactivation are provided for stress/displacement elements (including substructures): strain-free reactivation and reactivation with strain. Strain-free reactivation resets the initial configuration; reactivation with strain does not.
Although elements cannot be created within an analysis, a similar effect can be achieved by creating elements in the model definition, removing them in the first step, and subsequently reactivating them.
Strain-free reactivation
When stress/displacement elements are reactivated in a strain-free state, they become fully active immediately at the moment of reactivation (the start of the step in which they are reactivated). They are reset to an “annealed” state (zero stress, strain, plastic strain, etc.) in the configuration in which they lie at the start of the reactivation step. This configuration depends on whether a small- or large-displacement analysis is being conducted. Alternatively, reactivation in a nonvirgin state can be specified, as described below.
Since these elements are reactivated in a virgin state (i.e., with zero stress), they exert zero nodal forces on the rest of the model. This result allows reactivation to be done immediately, without an adverse effect on the smoothness of the solution.
After reactivation the strains and the deformation gradients are based on the displacements subsequent to the moment of reactivation, rather than on their total displacements. Thus, the current configuration at the start of the reactivation step is the new initial configuration for the element.
This kind of reactivation usually is used to model the creation of an undeformed and unstrained region of the model that is sharing a boundary with another, possibly stressed, deformed region. For example, in tunnel excavation an unstressed tunnel liner is added to line the walls of an already deformed tunnel (see “Stress-free element reactivation,” Section 1.1.11 of the Abaqus Example Problems Guide).
Input File Usage: Use the following option to reactivate elements in a strain-free state:
*MODEL CHANGE, ADD=STRAIN FREE (default)
Abaqus/CAE Usage: Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Reactivated in this step
Small-displacement analysis
In small-displacement analysis the displacements at reactivation are considered to be small; therefore, volume, mass, initial length, and orientation directions do not change.
Large-displacement analysis
In large-displacement analysis the new configuration can be significantly different from the original configuration specified in the model definition. The change in configuration may result from large deformation or rigid body motion. For the nodes of the reactivated elements to be in the correct position upon reactivation, these nodes must be shared by elements that are not removed. Otherwise, the nodes of the removed elements remain at the location occupied at the time of removal. For cases where an enclosed region of material is reactivated, the shared-node restriction may require that a duplicate set of elements whose material properties do not influence the stress solution be defined on top of the removed elements. These duplicate elements provide a means of tracking the position of the nodes of the removed elements.
Upon reactivation an element can have a significantly different volume or mass, so the mass matrix is reformed for the element. Any local orientations applicable to the element are redefined on the new configuration. For shell and membrane elements, however, the thickness of the reactivated elements is the thickness as specified at the start of the analysis by the element’s section definition, a nodal thickness definition (“Nodal thicknesses,” Section 2.1.3), or an import definition (“Transferring results between Abaqus analyses: overview,” Section 9.2.1).
The current normals on structural elements at the moment of reactivation become new initial normals for that element. The current normal is the element’s original normal (as specified in the model definition) rotated by the nodal rotation at the moment of reactivation. This scheme preserves the angle between the normals of reactivated elements and those of the elements with which they share nodes. (Usually, this angle should be zero and the normals should be identical, such as when a strain-free layer is added to an already deformed shell or beam. This can be achieved by ensuring that the normals are identical in the model definition.) If the reactivated structural elements share nodes with only non-structural elements (elements that do not provide stiffness to rotational degrees of freedom), duplicate structural elements are required so that the rotational degrees of freedom at the shared nodes will follow the deformation and rigid body motion before reactivation.
In a large-displacement analysis an element that is being reactivated strain free fits into whatever configuration is given by its nodes at the moment of reactivation. You must ensure that this configuration is meaningful and is not severely distorted. Abaqus/Standard will apply geometry checks on the reactivated elements; these checks are the same as the checks that are done in the analysis input file processor. Warnings are printed in the message file if the elements seem inappropriately distorted; and error messages are given if the distortion is severe, in which case the analysis will be stopped. If a geometry check on an element produces a warning or an error message, its current coordinates—and normals if applicable—are printed to the message file for your inspection. The current coordinates can be printed for all elements being reactivated by requesting detailed printout for element removal/reactivation, as explained in “The Abaqus/Standard message file” in “Output,” Section 4.1.1.
Reactivating axisymmetric elements
Abaqus/Standard will not stop the analysis if an axisymmetric element has a very small negative radial coordinate at reactivation (if the magnitude of the radial coordinate is less than 1 0 ^ { - 4 } times the average element length). In this case a warning is printed, and a radial coordinate of zero is assumed. If the radial coordinate is negative and larger than 1 0 ^ { - 4 } times the average element length in magnitude, the analysis will stop.
For axisymmetric-asymmetric elements (SAXA and CAXA) the displacements at reactivation are considered small even in large-displacement analysis because these elements require an axisymmetric original configuration, but the configuration given by the nodes of these elements at reactivation would not, in general, be axisymmetric. Therefore, the original configuration is assumed not to change for these elements.
Reactivating coupled temperature-displacement and coupled thermal-electrical-structural elements
In a fully coupled temperature-displacement analysis and a fully coupled thermal-electrical-structural analysis, continuum elements attain their full mechanical stiffness immediately upon strain-free reactivation; however, to ensure smoothness of the solution, thermal conductivity is ramped up from zero over the step.
Reactivating spring elements and substructures
If spring elements or substructures are reactivated “without strain,” the configuration at the moment of reactivation represents the zero-displacement state of the element; the forces in the spring or substructures are based on relative displacements subsequent to the moment of reactivation.
Reactivation with strain
Elements reactivated with strain start in an annealed state unless reactivation in a nonvirgin state is specified, as described below.
The following scheme is implemented for the elements during the reactivation step: Let u ^ { g } represent the displacements of the nodes of this element, which are the displacements as shared by the rest of the model or as specified by boundary conditions. In general, these displacements can vary with time over the reactivation step. At any time in the reactivation step Abaqus/Standard enforces displacements, u ^ { e } , for the element:
u ^ {e} = \alpha (t) u ^ {g},
where \alpha ( t ) is a parameter that ramps linearly from 0 to 1 during the step. Thus, during the step the displacements felt by the reactivated elements ramp up to their actual values. To produce a consistent stiffness matrix, the element stiffness is also multiplied by \alpha ( t ) ; therefore, the rest of the model experiences the reactivated elements as though their stiffnesses were ramped up during the step.
This ramping up of displacements instead of direct ramping up of element forces ensures that the strain in the element ramps up from zero to the strain given by the displacement of its nodes. This gradual