Automesh Panel

Size and Bias Subpanel

Use the Size and Bias subpanel to perform size and bias meshing, a flexible and powerful meshing method. A minimum of inputs are required for the element criteria settings. The algorithm options set preferences on how to handle certain situations when encountered in the geometry. When using existing finite elements as the basis for mesh generation, feature recognition settings allow the mesher to break up the areas defined by the selected elements into logical groupings with mesh controls set for each group boundary.

Size and Bias meshing works interactively or automatically. In interactive mode, manual control is presented via the Secondary Automesh panel during the mesh generation stage. Interactive meshing allows you to control mesh size and element type, and to set different mesh generation algorithms and test element quality on a surface-by-surface basis. The resulting modified mesh can be updated at any time, giving immediate feedback as to the effectiveness of the change. When meshing in the automatic mode, the mesh will be generated using only the settings, criteria and options set in the Automesh panel.

Size and biasing meshing produces a mesh with consistent element size. If meshed interactively, the number of elements (element density) node spacing (biasing), element type and mesh style can be modified for each surface face and edge.

Option	Action
entity selector	Select surfaces or existing finite elements to define the area to mesh.
features	When using existing finite elements as a basis for automeshing, feature recognition is used to define logical faces. Select how the automesher treats features. connected features Detect features based on the specified feature angle and make additional effort to void any "orphan" or non-closed feature lines. Connected features is similar to auto detect features, but includes a more rigorous check to combine small areas and avoid creating features that end abruptly or do not connect to any other features. Figure 1. Before Re-meshing   Figure 2. After Re-meshing auto detect features Detect features based on the specified feature angle. feature edges Select surface edges to preserve as features. lines Select lines in geometry to preserve as features. surface edges Detect and utilize the geometric lines associated with the selected elements as features in the re-meshing operation. Figure 3. Before Re-meshing   Figure 4. After Re-meshing
interactive/automatic	interactive Expose the interactive Automeshing secondary panel once the meshing has started. automatic Use only the settings and selections made in the panel to complete the meshing process.
element size	Enter a floating point numeric value for the average element size. The length of any active (shared or free) surface edge will be divided by this number to determine the number of elements to place along that edge.
mesh type	Select the type of element to use during mesh creation. Mixed Uses quads primarily, but inserts trias when making density transitions, resulting in improved mesh quality. Figure 5. Example: Mixed Elements Quads Attempts to use quads only, however, at least one tria element must be created if the sum of the element densities around the perimeter of the face or surface is odd. Figure 6. Example: Quad Elements. The sum of element densities on the perimeter of the lower surface is odd, resulting in a tria. Adjusting the element densities while meshing interactively can usually eliminate all tria elements. Figure 7. Example: Quad Elements. Adjusting the bottom edge density from 11 to 10 makes the sum even and generates all-quads. Quads only Uses a subdividing routine that tends to generate more orthogonal quad elements. Tria elements may still be introduced depending on the density settings. Figure 8. Example: Quad Elements Only Tria Uses all trias to mesh. Figure 9. Example: Tria Elements Advanced Choose any of the other types individually for mapped elements (elements on surfaces that can be mapped to simple geometric shapes) and free elements (those that cannot easily map to simple shapes).
mapped type	Select the type of elements to use for surfaces that can be mapped to simple geometric shapes.
free type	Select the type of elements to use for surfaces that cannot be mapped to simple geometric shapes.
feature angle	Define a maximum angle across which elements can be maintained. Note: Any time two adjacent elements’ normals would exceed this angle, a new set of nodes is created between them to maintain clean feature lines. Using a higher value results in elements spanning the feature line. Figure 10. Feature Lines Preserved. With an appropriate value, the features lines are preserved. Figure 11. Feature Lines Blurred. If the feature angle is too high, the feature lines are blurred.
vertex angle	Define the angle used for breaking feature-edges into simpler segments.
elems to surf comp/elems to current comp	Select the destination component for the newly created elements as the “current” active component or the component to which the surface belongs.
first order/second order	first order Linear shape function second order Polynomial shape function
connectivity	Select how the connectivity between the newly created elements and any adjacent existing elements will be handled. keep connectivity Use the existing nodes on any shared boundary edges. redo connectivity Re-seed any existing nodes along the boundary of the newly created mesh to optimize mesh quality. break connectivity Ignore any existing adjacent elements and generate the mesh according to the size and type specified.
flow: align	Produce a more orthogonal quad-dominant mesh. Figure 12. No Flow Alignment Figure 13. Flow Alignment. Flow alignment is used, producing straighter rows of elements.
flow: size	Enforces a global mesh element size with minimal min/max element size variation. Important: Only available when flow: align is selected.
map: size	Keep the elements roughly the same size.
map: skew	Prevent the mesh from producing highly-skewed elements.
anchor nodes	Designate nodes that will remain and be reused in the new mesh. Anchor nodes are "fixed" so that the automesher cannot move or replace them; in essence, they are exceptions to the re-meshing operation, and the new mesh must utilize them.
link opposite edges with AR <	Link mesh settings on opposing edges of rectangular surfaces. Use the toggle to define the maximum aspect ratio (AR) to allow between large and small edge sizes of linked edges. auto corresponds to a value of 2.11. Increasing the value will add more surfaces to the linked chain, whereas decreasing the value will remove some surfaces from the linked chain. Figure 14. Mesh without Link Opposite Edges with AR < Selected Figure 15. Mesh with Link Opposite Edges with AR < Set to Auto Figure 16. Mesh with Link Opposite Edges with AR < Set to 8.0

