3.7. Generating the New Mesh

The following methods are available for generating a new mesh:

3.7.1. Generating a New Mesh via Splitting and Morphing

This method for generating a new mesh supports both 2-D and 3-D elements. Splitting occurs first for mesh refinement (although for the contact-based criterion with wearing, only morphing is needed).

In 2-D meshes, mesh morphing occurs after mesh splitting. The morphing operation can also modify elements that have not been split. The morphing process attempts to improve the element distortion metrics by optimizing the metrics immediately following splitting. If the shape metrics of specific elements cannot be improved without sacrificing the quality of the neighboring elements, then the element is not changed via morphing. The morphing process is iterative and converges when a maximum number of iterations (set automatically depending on problem size and element type) are reached or no further element shape quality enhancement is possible. Morphing works by moving the nodes in the mesh (except for the nodes on the boundary).

In 3-D tetrahedron splitting, cotangent-weighted Laplacian mesh smoothing and topology correction (by 2-3, 3-2, 2-2, and 4-4 face swaps) occur automatically after splitting. 3-D mesh refinement is more tolerant of large deformation and mesh distortion than the same 2-D process because of the additional topology-correction step. As in the 2-D case, morphing in 3-D does not change node locations on the boundary; however, topology correction may modify elements on the boundary.

When energy- and position-based criteria are used, solid elements are split directly and appropriate transitional elements are generated around a split region to ensure compatible transition with the unsplit regions. In such cases, parent elements within a component are split and the child elements are automatically made part of the component. Parent elements are dissociated from the component and removed from the simulation database during the splitting procedure. In this way, component information is automatically transferred from parent to child elements during the splitting procedure. For more information, see Geometry Details for Mesh Splitting .

Elements supporting contact-based criteria are TARGE169, TARGE170, CONTA171, CONTA172, CONTA173, and CONTA174. Mesh nonlinear adaptivity has the same restrictions for contact and target elements as for rezoning.

For contact-based criteria that use the NUMELEM criterion option (NLADAPTIVE,,,NUMELEM), the candidate solid elements for splitting are selected indirectly. Nonlinear adaptivity criteria are applied to components of target elements and the decision to split the corresponding contacts is dependent on solution-based quantities at the specific substep at which criteria checking occurs. For example, consider the following figure, showing a 2-D target-contact interface at a subset on which contact-based mesh nonlinear adaptivity criteria are checked:

Figure 3.21:  Rigid Target-Contact Interface

Rigid Target-Contact Interface

The mesh nonlinear adaptivity algorithm associates contact and target elements with each other using pinball radius values. For two components, CM1 and CM2 (where CM1 is consists of target element T1, and CM2 consists of both target elements T2 and T3), the following associations are made:

C1 C2 C3 C4 C5 C6
T1 (CM1)YYYY--
T2 (CM2)---YY-
T3 (CM2)----YY

The program’s decision to split contact elements is determined by checking the total number of contact elements associated with a single target element of a particular target component, and the user-defined number of desired contact elements (NLADAPTIVE). The following commands assign the desired number of contact elements to be 3 and 5 for individual target elements of CM1 and CM2, respectively:

nladaptive,CM1,add,contact,numelem,3
nladaptive,CM2,add,contact,numelem,5

If the total number of contact elements assigned to a target element is smaller than the user-defined desired number during a substep where mesh nonlinear adaptivity criteria are checked, splitting occurs. If the total number of contact elements is greater than the user-defined desired number, no further refinement is done.

A size check also exists for contact-based criteria that use the NUMELEM criterion option. The desired size of contact elements associated with a particular target component is calculated by dividing the size of the target element by the user-defined desired number of elements. For example, the desired size for component CM1 in the previous example is (size of T1) / 3. If the individual contact element size for elements associated with a target element during a substep where mesh nonlinear adaptivity is checked is smaller than the desired size, no more refinement is done.

