MeshSim Automesh Generation Methods in StressCheck

There are several different types of automesh generation records that may be created, each with a corresponding automesh method. These methods may be divided into two groups: global (body-based) and local (feature-based) methods. The attributes associated with each method are described below.

Note: if an input value for an attribute is not provided (check box next to the input field is turned off), the automesher will perform according to its own internal default rules for that attribute. A newer release may produce a different mesh for the same case, than was produced by an earlier release. Consequently, the meshes that you obtain may be different from the examples shown in the documentation.

Global (Body-Based) Automesh Methods

The Auto or Extrude methods are used to generate a global automesh for one or more bodies. Only one global automesh generation record should be provided for each distinct body. However, multiple bodies may be included in a single global automesh generation record.

Note that in order to produce a mesh, a model must contain at least one active Auto or Extrude mesh record.

For additional information and tips on global automeshing, refer to What Do the MeshSim Global Automeshing Parameter Inputs Affect? and StressCheck Tutorial: Automeshing Tips.

Auto Method

Attributes that control the automesher everywhere in the domain where local meshing attributes are not provided. This mesh generation record may be used for either solid or sheet bodies. Select the solid or sheet bodies, supply the attribute input values, then click Accept to save the automesh generation record. Click Automesh to launch the automesh process for any active records. The attribute input values are:

Ratio

The user may specify the ratio of the length of the largest edge relative to the length of the smallest coordinate aligned bounding box which surrounds the part (Figure 1). Default value is 0.75. Valid range value: 0.01 to 1.0.

Note: the Ratio attribute is useful to control the aspect ratios of elements in flat, unfeatured regions of a body.

Curvature D/H

The user may specify the ratio of the distance from the chord formed by an element edge and its associated curve (D) or surface, relative to the length of the element edge (H, as shown in Figure 2). Default value is 0.114. Valid range value: 0.005 to 0.4.

Note: the Curvature D/H attribute is useful for controlling the refinement of elements in curved regions, such as holes, blends and fillets. If the check box is disabled, the mesher will not check the D/H ratio of the elements it produces. If the check box is enabled, the ratio is tested and the elements produced will satisfy the limit supplied. In addition, when the D/H checkbox is enabled, the automesher will utilize additional rules that take into consideration the individual characteristics of geometric surfaces found in the model. For example, the mesher will attempt to mesh a cylindrical surface with fewer elements in the length direction than in the circumferential direction.

Curvature Min. Length

The minimum length of any element edge in curved regions of the mesh (in model units). Default value is 0.015. Valid range value: 0.001 to 0.4.

Note: the Curvature Min. Length attribute is useful for providing a lower bound for element sizes when simultaneously decreasing D/H. This ensures the model is not overly refined in curved regions. Also note that the global record value will be enforced on local automesh records (with the exception of Any Boundary where the Curvature Min. Length can be defined).

Geometric (Planar Reference Only)

If the check box is on (default), geometrically mapped elements will be generated. If the check box is off, quadratically mapped (midside node) elements will be generated. For more information on quadratic vs geometric mapping, refer to What’s the Difference Between Quadratic and Geometric Mapping? and Why Is There a Recommended Maximum P-level for Quadratically Mapped Automeshes?

Note: in 3D, quadratically mapped (midside node) elements will always be generated. If required for the analysis, after mesh generation the mapping may be converted to geometric mapping by using Tools > Convert Element Mapping. In the case of multi-body contact models, the element mapping will be automatically converted to geometric in active contact zones upon solving.

Transition Rate

Rate of transition from small elements in a local region to larger elements in a global region. Default value is 0.05. Valid range value: 0 to 1.

A value of zero (0.0, the default) indicates that elements will remain small in both the local and global region. A value of one (1.0) indicates that elements will transition rapidly from a small size in the local region to a larger size in the global region. A value in between will indicate a more gradual transition between local and global mesh regions.

Note: the Transition Rate attribute is useful for increasing/decreasing element counts throughout the body, while leaving curved features relatively refined.

Suppress Small Features Toggle

Suppresses small features with absolute size of specified value. Otherwise, uses relative size of 0.00005. Note: this toggle replaces the _ms_suppress reserved parameter in StressCheck v10.5 and earlier. A warning will appear when opening a model which has _ms_suppress defined indicating that this parameter has been deprecated.

For more information on this feature, refer to How Do I Troubleshoot Small-Feature Automeshes?