Batchmesh/QI Optimize Subpanel

Use the Batchmesh/QI Optimize subpanel to perform Quality Index meshing, an iterative automatic mesh generation method driven by element quality criteria. During the mesh generation process, the quality index of the mesh is determined by evaluating each element against a set of element quality tests. If all required element quality criteria are passed, then that element has a perfect quality index of zero. As the element quality deteriorates, the quality index value increases; a lower quality index score indicates an element more closely meets the ideal quality requirements.

The compound quality index sum of the quality index values for each of the elements is included in the current meshing area. The quality index value itself has no direct physical meaning; it is a way to compare one generated mesh pattern against another pattern generated for that same area. The quality index based mesh optimization routine attempts to modify the mesh pattern and apply node smoothing routines to obtain a lower overall quality index value.

Option	Action
batchmesh/QI optimize	Switch between QI optimize meshing parameters and BatchMesh parameters.
entity selector	Select surfaces or existing finite elements to define the area to mesh.
features	When using existing finite elements as a basis for automeshing, feature recognition is used to define logical faces. Select how the automesher treats features. connected features Detect features based on the specified feature angle and make additional effort to void any "orphan" or non-closed feature lines. Connected features is similar to auto detect features, but includes a more rigorous check to combine small areas and avoid creating features that end abruptly or do not connect to any other features. Figure 17. Before Re-meshing   Figure 18. After Re-meshing auto detect features Detect features based on the specified feature angle. feature edges Select surface edges to preserve as features. lines Select lines in geometry to preserve as features. surface edges Detect and utilize the geometric lines associated with the selected elements as features in the re-meshing operation. Figure 19. Before Re-meshing   Figure 20. After Re-meshing
element size	Enter a floating point numeric value for the average element size. The length of any active (shared or free) surface edge will be divided by this number to determine the number of elements to place along that edge.
mesh type	Select the type of element to use during mesh creation. Mixed Uses quads primarily, but inserts trias when making density transitions, resulting in improved mesh quality. Figure 21. Example: Mixed Elements Quads Attempts to use quads only, however, at least one tria element must be created if the sum of the element densities around the perimeter of the face or surface is odd. Figure 22. Example: Quad Elements. The sum of element densities on the perimeter of the lower surface is odd, resulting in a tria. Adjusting the element densities while meshing interactively can usually eliminate all tria elements. Figure 23. Example: Quad Elements. Adjusting the bottom edge density from 11 to 10 makes the sum even and generates all-quads. Quads only Uses a subdividing routine that tends to generate more orthogonal quad elements. Tria elements may still be introduced depending on the density settings. Figure 24. Example: Quad Elements Only Tria Uses all trias to mesh. Figure 25. Example: Tria Elements Advanced Choose any of the other types individually for mapped elements (elements on surfaces that can be mapped to simple geometric shapes) and free elements (those that cannot easily map to simple shapes).
