natural_image

Geometric mesh grid with triangular mesh overlay, no text or symbols present

Figure 12.3.3–4 Initial mesh and Mises stress distribution for a plane stress plate with a hole, subjected to a uniform horizontal boundary traction. # Minimum/maximum control Figure 12.3.3–5 illustrates the adaptive mesh that was generated by Abaqus/CAE when the user selected the minimum/maximum control method and specified the two error targets $( \eta _ { \mathrm { m i n } }$ and $\eta _ { \mathrm { m a x } } )$ . In this example $\eta _ { \mathrm { m i n } } { = } 5 \%$ and $\eta _ { \mathrm { m a x } } { = } 1 \%$ , and the mesh bias is set to the default setting. These settings result in a mesh that focuses tightly around the hole, the stress riser, while transitioning smoothly to a relatively coarse mesh away from the hole. # Uniform error distribution Figure 12.3.3–6 illustrates the adaptive mesh that was generated by Abaqus/CAE when the user selected the uniform error distribution method and specified the single uniform error indicator target ( ). In this example $\scriptstyle \eta = 1 \%$ . This setting results in a mesh that focuses around the hole, the stress riser, while also refining the mesh in less stressed regions. # Impact of additional remeshing rule settings You specify the sizing method when you create a remeshing rule, and the sizing method calculates new element sizes during the adaptive remeshing process. However, the following additional settings in the remeshing rule can affect the mesh generated by Abaqus/CAE, regardless of the sizing method that you selected: • region selection, • step and frame selection, 

natural_image

Geometric pattern with nested triangles and a central circle, no text or symbols present

Figure 12.3.3–5 Adaptive remesh resulting from the minimum/maximum control sizing method. 

natural_image

Symmetrical geometric pattern with triangular mesh lines and a central circle (no text or symbols)

Figure 12.3.3–6 Adaptive remesh resulting from the uniform error distribution sizing method. • size constraints, • approximate maximum number of elements, and • refinement and coarsening rate factors. # Region selection Sizing methods are defined across sets of elements, corresponding to the regions over which the remeshing rules were applied in Abaqus/CAE. Within each set of elements, Abaqus/CAE applies the sizing operation to the error indicator variables specified in the remeshing rule. The results of the sizing operation are based on the extrapolation of whole element calculations to the nearest nodes, and the results are node based. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Edit Region # Step and frame selection Abaqus applies sizing operations to error indicator variables from only the last available frame in a specified step. See “Error indicator characteristics” in “Selection of error indicators influencing adaptive remeshing,” Section 12.3.2, for a discussion of how your selection of the step, frame, and error indicator can affect your ability to capture the response in transient analyses. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Step and Indicator: Step; select the step to which the rule is applied and Mesh module: Create Remeshing Rule: Step and Indicator: Output Frequency; choose either Last increment of step or All increments of step # Size constraints When you create the remeshing rule, you can constrain the sizing operation from specifying elements greater than or less than size constraints that you define for the remesh rule region. Abaqus/CAE provides default settings for these constraints. • The default minimum element size constraint is 1% of the default boundary seed size for the part instance to which the remeshing rule is applied. • The default maximum element size constraint is 10 times the default boundary seed size for the part instance to which the remeshing rule is applied. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Constraints: Element Size # Approximate maximum number of elements For a remeshing rule you can specify an approximate limit for the maximum number of elements. By using this constraint, you can control the cost of your analysis and ensure that unreasonably large meshes are not created. If the target error requires more elements than the specified limit when this constraint is defined, Abaqus/CAE will reduce the target error internally so that the generated elements approximately satisfy the specified element count. The use of this constraint may prevent an adaptivity process from achieving the error targets. By default, this constraint is not active. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Constraints: Approximate maximum number of elements # Refinement and coarsening rate factors The refinement and coarsening factors that you specify define a constraint on the mesh size in terms of iteration to iteration changes to the mesh. These factors modulate the aggressivity of the sizing methods. The refinement factor controls the refinement of the mesh or the introduction of smaller elements. The coarsening factor controls the coarsening of the mesh or the introduction of larger elements. Abaqus/CAE provides default settings for these rate factors, which are designed to prevent excessive coarsening or prohibitively expensive refinement in a single remesh iteration. The refinement factor can have a significant effect on the convergence of the adaptive meshing procedure. Once you have settled on sizing method parameters that work well for your application, you may be able to achieve faster and more efficient mesh convergence by increasing the refinement factor. In cases where your adaptivity process is not converging well, however, an increased refinement factor could result in an excessive increase in elements in a remesh iteration. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Constraints: Rate Limits # Reconciling overlapping remeshing rules Abaqus/CAE imposes no restrictions on the region or the steps associated with your remeshing rules. You can apply multiple remeshing rules and, hence, sizing functions to the same region at the same time. Similarly, you can specify remeshing rules that overlap one another. When Abaqus/CAE generates the new mesh, it considers all of the remeshing rules at all of the locations and uses the smallest calculated element size to drive the meshing algorithm. # 12.4 Analysis continuation after mesh replacement • “Mesh-to-mesh solution mapping,” Section 12.4.1 # 12.4.1 MESH-TO-MESH SOLUTION MAPPING Product: Abaqus/Standard # Reference • \*MAP SOLUTION # Overview Mapping a solution from one mesh to another is a step in a remeshing analysis technique, where a mesh that has deformed significantly from its original configuration is replaced by a mesh of better quality and the analysis continues. The solution mapping technique: • is used when elements become so severely distorted during an analysis that they no longer provide a good discretization of the problem; • maps the solution from an old, deformed mesh to a new mesh so that the analysis can continue; and • can be used only with continuum elements. Refer to “Adaptivity techniques,” Section 12.1.1 for a high-level discussion comparing this and other Abaqus adaptivity methods. # 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,” Section 1.1.22 of the Abaqus Example Problems Guide and “Upsetting of a cylindrical billet: quasi-static analysis with mesh-to-mesh solution mapping (Abaqus/Standard) and adaptive meshing (Abaqus/Explicit),” Section 1.3.1 of the Abaqus Example Problems Guide. # 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. $\mathrm { l n p u t ~ F i l e ~ U s a g e } ; \qquad \ast \mathrm { M A P ~ S O L U T I O N } , \mathrm { S T E P } = \ o { s t e p } , \mathrm { I N C } = \ o { i n c r e m e n t }$ # 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,” Section 34.2.1). 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” in “Output to the output database,” Section 4.1.3. 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 12.4.1–1). Table 12.4.1–1 Output database nodal output requirements for fully coupled procedures.

Procedure	Nodal output variable
“Fully coupled thermal-stress analysis,” Section 6.5.3	NT11
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1	POR
“Geostatic stress state,” Section 6.8.2	POR

# 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, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2). 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). 1. 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.) 2. 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: • “Static stress analysis,” Section 6.2.2 • “Quasi-static analysis,” Section 6.2.5 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 • “Geostatic stress state,” Section 6.8.2