Suppress Slivers Toggle

Maximum aspect ratio of sliver faces to suppress. Defaults to no removal. Otherwise, value is minimum angle in degrees, with min allowable value of 5 degrees. Note: this toggle replaces the _ms_slivers reserved parameter in StressCheck v10.5 and earlier. A warning will appear when opening a model which has _ms_slivers defined indicating that this parameter has been deprecated.

For more information on this feature, refer to How Do I Troubleshoot Small-Feature Automeshes?

Assembly Meshing Toggle

Available in StressCheck v12.0 and newer, if the Assembly Meshing toggle is enabled then StressCheck will attempt to match meshes locally and automatically generate multi-body contact constraints based on a user-defined boundary proximity tolerance. Assembly Meshing is disabled by default.

For more details on the workflow, refer to the Multi-Body Contact Analysis section “Automatic Contact Setup”.

Angle (StressCheck v10.5 and older)

Smallest vertex angle allowed for any element. The vertex angle is determined by computing the smallest angle between two edges converging to the node. In 3D there are three edges per node, therefore three angles are computed and the smallest is the vertex angle. Default value: 5.0

Below is an animated example of MeshSim automesh generation for Create > Mesh > Auto using the default attributes:

Extrude Method

An extrusion mesh is only applicable when the front face of the solid domain is identical with the back face. In this case, it is possible to instruct the automesher to first generate a mesh of planar (2D) elements on the front face, and then extrude these elements through the depth direction of the body to form solid elements. Select the front faces, select the back faces in the same order that the corresponding front faces were selected, supply the input values, then click Accept to save the record. Click Automesh to process the record, and any other active records. Note the Extrude Method is a global assignment so it cannot be used in combination with Auto. The attribute input values are:

Ratio

The user may specify the ratio of the length of the largest edge relative to the length of the smallest coordinate aligned bounding box which surrounds the part. Default value is 0.1. Valid range value: 0.01 to 1.0.

Note: the Ratio attribute is useful to control the aspect ratios of elements in flat, unfeatured regions of a body.

Curvature D/H

The user may specify the ratio of the distance from the chord formed by an element edge and its associated curve (D) or surface, relative to the length of the element edge (H). Default value is 0.114. Valid range value: 0.005 to 0.4.

Note: the Curvature D/H attribute is useful for controlling the refinement of elements in curved regions, such as holes, blends and fillets. If the check box is disabled, the mesher will not check the D/H ratio of the elements it produces. If the check box is enabled, the ratio is tested and the elements produced will satisfy the limit supplied. In addition, when the D/H checkbox is enabled, the automesher will utilize additional rules that take into consideration the individual characteristics of geometric surfaces found in the model. For example, the mesher will attempt to mesh a cylindrical surface with fewer elements in the length direction than in the circumferential direction.

Curvature Min. Length

The minimum length of any element edge in curved regions of the mesh (in model units). Default value is 0.05. Valid range value: 0.001 to 0.4.

Note: the Curvature Min. Length attribute is useful for providing a lower bound for element sizes when simultaneously decreasing D/H. This ensures the model is not overly refined in curved regions.

Transition Rate

Rate of transition from small elements in a local region to larger elements in a global region. Default value is 0.05. Valid range value: 0 to 1.

A value of zero (0.0, the default) indicates that elements will remain small in both the local and global region. A value of one (1.0) indicates that elements will transition rapidly from a small size in the local region to a larger size in the global region. A value in between will indicate a more gradual transition between local and global mesh regions.

Note: the Transition Rate attribute is useful for increasing/decreasing element counts throughout the body, while leaving curved features relatively refined.

Mirror

If this check box is on, the extruded mesh will be mirrored about the center of the domain.

Layers

The total number of layers in the extruded mesh (including mirrored layers if any). Default value is 2.0.

First Layer Depth

Thickness of the first layer of elements measured from the front face. Layer thickness grows geometrically. Default value is 0.05.

Angle (StressCheck v10.5 and older)

Smallest vertex angle allowed for any element. The vertex angle is determined by computing the smallest angle between two edges converging to the node. In 3D there are three edges per node, therefore three angles are computed and the smallest is the vertex angle. Default value: 5.0

Below is an animated example of MeshSim automesh generation for Create > Mesh > Extrude using Ratio:0.05, Curvature D/H:0.1, Curvature Min. Length:0.001, Transition Rate:0, Layers:1 and First Layer Depth:1. Note: in this case the geometry was constant thickness, and the number of front faces was equal to the number of back faces, so therefore the Extrude automesh method is applicable:

Local (Feature-Based) Automesh Methods

The Boundary Layer, Any Boundary or Local Size methods may be used to refine one or more user-specified features (i.e. points, curves or surfaces) within a body or bodies. For general tips on local automeshing, refer to StressCheck Tutorial: Feature-Based Mesh Refinement and What is the Size Input for Local Automeshing?.