use current criteria/criteria file	Switch between using the current element quality criteria or use a custom criteria file.
edit criteria	Open the Criteria File Editor. Important: Only available when user current criteria is selected.
feature angle	Define a maximum angle across which elements can be maintained. Note: Any time two adjacent elements’ normals would exceed this angle, a new set of nodes is created between them to maintain clean feature lines. Using a higher value results in elements spanning the feature line. Figure 26. Feature Lines Preserved. With an appropriate value, the features lines are preserved. Figure 27. Feature Lines Blurred. If the feature angle is too high, the feature lines are blurred.
vertex angle	Define the angle used for breaking feature-edges into simpler segments.
smooth across common edges with	Node smoothing moves nodes across adjacent surface edges whose feature angle is less than the value specified. When selected, strict adherence to the geometry of the surface edges in not enforced for non-feature edges; some deviation from the geometry can occur.
elems to surf comp/elems to current comp	Select the destination component for the newly created elements as the “current” active component or the component to which the surface belongs.
first order/second order	first order Linear shape function second order Polynomial shape function
connectivity	Select how the connectivity between the newly created elements and any adjacent existing elements will be handled. keep connectivity Use the existing nodes on any shared boundary edges. redo connectivity Re-seed any existing nodes along the boundary of the newly created mesh to optimize mesh quality. break connectivity Ignore any existing adjacent elements and generate the mesh according to the size and type specified.
flow: align	Produce a more orthogonal quad-dominant mesh. Figure 28. No Flow Alignment Figure 29. Flow Alignment. Flow alignment is used, producing straighter rows of elements.
flow: size	Enforces a global mesh element size with minimal min/max element size variation. Important: Only available when flow: align is selected.
anchor nodes	Designate nodes that will remain and be reused in the new mesh. Anchor nodes are "fixed" so that the automesher cannot move or replace them; in essence, they are exceptions to the re-meshing operation, and the new mesh must utilize them.
preserve edges	Open the Preserve Edges tool and define settings to ensure that specific component edges and feature lines do not accidentally get discarded during auto cleanup or batch meshing.

Edge Deviation Subpanel

Use the Edge Deviation subpanel to set specific meshing parameters to limit how far the mesh elements can deviate from the actual edges of the surfaces meshed, or when in the case of re-meshing elements, deviation from inferred edges based on features.

Controls for the minimum and maximum allowable element size, edge deviation and maximum angle are introduced with this method. Edge deviation normally occurs on curved edges, because individual elements have straight edges and therefore can only approximate a curve.

Figure 30. Meshing Curved Surfaces. The planar elements (tan color) can deviate from the curved grey geometry.

This method can produce a mesh in which the element size varies, even within the same surface. Areas of high curvature will tend to have smaller elements than areas of low or no curvature. The element size boundaries controls this effect.

Figure 31. Example: Edge Deviation. Edge deviation control when meshing creates smaller elements, and spaces nodes closer together to limit how much the elements can deviate from the surface edges.

