MeshSim Automesh Generation Overview

StressCheck provides a general purpose automesh generation utility that may be used to automatically mesh either 2D sheet bodies or 3D solid bodies, as well as automatically refine the meshes of specific features within these bodies. The automesh generation utility utilizes the MeshSim automesher from Simmetrix, Inc. In order to generate an automesh for a sheet or solid body in StressCheck, you must perform two distinct steps:

• First, navigate to the Mesh tab in the Input dialog and create one or more active global (i.e. Auto or Extrude method) automesh generation records that contain the instructions for performing the desired automesh generation operations. For example, set the C/A/O/M to Create > Mesh > Auto, select a body or bodies, input desired automesh generation attributes, and click Accept.
• Next, click the Automesh button to execute the instructions contained in the automesh generation records. For example, if Create > Mesh > Auto was used in 3D, the resulting automesh would be midside node (quadratically mapped) tetrahedra.

Note: with the release of StressCheck v12.0, manually generated nodes (and any elements meshed from these nodes) can be used to “seed” the MeshSim automesh generator. For example, nodes placed at specific intervals along a curve will be respected when the automatic meshing routine is invoked.

A Note on Midside Node Automeshes

The automesh generation procedure introduces midside nodes into the mesh in order to control element curvature; the displacement functions controlled by p-extension are kept completely separate. StressCheck can interpret these midside nodes in two ways: the midside nodes may be used as the basis for quadratic mapping, or may be used to determine associativity with the geometric entities of the solid body to perform geometric mapping.

Geometric mapping produces a more accurate representation of the geometry than quadratic mapping, which uses a parabola to approximate all shapes. Geometric mapping is more computationally intensive than quadratic mapping since it must obtain at least 6 sample points from each edge, and 36 sample points from each surface, whereas quadratic mapping uses at most one midside node along each element edge.

After the automesh generation procedure is completed, if necessary (such as in the case of multi-body contact analysis) the mapping method used may be changed by the user by selecting the Main Menu option: Tools > Convert Element Mapping. Note: The MeshSim automesher performs all element quality tests using quadratic mapping. Therefore, it is possible that changing to geometric based mapping will cause some elements to become illegal. Always check mesh quality (Check > Mesh > Distortion) after changing the mapping method.

During automesh generation, the MeshSim automesher may move nodes small distances away from CAD geometry in order to prevent invalid elements. If this occurs StressCheck provides a warning that various nodes were moved, along with the distance each node was moved. However, if hundreds of nodes were moved for a large model the user would have to read each node distance to check for problems.

To alleviate this a single message stating the largest moved distance follows the automeshing procedure. If this distance is negligibly small (as in most cases) then the user can proceed with analysis without checking each individually moved node. These warnings may be found in the Error Log.

For more information on midside node (quadratically mapped) meshes, refer to What’s the Difference Between Quadratic and Geometric Mapping?

Automesh Generation Procedure

The automesh generation procedure consists of first deleting all existing automeshed nodes/elements (if any) from a previous automesh generation operation, followed by the new automesh generation operation. If present, manually generated nodes/elements will be preserved during the automesh generation operation and will be used to “seed” the resulting automesh. Any time a parametric change is applied to the model, if active these automesh generation records will be used to re-mesh all bodies in the model.

Note: in order to generate an automesh, there must be at least one active global (i.e. Auto or Extrude method) automesh generation record.

Automesh Generator Limitations

The limitations of the MeshSim automesh generators are as follows:

• In 3D, for the Auto method the automesher generates only 10-noded, quadratically-mapped tetrahedral elements. The mapping can be converted to geometric after the mesh is completed by selecting Convert Element Mapping from the Tools menu. Check mesh distortion after converting the mapping.
• In 2D, the automesher will produce triangular elements by default, but the mapping can be chosen to be either quadratic (Geometric: option disabled) or geometric (Geometric: option enabled, the default). As described below in the Quad-Mesh Generator section, 2D mesh can be constructed which uses quadrilateral elements (if possible) using the Create > Quad-Mesh option. In this case, only geometric mapping is supported.
• In 3D, the automesher works best on solids that do not have thin sections. Models with thin sections may cause the mesher to generate too many elements to be solved in a reasonable time by StressCheck. The number of elements that can be solved will depend on the available memory/disk space of your system.

Creating a New Automesh Generator Record

To access the MeshSim automesh generators in StressCheck, select Class > Mesh or navigate to the Mesh tab in the Input dialog. Then, set the C/A/O/M Action to Create, the Object to the desired automesh generator (Mesh, Tri-Mesh or Quad-Mesh), and the Method to one of the MeshSim Automesh Generation Methods. Then, select a sheet body, solid body, boundary or point as required by the Method, input the desired MeshSim automesh parameters, and click Accept. Once ready to generate the automatic mesh, click Automesh.