Boundary Layer Method

A boundary layer mesh record describes a local mesh refinement region around one or more selected boundaries (curve/surface) of a solid body. The boundary layers will be constructed in a geometric progression, based on the ratio of the thickness of the first layer (To) relative to the total thickness of the refinement region (T-Total). Given the thickness of the i^th layer to be ‘t_i’, the total thickness of the refinement region to be ‘T’, and the number of layers to be ‘n’, the following relation holds for geometric growth:

t_i+1 = r*t_i and T-Total = To + To*r + To*r² + To*r³ + … + To*r^n-1 = To*(rⁿ-1)/(r-1)

The automesher calculates the growth factor ‘r’ from the input values. Isotropic layer heights (r=1) can be generated by setting the total height equal to the number of layers times the first layer height, T-Total = n*To. Select the curves and/or surfaces, supply the input values, then click Accept to save the record. Click Automesh to process the record, and any other active records. The input values are:

Ratio

The ratio of the length of the longest attached element edge to the characteristic length of the geometric curve or surface. Default value is 0.05. Valid range value: 0.01 to 1.0.

Layers

Number of layers of elements generated radially from/normal to the selected curve/surface. Default value is 2.0.

Inner Thickness (To)

Thickness of the first layer of elements attached to the selected curve/surface. Default value is 0.0225.

Total Thickness (T-Total)

Total thickness of the element layers as measured radially from/normal to the selected curve/surface. Default value is 0.045.

Side

For surface boundary layers only. If “Negative Normal” is selected, the mesh refinement will be generated on the side of the face corresponding to its negative normal. If “Positive Normal” is selected, the refinement will be generated on the side of the face corresponding to its positive normal. If “Both Sides” is selected, the refinement will be generated on both sides of the face. Default is Both Sides.

Note: if not known in advance, the positive surface normal can be determined by navigating to the Geometry tab, setting the A/O/M to Check > Any Surface > Offset, and hovering the mouse cursor over the desired surface. A green arrow will indicate the positive surface normal.

Mixed Mesh Toggle

Controls whether the boundary layer mesh will be constructed of only tetrahedrons (off) or a mix of pentahedrons & hexahedrons (on). On by default. If the boundary layer is applied to a surface, the mesher will attempt to produce a quad-dominant mesh on the selected surface in order to produce a mostly hexahedral boundary layer mesh. If applied, to a curve, the innermost layer of elements will be all pentahedrons, with hexahedrons in the outer layers.

Shrink to Fit Toggle

Controls whether boundary layers will be trimmed or shrunk to avoid intersections. Off by default. When on, the number of layers will be maintained throughout the boundary layer mesh, but the layer thicknesses will be adjusted to avoid nearby geometry or self-intersections.

Below is an animated example of MeshSim automesh generation for Create > Mesh > Boundary Layer. A cylindrical hole surface is selected, and it can be observed that only the mesh around the selected surface is refined with radial boundary layers for Ratio: 0.3, Layers: 3, Inner Thickness: 0.1, Total Thickness: 0.5, Mixed Mesh on and Shrink to Fit off:

For a demonstration of this feature, refer to StressCheck Tutorial: Mixed (Hexa/Penta) Boundary Layer Automesh Refinement.

Any Boundary Method

Identify a boundary (curve/surface) of a sheet or solid body where you wish to control the local meshing attributes. Elements will be associatively attached to the selected boundary. The attributes assigned to the boundary will override the global meshing attributes only for this boundary. Select the boundary or boundaries, supply the inputs, and click Accept to save the record. Click Automesh to process the record, and any other active records. The input values are:

Ratio

The ratio of the longest element edge to the characteristic length of the selected boundary. Default value is 0.1. Valid range value: 0.01 to 1.0.

Curvature D/H

The user may specify the ratio of the distance from the chord formed by an element edge and its associated curve (D) or surface, relative to the length of the element edge (H). Default value is 0.057. Valid range value: 0.005 to 0.4.