Option	Action
entity selector	Select surfaces or existing finite elements to define the area to mesh.
features	When using existing finite elements as a basis for automeshing, feature recognition is used to define logical faces. Select how the automesher treats features. connected features Detect features based on the specified feature angle and make additional effort to void any "orphan" or non-closed feature lines. Connected features is similar to auto detect features, but includes a more rigorous check to combine small areas and avoid creating features that end abruptly or do not connect to any other features. Figure 32. Before Re-meshing   Figure 33. After Re-meshing auto detect features Detect features based on the specified feature angle. feature edges Select surface edges to preserve as features. lines Select lines in geometry to preserve as features. surface edges Detect and utilize the geometric lines associated with the selected elements as features in the re-meshing operation. Figure 34. Before Re-meshing   Figure 35. After Re-meshing
interactive/automatic	interactive Expose the interactive Automeshing secondary panel once the meshing has started. automatic Use only the settings and selections made in the panel to complete the meshing process.
min/max element size	Define element size boundaries. Note: The values specified here are rigidly enforced, even if other settings (that is max deviation) are violated.
max deviation	Define an allowable deviation between the element edge and the surface edge. To meet this requirement, element edge lengths along a curved surface edge are reduced as needed down to a lower limit set by the min elem size field.
max angle	Define the maximum allowable angle between two element edges. This helps determine the size of an element to create; if the angle formed by adjacent element edges would exceed this value, smaller elements are tried until the angle is equal to or less than this value.
mesh type	Select the type of element to use during mesh creation. Mixed Uses quads primarily, but inserts trias when making density transitions, resulting in improved mesh quality. Figure 36. Example: Mixed Elements Quads Attempts to use quads only, however, at least one tria element must be created if the sum of the element densities around the perimeter of the face or surface is odd. Figure 37. Example: Quad Elements. The sum of element densities on the perimeter of the lower surface is odd, resulting in a tria. Adjusting the element densities while meshing interactively can usually eliminate all tria elements. Figure 38. Example: Quad Elements. Adjusting the bottom edge density from 11 to 10 makes the sum even and generates all-quads. Quads only Uses a subdividing routine that tends to generate more orthogonal quad elements. Tria elements may still be introduced depending on the density settings. Figure 39. Example: Quad Elements Only Tria Uses all trias to mesh. Figure 40. Example: Tria Elements Advanced Choose any of the other types individually for mapped elements (elements on surfaces that can be mapped to simple geometric shapes) and free elements (those that cannot easily map to simple shapes).
mapped type	Select the type of elements to use for surfaces that can be mapped to simple geometric shapes.
free type	Select the type of elements to use for surfaces that cannot be mapped to simple geometric shapes.
feature angle	Define a maximum angle across which elements can be maintained. Note: Any time two adjacent elements’ normals would exceed this angle, a new set of nodes is created between them to maintain clean feature lines. Using a higher value results in elements spanning the feature line. Figure 41. Feature Lines Preserved. With an appropriate value, the features lines are preserved. Figure 42. Feature Lines Blurred. If the feature angle is too high, the feature lines are blurred.
vertex angle	Define the angle used for breaking feature-edges into simpler segments.
elems to surf comp/elems to current comp	Select the destination component for the newly created elements as the “current” active component or the component to which the surface belongs.
first order/second order	first order Linear shape function second order Polynomial shape function
connectivity	Select how the connectivity between the newly created elements and any adjacent existing elements will be handled. keep connectivity Use the existing nodes on any shared boundary edges. redo connectivity Re-seed any existing nodes along the boundary of the newly created mesh to optimize mesh quality. break connectivity Ignore any existing adjacent elements and generate the mesh according to the size and type specified.
flow: align	Produce a more orthogonal quad-dominant mesh. Figure 43. No Flow Alignment Figure 44. Flow Alignment. Flow alignment is used, producing straighter rows of elements.
flow: size	Enforces a global mesh element size with minimal min/max element size variation. Important: Only available when flow: align is selected.
map: size	Keep the elements roughly the same size.
map: skew	Prevent the mesh from producing highly-skewed elements.
link opposite edges with AR <	Link mesh settings on opposing edges of rectangular surfaces. Use the toggle to define the maximum aspect ratio (AR) to allow between large and small edge sizes of linked edges. auto corresponds to a value of 2.11. Increasing the value will add more surfaces to the linked chain, whereas decreasing the value will remove some surfaces from the linked chain. Figure 45. Mesh without Link Opposite Edges with AR < Selected Figure 46. Mesh with Link Opposite Edges with AR < Set to Auto Figure 47. Mesh with Link Opposite Edges with AR < Set to 8.0
anchor nodes	Designate nodes that will remain and be reused in the new mesh. Anchor nodes are "fixed" so that the automesher cannot move or replace them; in essence, they are exceptions to the re-meshing operation, and the new mesh must utilize them.