The NUMELEM criterion option for contact-based mesh nonlinear adaptivity is used primary for gap filling simulation, such as a rubber seal simulations. As shown in the following figure, successive refinements of a mesh reduces the maximum gap significantly.

Figure 3.22:  Gap Reduction with Successive Mesh Refinement by Element Splitting

Gap Reduction with Successive Mesh Refinement by Element Splitting

Besides size and number requirements, the decision to split an underlying solid element at a given substep also depends on the relative penetration or gap status of the corresponding contact element with respect to a previous reference substep, as shown in the following figure:

Figure 3.23:  Contact-Status-Based Determination for Splitting

Contact-Status-Based Determination for Splitting

If the penetration increases (gap reduces), the contact element is moving toward the target, and therefore the underlying solid element is split to estimate a smaller pinball radius and improve gap reduction. In other cases, the underlying solid element is not split.

Should the splitting violate the size or number criteria, it does not occur. For a split to occur, all three criteria must be met in a substep where criteria checking occurs.

In certain cases, transitional elements can affect the size and number criteria. One such case occurs when neighboring target elements belong to different components with different size criteria defined via the NLADAPTIVE command. Consider the following simulation:

Figure 3.24:  Effect of Transitional Element Generation on Size and Numbering Criteria

Effect of Transitional Element Generation on Size and Numbering Criteria

In this case, CM1 and CM2 are the two defined components. CM1 consists of target element T1, and CM2 consists of both target elements T2 and T3. The following mesh nonlinear adaptivity commands are issued:

nladaptive,CM1,add,contact,numelem,6
nladaptive,CM2,add,contact,numelem,4

Because T2 and T3 are of a much smaller size than T1, the size allowance of contact elements scoped to CM2 is much smaller than that of CM1. In substep 1, contact elements scoped to both CM1 and CM2 are candidates for refinement. In substep 2, however, only contact elements scoped to CM2 are candidates, while contact elements scoped to CM1 are not refined. Because transitional elements are generated for compatibility, some contact elements scoped to CM1 may be refined as an indirect consequence of refinements to the CM2 contacts. The program allows a small tolerance for the size criteria so that transition regions do not become over-refined during splitting.

3.7.2. Generating a New Mesh via General Remeshing

For the mesh-quality-based criterion (NLADAPTIVE,,,MESH), general remeshing is applied to repair the mesh quality. The regions to remesh are initialized by seed elements. For 3-D models, seed elements have a skewness >= a specified threshold (NLADAPTIVE,,,MESH,SKEWNESS). For 2-D models, seed elements have a shape metric of maximum corner angle >= a specified threshold (NLADAPTIVE,,,MESH,SHAPE).

When the mesh-quality-based criterion threshold is reached at a particular substep of a load step during a nonlinear adaptive solution, the program creates a source mesh (based on the deformed mesh) for use by the remesher. The source mesh contains the seed elements, with additional elements included based on the specified number of sculpting layers. Using the source mesh, the remesher attempts to generate a new mesh, or target mesh, of better quality. If the target mesh is better than the source mesh, the solution continues using the new mesh.

Depending on the seed elements and sculpting layers, it is possible that the remeshing domains cover the whole mesh or some partial mesh of the source model.

The following topics related to general remeshing are available:

3.7.2.1. Understanding Remeshing Regions and Domains

A nonlinear adaptivity (NLAD) region is a group of elements which you can select or assign from geometry parts or bodies.

A remeshing region is a group of elements from the source mesh, where the elements have unique material- and element-component properties. The remeshing region is the atomic 2-D or 3-D remeshing volume in the remeshing process; the interface surfaces between regions are enforced to a conformal mesh.

An element in a remeshing region may belong to multiple NLAD regions, as shown in this figure:

Figure 3.25:  NLAD Regions and Remeshing Regions

NLAD Regions and Remeshing Regions

Remeshing regions are driven by your defined NLAD regions. Understanding the relationship between NLAD regions and remesh regions is useful when modeling workarounds for self-contact penetration in 3-D models.