If the check box is disabled, the mesher will not check the D/H ratio of the elements it produces. If the check box is enabled, the ratio is tested and the elements produced will satisfy the limit supplied. In addition, when the D/H checkbox is enabled, the automesher will utilize additional rules that take into consideration the individual characteristics of geometric surfaces found in the model. For example, the mesher will attempt to mesh a cylindrical surface with fewer elements in the length direction than in the circumferential direction.

Curvature Min. Length

The minimum length of any curved element edge in selected boundary (in model units). Default value is 0.015. Valid range value: 0.001 to 0.4.

Below is an animated example of MeshSim automesh generation for Create > Mesh > Any Boundary. Two curves in a blend are selected, and it can be observed that only the mesh around the selected curves is refined for Ratio: 0.1 and D/H: 0.1:

Note: in previous releases, this method was labeled “Curve”.

Remark: for cases in which the selected boundary size in an Any Boundary automesh record is much smaller than the overall mesh size, the “Curvature Min. Length” field should be enabled in the Any Boundary record and provided a suitable input value. Otherwise, MeshSim will use the Global automesh record’s “Curvature Min. Length” input value (or if disabled, its default value of 0.015), which is proportional to the full mesh size and may be too coarse for the Any Boundary record to overcome.

Local Size Method

Identify a point, system or boundary (curve/surface) of a sheet or solid body where mesh refinement is desired. Select the point, system and/or boundaries, supply the input value, and click Accept to save the record. Click Automesh to process the record, and any other active records. Note: selected points/systems do not need to be associative, but must lie within the domain of the body. The input value is:

Size

The length of the element edges in the neighborhood of the selected object(s). Default value is 0.1. Note: for selected points/systems, the length of element edges near the points/systems will respect the Size input only if smaller Transition rate values (e.g. 0.05) are used.

Below is an animated example of MeshSim automesh generation for Create > Mesh > Local Size. Several points are selected, and it can be observed that only the mesh around the selected points is refined for Size:0.1:

Note: in previous releases, this method was labeled “Local”.

Thin Section Method

Creates a structured mesh of several layers through a Thin Section specified by source and destination faces (similar to the Extrude method). Left click to select source faces (hold Shift to select multiple) and hold Ctrl+Shift to select destination faces (use Ctrl to deselect either). Unlike the Extrude method, there does not need to be a 1 to 1 correspondence between source and destination faces. This feature is useful when meshing areas that would otherwise produce very high aspect ratio tetrahedrons that may negatively impact solution quality and computational time.

The Thin Section mesh is specified on a region of bounded surfaces, so only 1 Thin Section record per region is permitted. If a region has multiple thin areas, simply include all necessary surfaces in your selection of sources and destinations in a single record. If multiple records are present on a single region, they will be processed as a single record using the input parameters from the first record only.

In cases where multiple Thin Section meshes are adjacent and are not simply stacked, the Thin Section records must be specified in the correct order to avoid conflicting mesh projections. Below is an example of a case where the records must be created in a specific order or the mesher will fail (Figure 3):

Note, also, that multiple adjacent Thin Section records may share source faces but may not share destination faces and that adjacent Thin Section meshes may not form a cyclical loop.

Layers

Specify the number of layers between the source and destination. Toggle off to use default of 1. Maximum 10 layers. Off by default.

Thin Section Distance

Specify the maximum distance to be considered “thin” between source and destination faces for regions that are partially thin. Toggle off or enter 0 to instruct the mesher to consider the entire region for Thin Section meshing. If a nonzero value is entered, the structured mesh will only be constructed in areas between the sources and destinations that are closer than the specified distance. Off by default.

Note: In general it is recommended to enter a Thin Section Distance instead of toggling it off or set to zero, and set it to a value slightly larger than the distance between surfaces.

Pentahedron/Hexahedron Toggle

Controls whether the Thin Section mesh will be constructed of all pentahedrons or mostly hexahedrons. Note: Some cases with complex surface geometry may fail to mesh with the hexahedron option but succeed with pentahedrons.

The below animation provides an example of a Thin Section mesh across the web of a rib section (3 surfaces picked on one side, 1 surface on the other side) with Layers:2, Thin Section Distance off, and Hexahedron on:

For a demonstration of this feature, refer to StressCheck Tutorial: Automeshing Thin Regions with Pentas and Hexas via the Thin Section Method.

Crack Automesh Methods

The Crack Edge (Planar), Crack Face (3D) and Crack Front (3D) methods may be used to represent a crack profile for fracture mechanics applications. The crack profile is generated by “unzipping” the nodes along edges (Planar) or edges/faces (3D).

