Mesh-to-mesh solution mapping | ||||||
|
| |||||
ProductsAbaqus/Standard
When to remesh
Abaqus/Standard uses a Lagrangian formulation: the mesh is attached to the material and, thus, deforms with the material. When the strains become large in geometrically nonlinear analyses, the elements may become so severely distorted that they no longer provide a good discretization of the problem. Severe distortion may occur in rubber elasticity problems or in plastic or viscoplastic calculations, especially when modeling manufacturing processes. When severe distortion occurs, it is necessary to remesh: to create a new mesh better designed to continue the analysis and to map the old-model solution onto this mesh.
You must decide when remeshing is needed. This decision can be assisted by looking at the magnitude of strains that have occurred during the phase of the analysis using a particular mesh, as discussed later. When remeshing is required, a new mesh for the deformed object must be generated using the mesh generation capability in Abaqus or an external mesh generator. The analysis is then continued as a new problem using the new mesh. In most cases it will be desirable to transfer the solution from the old mesh to the new mesh.
Discontinuity in the solution
Whenever the solution is mapped from another mesh, you can expect that there will be some discontinuity in the solution because of the change in the mesh and as a consequence of the solution mapping algorithm. If the discontinuity is significant, it is an indication that the meshes are too coarse or that the remeshing should have been done at an earlier stage before too much distortion occurred.
The remeshing technique works well, provided that the meshes are sufficiently fine for the problem and that the remeshing is done before the elements become too distorted.
Remeshing criterion
The first requirement for remeshing is some indication that the mesh is becoming distorted in regions where this distortion could cause the solution to be inaccurate. One possible criterion for remeshing would be extreme element distortion in areas where high strain gradients need to be resolved accurately. Inaccuracy is less of a concern if the distorted elements have moved into an area where further changes in the strain field are uniform; the elements can represent states of constant strain accurately no matter how distorted they are. Ultimately, however, the decision to remesh is a matter of judgment.
Generating a new mesh
Once you have decided that the current mesh is inadequate, a new mesh that is more suitable to the current state of the problem must be generated by using the mesh generation capabilities in Abaqus or an external mesh generator. Deformed configuration plots may be useful to provide data about the current shape of the object being modeled. Usually the external surface can be defined for use in a mesh generator from the results file output at the sets of nodes that form the surfaces of the body. See Erosion of material (sand production) in an oil wellbore and Upsetting of a cylindrical billet: quasi-static analysis with mesh-to-mesh solution mapping (Abaqus/Standard) and adaptive meshing (Abaqus/Explicit).
Remeshing a contact problem
In a region of contact the new mesh must conform closely to the shape of the surface from the old analysis. This requirement is especially important for problems involving contact between two deformable bodies; if the surfaces defined by the new mesh are even slightly different from the surfaces in the old analysis, the contact algorithms may fail to converge.
Specifying the solution to be interpolated onto the new mesh
The simulation is continued by interpolating the solution onto the new mesh from the output databases generated with the old mesh.
Specifying the time at which the solution must be read
Solution transfer will occur, by default, from the latest step and increment for which solution variables are available. Alternatively, you can specify the step and increment at which the old solution will be read.
Input File Usage
MAP SOLUTION, STEP=step, INC=increment
Obtaining equilibrium
An initial step should be included to allow Abaqus/Standard to check for equilibrium after this interpolation has been done. By default, Abaqus/Standard resolves the stress unbalance linearly over the step (see the discussion on establishing equilibrium when an initial stress field is applied in Initial conditions in Abaqus/Standard and Abaqus/Explicit). You can choose to have the stress unbalance resolved in the first increment instead.
Input File Usage
Use the following option to have Abaqus/Standard resolve the stress unbalance linearly over the step:
MAP SOLUTION, UNBALANCED STRESS=RAMP
Use the following option to have Abaqus/Standard resolve the stress unbalance in the first increment of the step:
MAP SOLUTION, UNBALANCED STRESS=STEP
Translating and rotating the old-job mesh
The mesh from the old job can be repositioned prior to performing the mapping by giving a translation and/or rotation relative to the global origin. Specify a translation by giving a translation vector. Specify a rotation by giving two points to define a rotation axis plus a right-handed angular rotation around that axis.
Input File Usage
MAP SOLUTION, STEP=step, INC=increment translation vector data rotation axis and angular rotation data
Required output from the old job
The files required for restart and the output database must be requested for the old job. Nodal displacement results are not output automatically from the old job; you must explicitly request output of the displacement variable U for all nodes, as described in Node output. Alternatively, you can request preselected field output and obtain node displacement output sufficient for solution mapping.