A remeshing domain is a grouping of elements, each connected by at least one element face in a 3-D model, or by at least one element edge in a 2-D model.

For a 3-D model, no face connection exists between domains, but node or edge connections can exist. For a 2-D model, no edge connection exists between domains, but node connections can exist.

A domain can contain multiple regions, composed of a grouping of elements, each connected by at least an element face but having unique material- and element-component properties.

The following figure shows a 3-D model composed of six parts, naturally decomposed to six domains:

Figure 3.26:  Understanding 3-D Domains

Understanding 3-D Domains

The two cubes in the figure have edge connections only, so they decompose into two domains for remeshing because they have no face connection.

The following figure is a 2-D model composed of four domains, where interfaces between the domains can be in contact, but no mesh connections (no conforming meshes) exist. Part 4 (P4) is composed of 4 regions (P4R1 through P4R4).

Figure 3.27:  Understanding 2-D Domains

Understanding 2-D Domains

Remeshing domains are logical 2-D/3-D geometries composed of parts to remesh, whereas remeshing regions are the effective and specific 2-D/3-D geometry parts to remesh. The program maintains the interfaces between regions so that the source mesh material and element components are maintained.

Partial model remeshing is an option for minimizing the solution time. The meshing algorithm ensures a conformal mesh between the remeshed regions and untouched regions.

Figure 3.28: Understanding 3-D Regions shows one 3-D domain consisting of three regions, and Figure 3.29: Understanding 2-D Regions shows one 2-D domain consisting of four regions:

Figure 3.28:  Understanding 3-D Regions

Understanding 3-D Regions

Figure 3.29:  Understanding 2-D Regions

Understanding 2-D Regions

The program detects remeshing regions and domains according to the seed elements and the specified number of sculpting layers. The elements to be remeshed will thus have the same element and material properties as the seed elements. Depending on these seed elements and the specified number of sculpting layers, it is possible that the remeshing domains cover the whole mesh or some partial mesh of the deformed model during solution.

Partial model remeshing is an option for minimizing the solution time. The meshing algorithm ensures a conformal mesh between the remeshed regions and untouched regions.

3.7.2.2. Optional Remeshing Controls

If desired, more granular control of the source mesh geometry is available via the NLMESH command. The command's remeshing controls are global and apply to every remeshing throughout a load step of the nonlinear analysis. For even more control of the remeshings within a load step, you can perform a restart analysis by modifying the remeshing controls.

3.7.2.2.1. Boundary-Angle and Edge-Angle Control

User-specified boundary-angle and edge-angle thresholds are available (NLMESH,BDRA and NLMESH,AEDG, respectively).

The program detects the most appropriate mesh segmentations and remeshes specific 2-D or 3-D mesh entities using a systematic bottom-up approach. Conformal mesh interfaces between regions are guaranteed, and new nodes on exterior surface are guaranteed to be located on the exterior facets of the source mesh.

The boundary angle (NLMESH,BDRA) is the outer normal vector angle from two adjacent facets, where a facet is an element face (3-D) or an element edge (2-D).

Figure 3.30:  3-D Boundary Angle Between Two Adjacent Faces on an Exterior Surface

3-D Boundary Angle Between Two Adjacent Faces on an Exterior Surface

Figure 3.31:  2-D Boundary Angle Between Two Adjacent Edges on an Exterior Surface

2-D Boundary Angle Between Two Adjacent Edges on an Exterior Surface

For 3-D models, the edge angle (NLMESH,AEDG) is the outer normal vector angle from two adjacent boundary edges in a 3-D patch.

Consider the following example 3-D model:

Figure 3.32:  3-D Edge Angle in a Segment

3-D Edge Angle in a Segment

When the specified threshold value for the edge angle (NLMESH,AEDG) exceeds 25 degrees, the remesher has more freedom to remesh. In this case, the highlighted feature may be lost after remeshing, as it is no longer necessary for the node to be retained based on your input. The same applies to boundary angles (NLMESH,BDRA). Too large a value (typically > 40) can result in a loss of certain features that you had expected to retain after remeshing, and may affect solution convergence adversely.