The MeshSim automesh utility is capable of automatically generating meshes of the standard element types, depending on the selected mesh generator and MeshSim Automesh Generation Methods (e.g. Auto, Extrude, Face to Face, etc.). Below are the automesh generators available in the Object combo-box, and the associated methods available for each automesh generator.

Mesh Generator

The Mesh generator is accessed by changing the C/A/O/M to Create > Mesh, and then selecting one of the below methods. Triangular (Planar), Tetrahedral (3D), or Pentahedral (3D) standard element types may be generated using the Mesh generator. Below is an animated example of MeshSim automesh generation for Create > Mesh > Auto:

The following automesh generation methods are available for Create > Mesh:

• Any Boundary
• Auto
• Boundary (Bndry.) Layer (3D only)
• Crack Edge (2D/Planar only)
• Crack Face (3D only)
• Crack Front (3D only)
• Edge to Edge
• Extrude (3D only)
• Face to Face (3D only)
• Local Size
• Match
• Simple Graded
• Thin Section

The Auto and Extrude methods are global methods. Learn more about the MeshSim Automesh Generation Methods.

Tri-Mesh Generator

The Tri-Mesh generator is accessed by changing the C/A/O/M to Create > Tri-Mesh, and then selecting one of the below methods. Triangular (Planar) or Pentahedral (3D) standard element types may be generated using the Tri-Mesh generator. Below is an animated example of MeshSim automesh generation for Create > Tri-Mesh > Extrude. Note: in this case the geometry was constant thickness, so therefore the Extrude automesh method is applicable:

The following automesh generation methods are available for Create > Tri-Mesh:

• Any Boundary
• Auto
• Boundary (Bndry.) Layer
• Crack Edge
• Extrude
• Local Size
• Simple Graded

The Auto and Extrude methods are global methods. Learn more about the MeshSim Automesh Generation Methods.

Quad-Mesh Generator

The Quad-Mesh generator is accessed by changing the C/A/O/M to Create > Quad-Mesh, and then selecting one of the below methods. Quadrilateral (Planar) or Hexahedral (3D) standard element types may be generated using the Tri-Mesh generator. Note: in some cases, if automatically generated quadrilateral/hexahedral elements are too distorted, these will be split into equivalent triangular/pentahedral elements. Below is an animated example of MeshSim automesh generation for Create > Quad-Mesh > Auto:

The following automesh generation methods are available for Create > Quad-Mesh:

• Any Boundary
• Auto
• Boundary (Bndry.) Layer
• Crack Edge
• Edge to Edge
• Extrude
• Local Size
• Simple Graded

The Auto and Extrude methods are global methods. Learn more about the MeshSim Automesh Generation Methods.

Activating/Inactivating Automesh Generation Records

An automesh generation record can be activated or inactivated. By activating an automesh generation record (“Active” toggle switch on, the default), a new automesh is generated when the Automesh button is pressed. By inactivating an automesh generation record (“Active” toggle switch off), a new automesh is not generated when the Automesh button is pressed. This feature is useful when meshing multiple bodies or surfaces, as only the “Active” automesh generation records will be used.

Note: when switching the “Active” toggle switch on/off, the Replace button must be pressed to update the automesh generation record. At least one active global automesh generation record must be present when the Automesh button is pressed.

Processing Multiple Automesh Generation Records

The user may define multiple automesh generation records for automeshing a model with one or more bodies. The following rules control the order in which automesh generation records are processed:

• Automesh generation records are processed in numerical order.
• The first automesh generation record found for each body will be used.
• Redundant automesh generation records will be ignored. For this reason each body should be referred to only once by global automesh generation records.

Checking Automesh Generation Quality

When using the automesh generators and performing the mesh distortion check (Check > Mesh > Distortion), you may find that several elements are identified as distorted (outside the range of valid vertex angles of 5 to 175 degrees) or invalid.

• Elements that are invalid require remeshing with different automesh inputs.
• Elements identified as distorted are acceptable to perform an analysis, but in some cases the stiffness matrix generation of these elements may fail as the polynomial order increases during a p-extension and/or during geometric nonlinear analyses.

Jacobian Determinant Check

During the distortion check the compliance with the vertex angles, and also that the Jacobian determinant is greater than zero in a number of interior points (27 for 10-noded tetrahedral elements), is verified. During the computation of the stiffness matrix, the number of integration (internal) points depends on the p-level for the element. If an element is too distorted, it may happen that for a given p-level (larger than 1), a negative Jacobian is found in some integration points and the stiffness matrix computation will not proceed. An error message will be issued by the program identifying the corresponding element.

If you encounter a situation like this, one possible solution is to fix the p-level of the element to the value for which the stiffness matrix was successfully computed. This should only be done in those cases where the distorted elements are outside the region of primary interest.