Crack Edge Method

Identify a curve of a 2D sheet body that will be treated as a thru-crack. After a mesh is automatically generated, the element connectivity on one side of the crack will be modified to produce a crack in the domain. Select the curve representing the crack path and click Accept to save the record. Then, click on the Automesh button to process the record, and any other active records.

Note: perform a Check > Edge > Free Edge to verify the crack edge automesh. The free edges will be shown in red highlight.

Note: the Crack Edge method may be combined with other local refinement techniques in order to further refine the mesh and the crack tip.

Below is an animated example of MeshSim automesh generation for Create > Mesh > Crack Edge. The spline curve representing the thru-crack is selected, and after the automesh is generated a Check > Edge > Free Edge is invoked:

Crack Face Method

Identify an internal/embedded surface within a 3D solid body that will be treated as a part-thru or thru-crack. After the mesh is automatically generated, the element connectivity on one side of the crack surface will be modified to produce a crack in the domain. Select the surface representing the crack, and then click Accept to save the record. Then, click on the Automesh button to process the record, and any other active records.

Note: enable Mesh Transparency to verify the crack face automesh. Boundary Layer automesh generation records are frequently combined with Crack Face automesh records in order to reduce discretization error as much as possible for fracture mechanics extractions (typical approach used prior the implementation of the Crack Front method). For tips on crack face automeshing, refer to Fracture Mechanics Meshing Strategies, Helpful Hints and Tips: Elliptical Crack Automeshing Guidelines and StressCheck Demo: Part-Thru Crack SIFs for Stiffened Lug.

Below is an animated example of MeshSim automesh generation for Create > Mesh > Crack Face. To produce an automesh suitable for fracture mechanics parameter extraction, the Crack Face automesh record of the quarter ellipse surface was combined with a Boundary Layer automesh record at the crack front bounding curve of Ratio:0.1, Layers:2, Inner Thickness:0.005, Total Thickness:0.01, and Mixed Mesh/Shrink to Fit on:

Crack Front Method

This is a specialized method to be used for 3D Fracture Mechanics models.

Select the bounding curve (or curves) representing the crack front (in the case of a crack modeled on a symmetry plane, also hold Ctrl+Shift and select the crack face), and then click Accept to save the record. Then, click on the Automesh button to process the record, and any other active records. Note: if multiple bounding curves are selected, only the first selected curve will influence the mesh density along the crack front mesh.

Once the mesh is automatically generated, the mesh on the crack surface will be modified to produce a crack in the domain (splitting the mesh). In addition a Boundary Layer refinement will also be incorporated around the crack front bounding curve to ensure high quality fracture mechanics parameter extractions. The refinement options are “Automatic Values”, in which StressCheck will automatically determine the appropriate Boundary Layer refinement parameters based on the selected boundary curve and the Fracture Mechanics Meshing Strategies, or “Manual Values”, in which the user may provide inputs for the Boundary Layer refinement parameters (Ratio, Curvature D/H, Layers, Inner Radius, Total Radius).

Mixed Mesh Toggle

The Mixed Mesh toggle (on by default) functions the same as for the Boundary Layer method, controlling whether the mesh around the crack front is constructed entirely of tetras or a mix of pentas and hexas.

Integration Layer Toggle

The Integration Layer toggle (on by default) will add an additional layer of refinement around the innermost layer. This option helps control the aspect ratio of the elements in which fracture mechanics parameters are to be evaluated, increasing the accuracy of integration. The default automatic parameters will produce 2 geometrically graded layers (plus a 3rd integration layer) for an all tetra mesh and 4 geometrically graded layers (plus a 5th integration layer) for a mixed mesh.

Grade Toward Ends Toggle

The Grade Toward Ends toggle (off by default) will produce a geometric gradation toward either end of the selected curve. Two layers are added to each end of the crack. Their sizes are based on the length of the selected curve representing the crack front; the 1^st layer has a size of 0.15³ times the curve length, and the 2^nd layer is 0.15² times the curve length. This option is useful for controlling error in fracture extractions due to singularities at the free surfaces.

Note: enable Mesh Transparency to verify the crack front automesh. Boundary Layer automesh generation records are frequently combined with Crack Face automesh records in order to reduce discretization error as much as possible for fracture mechanics extractions. For tips on crack front automeshing, refer to Fracture Mechanics Meshing Strategies, Helpful Hints and Tips: Elliptical Crack Automeshing Guidelines and StressCheck Demo: Part-Thru Crack SIFs for Stiffened Lug.