In fully coupled procedures you must request nodal output of the coupled field variable to the output database (see Table 1).
|
Identifying the old job
Specify the name of the old job from which restart and results data will be obtained by using the oldjob parameter in the command for running Abaqus or by answering a request made by the command procedure (see Abaqus/Standard and Abaqus/Explicit execution). The files required from the old job include: the restart file (.res), the output database (.odb), the model database (.mdl), the state database (.stt), and the part (.prt) file.
Solution mapping algorithm
Solution mapping operates by interpolating results from nodes in the old mesh to points (either nodes or integration points) in the new mesh. The first step, therefore, involves associating solution variables with nodes in the old mesh. For nodal solution variables, such as nodal temperature or pore pressure, the association is already made. For integration point variables Abaqus obtains the solution variables at the nodes of the old mesh by extrapolating values from the integration points to the nodes of each element and then averaging these values over all similar elements abutting each node.
Next, the location of each point in the new mesh is obtained with respect to the old mesh. The new mesh points include integration points in all cases and nodes in procedures that record nodal state in addition to displacements (for example, nodal temperatures in coupled temperature-displacement procedures).
The element (in the old mesh) in which the point lies is found, and the point's location in that element is obtained. (This procedure assumes that all points in the new mesh lie within the bounds of the old mesh: warning messages are issued if this is not so, and the values of the variables are set to zero.)
The variables are then interpolated from the nodes of the old element to the points in the new model.
All necessary variables are interpolated automatically in this way so that the solution can proceed with the new mesh.
Solution diffusion
This algorithm introduces some diffusion in the mapped solution. The effect of the diffusion scales with the solution gradient in the old mesh; hence, even for regions of the model where the mesh does not change from the old to the new model, diffusion due to the mapping can result in significantly different mapped quantities when the old-mesh solution gradient is high. You can moderate this effect by refining the old mesh in regions where solution gradients are high or by remeshing earlier.
Procedures
The solution mapping capability is supported for the following procedures:
Initial conditions
The solution mapped from the initial analysis forms the initial conditions for the remeshed analysis. Initial conditions such as temperature for a pure stress/displacement analysis can be specified. Any other specified initial conditions will be ignored.
Boundary conditions
Boundary conditions are not carried over from the old mesh to the new mesh. The boundary conditions applied at the beginning of the remeshed analysis should normally be the same as those in effect at the step and increment selected from the initial analysis. Although boundary conditions can be changed, the problem may fail to converge if the structure is far from an equilibrium state.
There are no restrictions on applying boundary conditions in a mapped solution analysis. Boundary conditions can be applied to all available degrees of freedom in the same way as they are applied in an analysis without a mapped solution (see Boundary conditions in Abaqus/Standard and Abaqus/Explicit).
Loads
There are no restrictions on applying loads in a mapped solution analysis. Loads can be applied in the same way as they are applied in an analysis without a mapped solution.
The loads applied at the beginning of the remeshed analysis should normally be the same as those in effect at the end of the initial analysis. Although the loads can be changed, the problem may fail to converge if the structure is far from an equilibrium state.
Predefined fields
Temperature and field variables are mapped from the old mesh to the new mesh. If the number of field variables is changed in the remeshed analysis, the number common to both analyses will be transferred. Predefined fields can be modified in the same way as they are modified in an analysis without solution mapping (see Predefined Fields).
Material options
Any of the mechanical constitutive models available in Abaqus can be used in a mapped solution analysis (see Abaqus Materials Guide). There is no restriction on agreement between material models in the old and new analyses. The solution mapping algorithm will transfer those variables common to both models. You must ensure that the material models are compatible.
Elements
The solution mapping capability can be used only with continuum elements (see Solid (continuum) elements).
Output
There is no output specific to a mapped solution analysis. Output can be requested in the same way as in an analysis without a mapped solution. The output variables available in Abaqus are listed in Abaqus/Standard output variable identifiers.
Input file template
HEADING NODE Data lines to define the new-model nodes occupying the space of the old model in its deformed configuration ELEMENT Data lines to define the new-model elements occupying the space of the old model in its deformed configuration … MAP SOLUTION, STEP=step, INC=inc translation and rotation data STEP STATIC (or COUPLED TEMPERATURE-DISPLACEMENT or GEOSTATIC or SOILS or VISCO) … END STEP