3.7.2.2.2. Sculpting Layers Control

Use sculpting layers to detect remeshing regions starting from detected seed elements. Specifying a larger number of layers results in relatively large regions containing more elements and causes segregated regions to be merged. If the specified number of layers is large enough, the entire domain is remeshed if it has at least a seed element detected. Using this control helps to avoid many tiny cavities in the remeshing regions.

The following figure shows the relationship between the remeshing region, the seed elements, and the specified number of sculpting layers:

Figure 3.33:  Partial Remesh: Sculpting Remesh Regions

Partial Remesh: Sculpting Remesh Regions

A generic approach to partial remeshing begins with one or two seed elements (usually highly distorted elements). When layer = 0, the remeshing region is composed of seed elements only. By increasing the number of sculpting layers (NLMESH,NLAY), the remeshing region becomes larger until it applies to the entire model. The FEA meshing engine remeshes the regions and guarantees a mesh interface conforming to untouched regions.

Partial remeshing enables:

  • Remeshing as needed on the fly (that is, remeshing regions as necessary to reduce the solver’s computational overhead, and to reduce accuracy loss caused by mesh modifications).

  • Adaptively changing local mesh sizing in different time phases of the simulation workflow.

3.7.2.2.3. Global Sizing Control

During remeshing, the average mesh size of the source model is detected and then applied to the target mesh by default; as such, the target mesh has a uniform size by default without change in average mesh density. The entire mesh nonlinear adaptivity process benefits, as it is unnecessary to add a significant number of elements (requiring, in turn, more computational resources). It is possible, however, to specify a global refining/coarsening factor (NLMESH,SRAT) to adjust mesh density in each remeshing .

The program writes the average and worst element mesh-quality metrics to the log file, where remeshing statistical data are available to help you make additional adjustments to the remeshing control parameters.

The following figure illustrates the global sizing factor:

Figure 3.34:  Global Sizing

Global Sizing

A factor >1 coarsens the model source mesh, and <1 refines the source mesh.

The factor is the ratio of the average target mesh length over the average source mesh length. A specified value of 0.5 refines the mesh and results in 8x the number of elements in the target mesh as compared to the source mesh for 3-D. In actual usage, the final element number is also affected by remesh constraints such as specified boundary or edge angles, number of element or material components, contact elements, boundary conditions or loads, and other factors.

Because the specified global sizing factor that you specify applies to all remeshings of a nonlinear analysis within a load step, a small value (< 0.7) may eventually lead to an unnecessarily refined mesh towards the end of the solution (depending on the initial 2-D/3-D model, the number of triggered remeshings, and the physics of the nonlinear deformation during solution). To avoid unreasonable solve times, therefore, carefully choose what value you specify for global sizing.

Typically, there is no need to coarsen the mesh during the analysis; however, if you wish to do so, specify a value between 1 and 1.3. (A value > 1.3 can corrupt the target model due to excessive coarsening and may cause errors during or after remeshing.)

3.7.2.2.4. Gradient Control

Both 2-D and 3-D remeshing offer local sizing and gradient control.

Options are available for 2-D and 3-D remeshing to retain the size gradient from the source mesh (NLMESH,GRAD):

VAL1 = 0 does not maintain the mesh-size gradient but generates a uniform mesh in the remeshing regions.
VAL1 = 1 generates a new mesh and retains the same local size as the source mesh.
VAL1 = 2 generates a new mesh and retains the same local size as the source mesh, but with additional sizing compensation based on the element-size change during solution due to large-deformation effects.