Replacing/Deleting Automesh Generation Records

If the user wishes to edit/replace the attributes in an existing automesh generation record, or delete an existing automesh generation record, the user first selects the automesh generation record from the scrolling listbox directly under the C/A/O/M combo-boxes. Once it is selected, the user may update the attributes and click the Replace button to update the automesh generation record, or click the Delete button to delete the automesh generation record.

Replacing an Automesh Generation Record

To edit/replace an existing automesh generation record, set the Action combo-box to Create or Edit, select the record of interest from the scrolling listbox, and then make your attribute changes. Then, click the Replace button to update the automesh generation record. Note: if only automesh generation attributes are to be replaced, set the Action to Edit. If the body is to be replaced, set the Action to Create. After clicking the Automesh button, the existing automesh will be deleted, and the MeshSim automesher will regenerate a new automesh using the updated attributes. Note: all active automesh generation records will be processed each time the Automesh button is clicked.

Deleting an Automesh Generation Record

To delete an existing automesh generation record, set the Action combo-box to Edit, select the record of interest from the scrolling listbox, and then click the Delete button. Note: deleting a global automesh generation record (Auto or Extrude method) will also delete the associated automeshes for each body referenced in the global automesh generation record. Deleting a local automesh generation record will not result in the deletion of associated automeshes.

General Automesh Improvement Strategies

Finding a combination of the four input parameters described in MeshSim Automesh Generation Methods – Ratio, D/H, MinLen and Trans – that gives the most satisfactory mesh, may require some experimentation.

Begin with the default global automesh input parameters. After generating the mesh, use the Check > Mesh > Distortion function to test the validity of the elements contained in the mesh. If all elements pass the distortion test, you may proceed to assign material properties and boundary conditions. If some elements are identified as invalid, it will be necessary to delete the current mesh by clicking the DeLast button, and try a new set of input parameters.

In general, reducing the value of any of the four input parameters will produce a finer mesh. Learn more about the four input parameters in MeshSim Automesh Generation Methods, What Do the MeshSim Global Automeshing Parameter Inputs Affect? and StressCheck Tutorial: Automeshing Tips.

Note: in previous versions of StressCheck, the “Isopar” option generated quadratically mapped elements, and the “Default” and “Legacy” toggles controlled which MeshSim version was used to generate the automesh. In StressCheck v11 and higher, 3D tetrahedral automeshes will always be quadratically mapped and StressCheck will always use the most recent MeshSim version to generate the automesh.

Guiding the Automesher

In order to “guide” the automesher to refine in certain regions, it is recommended to use imprint and Boolean-union operations to modify the geometry. By splitting surfaces and curves, the automesher will be forced to adapt the mesh.

For an example of guiding the automesher with solid modeling operations, refer to StressCheck Tutorial: Guiding the MeshSim Automesher with Imprint and Boolean-Union Operations.

Feature-Based Refinement

StressCheck makes available several options for local, feature-based (e.g. at points, curves and/or surfaces) refinement. This allows for coarser global automesh parameter inputs to be used except where local refinement is required. Learn more about feature-based refinement in MeshSim Automesh Generation Methods and StressCheck Tutorial: Feature-Based Mesh Refinement.

Note: in previous versions of StressCheck, the “Any Boundary” method and “Curve” method were analogous.

Mesh Seeding via Manually Generated Nodes/Elements

With the release of StressCheck v12.0, StressCheck supports mesh seeding strategies via manually generated nodes/elements. This allows the user to guide and compliment the MeshSim automesh generator with user-defined node locations and pre-existing, hand-meshed elements.

Node Seeding

Nodes can be placed within the model domain via a variety of node creation methods, and these nodes will be used to define element vertices during MeshSim automesh generation. For example, nodes placed at specific intervals along a curve via Create > Node > Offset will be respected when the automatic meshing routine is invoked:

Note: if only nodes are used for mesh seeding, the MeshSim automesher will create duplicate nodes in those locations. These duplicate nodes will not impact the analysis, and are necessary for proper element connectivity.

Element Seeding

A manually generated mesh of elements may be associated with the model domain, and these elements will automatically be incorporated into in the final mesh during MeshSim automesh generation. For example, a ring of hexahedral elements can be manually generated around a hole, and this ring of elements will be respected when the automatic meshing routine is invoked:

Note: the nodes used to generate these elements must be associated with the body to be automeshed. If the nodes are not associated, an error message will occur during the automatic meshing routine.

Was this article helpful?

0 out Of 5 Stars

5 Stars		0%
4 Stars		0%
3 Stars		0%
2 Stars		0%
1 Stars		0%

5 Submit

How can we improve this article?

Please submit the reason for your vote so that we can improve the article.

Submit