Below is an animated example of MeshSim automesh generation for Create > Mesh > Crack Front with “Automatic Values” selected, and all toggles enabled. To produce an automesh suitable for fracture mechanics parameter extraction, the Crack Front automesh record incorporated multiple layers of graded refinement around the crack front bounding curve.

For a demonstration of this feature, refer to StressCheck Tutorial: Crack Front Automeshing with Mixed Mesh, Integration Layer and Grade Toward Ends Options.

Semi-Automatic Mesh Methods

The Edge to Edge (Planar) or Face to Face (3D) methods may be used to generate a mesh from existing nodes and/or element faces, respectively. Note: these methods do not result in an automesh generation record.

Edge to Edge Method

When two curves containing an equal number of associated nodes are available, the Edge to Edge method will join these nodes with quadrilateral elements. Select one curve, and then select the other curve, and the quadrilateral elements will be automatically generated. Note: if the elements appear to be distorted, you may reverse the direction of one of the curves by using Select > Any Curve > Reverse. Below is an animated example of MeshSim automesh generation for Create > Mesh > Edge to Edge. One circle with 8 nodes is selected, and another circle with 8 nodes is selected to produce a disc of quadrilateral elements.

Face to Face Method

When there is a need to convert a two dimensional model to a three dimensional model, one possible procedure is to make a copy of the original 2D model which is offset in the Z direction. In this case, there is a one to one correspondence between the elements in the original model and the elements in the copy.

One option for constructing 3D elements (hexa or penta) between the two planar sections is to use the Face to Face manual element construction method (e.g. Create > Hexahedron > Face to Face) to join an element in one section with a corresponding element in the other section. This can be a very tedious process, especially when there may be tens or hundreds of elements in each section.

An alternative technique is to use the Create > Mesh > Face To Face method. This meshing method will allow you to join a set of elements in one section with a set of elements in another section in one operation. This technique works best when one of the sections being joined is a copy of the other. The procedure is to simply select the elements from the first section with a marquee pick (red highlight). Then select the elements in the second section with a marquee pick while holding both the Ctrl + Shift keys (green highlight). The two sections will be distinguished by different highlight colors. Click on the Accept button to complete the Face to Face meshing operation. Note: it is best to disable Wetted Faces during this operation in order to visualize the newly generated elements.

After all desired 3D elements have been created, the user must delete the 2D elements. If you are creating elements between only two sections, you may immediately click the Delete button to remove the currently selected 2D elements. If you have more than two profiles, you will have to wait until all sections have been meshed before deleting the 2D elements.

Note: The underlying assumption of this meshing method is that there is a one to one correspondence between elements in the first section and those in the second section, based on the ordering of the elements. For example, suppose there are three elements in each section. Elements in the first section are numbered 1, 2, 3, and elements in the second section are numbered 8, 9, 10. The nodes from element 1 will be joined with the nodes from element 8 to form a new 3D element. Similarly, elements 2 and 9 will form a new element, and 3 and 10 will form a new element. Naturally, each pair of elements must be of the same type (quad/quad or tri/tri). If any of the restrictions are violated, an error message will appear and no elements will be created. This technique can be used in other cases only if some care has been taken to construct the elements in each section such that the order of elements in the first section corresponds properly with the order of the elements in the second section.

Below is an animated example of MeshSim automesh generation for Create > Mesh > Face to Face. The nodes/elements associated with the Planar disc in the Edge to Edge method animated example have already been copied to Z=1, and Wetted Faces have been disabled. Select one set of disc elements, then hold Ctrl + Shift and select the other set of disc elements, then click Accept. The Planar elements may be deleted by clicking the Delete button.

Special Automesh Methods

Match Method

The Match method is currently available for flat surfaces in 3D only. Select one flat surface, then a neighboring flat surface on the same body, and click Accept to save the record. Then, click on the Automesh button to process the record, and any other active records. If the method is successful, the resulting automesh should have matching element faces at the selected surfaces.

Simple Graded Method

For local mesh refinement to be used in combination with Extrusion meshing only. Identify an edge in the front face of a solid body where a mesh refinement is to be inserted. All faces attached to the edge must be quadrilaterals. The elements attached to the edge will be hexahedral. Select the edge(s), supply the input values, and click Accept to save the record. The input values are:

Layers

Number of layers of elements around the selected edge.

Radius

Distance from the edge to the outer face of the mesh refinement layer.

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