Surface Deviation Subpanel

The meshing behavior in this subpanel is driven by distances between flat elements and model geometry. When flat elements are used to approximate a curved surface, there is always a discrepancy between each element and the actual curve of the surface, because the element uses a straight line between two nodes.

Figure 48. Surface Deviation. A gap is visible between the curved edge of the surface and the element edges.

The Surface Deviation meshing chooses the mesh density based on the severity of this deviation. Where the threshold deviation would be exceeded, smaller elements are used to reduce the deviation.

Figure 49. Surface Deviation Meshing. Smaller elements are used to accurately represent curved surfaces. Larger elements are used where the geometry shows less curvature.

Surface Deviation meshing only works in an automatic mode; interactive meshing with the Secondary Automesh panel is not possible. However, use the refine function to set a specific desired mesh size for a point, line or surface face. This option accesses another temporary subpanel that is slaved to the Surface Deviation subpanel. From this subpanel, select fixed points, lines, or surfaces to define an area in which you desire a more refined mesh. You can specify a different element size for these areas, which displays as a color-coded numeric value: yellow for points, green for lines, or red for surfaces. An option to show all or show active toggles the view of these numeric values; show active displays only the refinement value for the most recently selected point, line or surface, while show all shows all values for all selected entities.

After specifying refinement options, click mesh to create a smoothly-scaled mesh from your base element size to the size specified in the refine options.

Figure 50. Surface Deviation, Refinement Not Applied. The colored numbers indicate refinement targets: point (yellow), line (green), and surface (red).

Figure 51. Surface Deviation, Refinement Applied. The mesh is finer near the point (yellow), along the line/edge (green), and on the surface (red).

Option	Action
entity selector	Select surfaces or existing finite elements to define the area to mesh.
element size	Enter a floating point numeric value for the average element size. The length of any active (shared or free) surface edge will be divided by this number to determine the number of elements to place along that edge.
growth rate	Determine how rapidly elements can increase in size as they are created further and further away from features. Figure 52. Example: Growth Rate. Elements further from the features grow larger with each row.
min element size	Elements with edges smaller than this value will not be created.
span angle	Controls the element size at curve input. The smaller the angle, the more refined curvature will be and the more preserved the input shape will be. By default span angle is 25.0 degrees. Important: Valid only for element-based surface deviation. Figure 53. Example: Span Angle. β is the span angle of the edge ab. The length of ab is less than 2R( sin β/2 ).
feature angle	Define a maximum angle across which elements can be maintained. Note: Any time two adjacent elements’ normals would exceed this angle, a new set of nodes is created between them to maintain clean feature lines. Using a higher value results in elements spanning the feature line. Figure 54. Feature Lines Preserved. With an appropriate value, the features lines are preserved. Figure 55. Feature Lines Blurred. If the feature angle is too high, the feature lines are blurred.
max deviation	Define an allowable deviation between the element edge and the surface edge. To meet this requirement, element edge lengths along a curved surface edge are reduced as needed down to a lower limit set by the min elem size field.
mesh type	Select the type of element to use during mesh creation. Mixed Uses quads primarily, but inserts trias when making density transitions, resulting in improved mesh quality. Figure 56. Example: Mixed Elements Quads Attempts to use quads only, however, at least one tria element must be created if the sum of the element densities around the perimeter of the face or surface is odd. Figure 57. Example: Quad Elements. The sum of element densities on the perimeter of the lower surface is odd, resulting in a tria. Adjusting the element densities while meshing interactively can usually eliminate all tria elements. Figure 58. Example: Quad Elements. Adjusting the bottom edge density from 11 to 10 makes the sum even and generates all-quads. Quads only Uses a subdividing routine that tends to generate more orthogonal quad elements. Tria elements may still be introduced depending on the density settings. Figure 59. Example: Quad Elements Only Tria Uses all trias to mesh. Figure 60. Example: Tria Elements Advanced Choose any of the other types individually for mapped elements (elements on surfaces that can be mapped to simple geometric shapes) and free elements (those that cannot easily map to simple shapes).
mapped type	Select the type of elements to use for surfaces that can be mapped to simple geometric shapes.
free type	Select the type of elements to use for surfaces that cannot be mapped to simple geometric shapes.
elems to surf comp/elems to current comp	Select the destination component for the newly created elements as the “current” active component or the component to which the surface belongs.
first order/second order	first order Linear shape function second order Polynomial shape function
connectivity	Select how the connectivity between the newly created elements and any adjacent existing elements will be handled. keep connectivity Use the existing nodes on any shared boundary edges. redo connectivity Re-seed any existing nodes along the boundary of the newly created mesh to optimize mesh quality. break connectivity Ignore any existing adjacent elements and generate the mesh according to the size and type specified.
closed volume proximity	Dynamically create finer mesh across the narrow spaces between features in a closed volume/solid entity.
free edge deviation	Produce a finer mesh around curved edges (such as holes) even on planar surfaces. Clear this checkbox to base the mesh on surface chordal deviation only.
refine	Open a temporary subpanel, from which you can perform mesh refinement on or around specific points, lines, or surfaces. Use the switch to select the type of entity to use as a basis, then select the points/lines/surfaces and specify an element size in the numeric box.
show refined	If you use refine to perform localized mesh refinement, this checkbox displays the refinement element size you assigned to each entity marked for refinement.