Considerations for specifying 2-D / 3-D size gradient control:

Specify VAL1 = 0 with initial meshes which are not graded and have uniform sizing throughout the nonlinear adaptivity remeshing component. This value induces slight coarsening effects during large deformation. Therefore, using this option with global sizing control to slightly refine the mesh for every remeshing gives better results.
Specify VAL1 = 1 when VAL1 = 2 cannot achieve better convergence for initial meshes that are graded. In such cases, slight coarsening effects may be observed for high-deformation regions, and global sizing control may be necessary. Avoid this option for uniform initial meshes.
VAL1 = 2 (default) is the recommended value for all initial meshes that are graded. This value induces slight refinements within the vicinity of the area having large distorted elements. Typically, global sizing control is unnecessary.

2-D Mesh-Size Gradient-Control Options:

 

 

3-D Mesh-Size Gradient-Control Options:

 

 

 

 

3.7.2.2.5. Understanding the Remesh Log

Each remeshing operation generates a corresponding remeshing log in the solver output. The log contains the input and output statistics for that remeshing. The statistical data can help you to make any additional adjustments (if needed) to the remeshing controls (NLMESH).

Figure 3.35:  Example FEA Remesh Log File (2-D)

Example FEA Remesh Log File (2-D)

Figure 3.36:  Example FEA Remesh Log File (3-D)

Example FEA Remesh Log File (3-D)

The Source and Target columns contain the corresponding data before and after remeshing. For example, in the 3-D remesh log, the worst element quality is shown based on element volume skewness and element aspect ratio; the worst element IDs for the corresponding mesh quality metric appear in parentheses (for example, e6497 indicates that the element ID is 6497). Skewness(Vol) is the element volume skewness, ranging between 0 (perfect element) and 1 (highly distorted element). The Aspect Ratio ranges from 1 (perfect element) to infinity (highly distorted element).

Skewness (Volume) is the element volume skewness, ranging between 0 (perfect element) and 1 (highly distorted element). The Aspect Ratio ranges from 1 (perfect element) to infinite (highly distorted element).

The Remeshing result statistics section summarizes the remeshing domain/ or region decomposition data, as follows:

nNode[New] -- New nodes generated in all remeshed regions
nElem[New] -- New elements generated in all remeshed regions
nElem[Eff] -- Effective source elements that are now remeshed (that is, deleted and replaced)
nElem[Src] -- Number of elements available to remesh from the source mesh

A partial remesh is indicated by nElem[Eff] < nElem[Src]. A whole-model remesh is indicated by nElem[Eff] = nElem[Src].

The remesh log also shows the peak memory used and the elapsed time for the remeshing process.

3.7.2.2.6. Known Remeshing Limitations

Remeshing typically fails when either of the following conditions exist:

3.7.2.2.6.1. Non-manifold Mesh Geometry

Arbitrary element selection in the remeshing region and partial remeshing with a decomposed element group may create non-manifold FEA geometry, especially for 3-D cases where in each atomic region a non-manifold edge or node may exist.

Figure 3.37:  3-D Non-manifold Edge

3-D Non-manifold Edge

The following figure shows a 3-D non-manifold node with two connected exterior faces:

Figure 3.38:  3-D Non-manifold Node

3-D Non-manifold Node

Figure 3.39:  2-D Non-manifold Node

2-D Non-manifold Node

Dealing with Non-manifold Mesh Geometry

The remesher handles 3-D non-manifold geometry cases and simple cases of 2-D non-manifold geometry automatically.

Try the following approaches if 2-D non-manifold remeshing issues persist:

  • Modify any of the remeshing control options (NLMESH). This approach modifies remeshing regions and may help to remove the non-manifold geometry or reduce the complexity in source meshes.

  • Remesh the entire nonlinear adaptivity model, body, or part (rather than just a portion of the model, body, or part)

  • Redefine material or element components (insofar as possible)

3.7.2.2.6.2. Region Self-Contact Penetration

Self-contact penetration means that volume intersections exist in an atomic remeshing region.

For 2-D remeshing, the program handles self-contact automatically.

Figure 3.40:  2-D Self-Contact

2-D Self-Contact

3-D remeshing failure occurs if this conditions exists at any time during the nonlinear adaptivity simulation process. To prevent self-contact penetration, split the original NLAD region (a) into multiple regions (b), as shown in this figure:

Figure 3.41:  Workaround for 3-D Self-Contact Penetration

Workaround for 3-D Self-Contact Penetration

3.7.2.2.7. Dealing with Remeshing Failure

Remeshing failure at a given substep may occur in some nonlinear adaptivity problems, most often because the mesh metrics of the worst element in the target mesh are worse than those of the worst element in the source mesh.

In nonlinear FEA, even a single target element of poor quality in a critical region can cause the solution to diverge. To ensure that convergence is not adversely affected in such cases, the program continues solving using the old mesh and rejects the target mesh, as indicated in the output file at the remeshing substep:

Although the program automates the solution process in the event of remeshing failure and lends it some degree of fault tolerance, it is not an ideal situation. If many remeshing attempts in a nonlinear solution process are rejected, the solution may diverge, especially when additional loads make the mesh quality worse as the solution progresses. In such cases, a restart may be required with more relaxed shape and/or skewness options (NLADAPTIVE,,,,SHAPE or SKEWNESS, respectively). To a lesser extent, using the remeshing controls (NLMESH) to increase the number of sculpting layers, for example, may also help to achieve successful remeshings after restart.

FEA automatic local remeshing is a complex operation. There may be several reasons why a remeshing failure may be triggered. Two categories of remeshing failure exist:

3.7.2.2.7.1. Direct Remeshing Failure

Direct remeshing failures include cases where the remesher fails to generate a new target mesh based on the source mesh, indicated by errors in the remeshing log in the solver output. The errors can be caused by:

  • Unacceptable source mesh due to initial model setup

    This situation occurs rarely, but is possible when any of the following conditions exist:

    • Inconsistent element node orientations

    • Invalid element-node ID references

    • Invalid component-element ID references

  • Complicated non-manifold FEA geometry

    Due to the generic nature of the FEA local remeshing approach, non-manifold FEA geometry in remeshing regions may occur often. The remesher can handle non-manifold FEA geometry, but may have difficulty in exceptional cases where the source mesh has overly complicated non-manifold geometry, especially in 3-D models.

3.7.2.2.7.2. Your Expectation of Target Mesh Quality Is Not Met

You may deem a given remeshing to be a failure because target mesh quality does not meet your expectations. In this case, consider the following:

  • The quality of the source mesh at the remeshing substep may already be of sufficient quality.

    In this case, perhaps no remeshing is required after all.

  • Your remeshing requirements (specified via the mesh criterion options) may be too strict.

    For most 2-D models, try defining a maximum corner angle threshold of 155 to 175. For most 3-D models, try defining a skewness threshold of 0.87 to 0.97. These recommendations assume that you check the mesh quality at every substep during the solution.

  • The program may not be capable of generating a better quality mesh.

    Various factors may constrain the remesher's ability to generate a better quality mesh: many material or element components in the source mesh, tiny remeshing regions, boundary conditions or loads in the remeshing regions, or contact elements in the remeshing regions. One or more of these constraints may adversely affect the quality of the new mesh, even though they may be required by the physics in the model. In this case, try increasing the number of sculpting layers for remeshing (NLMESH).

  • More mesh-control refinement may be necessary.

    In some cases, the target mesh quality may not improve even when using recommended thresholds for the mesh criterion options. In such cases, try modifying other remeshing control parameters (NLMESH) to obtain a better mesh. For example, if a coarse mesh suddenly starts to fill a narrow gap with high element distortion, try to control the element sizing and achieve local remeshing control by specifying fewer sculpting layers for remeshing, eventually improving mesh quality.


Release 18.2 - © ANSYS, Inc. All rights reserved.