Rigid Body Mesh Subpanel

Rigid bodies are surfaces that are expected to be treated as undeformable in the solution. One example of a rigid body is in metal-forming. When modeling the results of a die pressing down on a metal sheet, it's important to model the shape of the die because that determines the shape of the metal sheet after being pressed. However, during a forming analysis the stresses and deformations of the die itself are not of interest, only those of the formed metal sheet. Other applications for rigid bodies include the impactors used in vehicle crash simulation.

A mesh that accurately represents the rigid geometry is important for such simulations to allow the solver collision detection routines to work effectively and accurately. Since stress and deformation of the rigid body are not calculated by the solver, the rigid body mesh focuses on accurately modeling the shape of the body rather than on producing a high-quality mesh. To this end, it uses the same faceting and shading routines that are used for drawing the model graphics. The resulting mesh may have high aspect ratio or extremely tapered elements that would not be suitable for solution, but can accurately represent the geometry.

Figure 61 and Figure 61 illustrate the differences between surface deviation meshing and rigid body meshing. Both meshes were generated using the same parameters in terms of min/max element size, maximum deviation and feature angle, and mesh type.

Figure 61. Cone with Surface Deviation Based Mesh. Many small elements are required to capture the geometry, even so, the elements exhibit a lot of warpage and those at the tip are distorted and do not accurately represent the geometry.

Figure 62. Cone with Rigid Body Mesh. The shape of the object can be accurately modeled using fewer larger elements since the element shape is not a concern.

Option	Action
entity selector	Select surfaces or existing finite elements to define the area to mesh.
min/max element size	Define element size boundaries. Note: The values specified here are rigidly enforced, even if other settings (that is max deviation) are violated.
max deviation	Define an allowable deviation between the element edge and the surface edge. To meet this requirement, element edge lengths along a curved surface edge are reduced as needed down to a lower limit set by the min elem size field.
max feature angle	Define a maximum allowable break angle between adjacent elements. The element size is adjusted such that the angle between the normals of adjacent elements does not exceed this value. Figure 63. . The minimum and maximum element sizes are 3 and 50 respectively. The mesh is constrained by the max deviation value set to 0.5. The element size is set such that the maximum distance between the element and the spherical surface does not exceed this setting. Figure 64. . The minimum and maximum element sizes are 3 and 50 respectively. The deviation setting is relaxed to 3.0, and the mesh is bound by the maximum feature angle setting of 45 degrees.
mesh type	Select the type of element to use during mesh creation. Mixed Uses quads primarily, but inserts trias when making density transitions, resulting in improved mesh quality. Figure 65. Example: Mixed Elements Tria Uses all trias to mesh. Figure 66. Example: Tria Elements