Automeshing Secondary Panel

Location: The Automeshing Secondary panel serves as the unified secondary panel for most of the plate and shell meshing panels; using those panels gives you access to this Automeshing Secondary panel. In the Automeshing Secondary panel you can interactively adjust a wide variety of parameters and choose from a suite of algorithms. HyperMesh responds with immediate feedback on the effects of the changes, until you are satisfied with the resulting mesh.

There are two approaches to automatic mesh generation, depending on whether or not you use surfaces as the basis for the operation.

If you use surfaces, you may choose from a greater variety of algorithms, have more flexibility in specifying the algorithm parameters, and employ the mesh-smoothing operation to improve element quality.
If you do not use surfaces, the meshing process is usually faster and uses less memory. Most of the functions are still available and operate in the same way. Furthermore, there are situations in which it is not possible or not desirable to create a surface.

For either approach, the panel operates the same. You control interactively the number of elements on each edge or side, and can determine immediately the nodes that are used to create the mesh. You can adjust the node biasing on each edge to force more elements to be created near one end than near the other, which allows you to immediately see the locations of the new nodes. You can also specify whether the new elements should be quads, trias, or mixed and whether they should be first or second order elements. The created mesh can be previewed, allowing you to evaluate it for element quality before choosing to store it in the database. While you are in the meshing module, you can use any of viewing tools on the visual options menu to simplify the visualization of complex structures in your model.

Figure 1. Solid Model Created by Dragging Automeshed Plate Elements		Figure 2. Second Order Elements Created for Boundary Element Solutions

The Automeshing Secondary panel shows the pre-generated mesh from its preceding Automesh subpanel, and provides tools to adjust the mesh before finalizing it.

While you are using the Automeshing Secondary panel, the function keys are disabled and you cannot change the element order on the Options panel.

As a secondary panel dependent on the subpanel that activates it, the changes you make are only applicable to the current meshing action. Leaving the secondary panel will render its settings irrelevant since the only means of return is to restart meshing from one of the Automesh subpanels.

To use the Automeshing Secondary panel:

Set the secondary panel mode by selecting the appropriate subpanel.
Use the criteria presented by the subpanel to alter the final mesh outcome.
Click mesh to finalize the mesh, reject to abort, or smooth to automatically improve the mesh quality.

Density Subpanel

Use the density subpanel to change the node density along a specified edge or edges.

Option	Action
adjust: edge	Change the number of nodes along an edge. When this selector is enabled: Left-click an edge to increase the number of nodes along it; right-click to decrease the number. Click-and-drag the current node density number to increase or decrease it.
calculate: edge	Calculate edge density to support the specified element size. When this selector is enabled, click an edge to set the necessary density to support the specified element size.
calculate: recalc all	Set all edges to the number of nodes necessary to support the specified element size.
elem size=	Specify the desired element size for edges. Use calculate: edge or calculate: recalc all to set edges to the necessary nodal density to support this element size as well as possible. Note: This will be a "best fit" calculation, as it is unlikely that the selected edge will be exactly the right length for the specified element size.
link opposite edges	Changes applied to one linked edge will be applied to the opposite edge of simple chains when edges are clicked.
set: edge	Set an edge's nodal density to the value specified in the elem density field. When this selector is enabled, click an edge to set its nodal density.
set: set to all	Set all edges to the nodal density specified in the elem density field.
elem density	Specify a required number of elements to lie on the edge, producing a number of nodes one greater than this value.
local view	Open the Local View menu to access display tools that are customized for use in the Automeshing Secondary panel.

Mesh Style Subpanel

Use the Mesh Style subpanel to specify the meshing algorithm to use for each face of each domain when you are following a surface-based approach.

Option

Action

elem type

Change the element type assigned to the selected surface(s).

toggle surf

Change the element type assigned to the selected surface by enabling the selector and then clicking the icon in the center of the surface to cycle through the available element types.

set surf

Set specific surfaces to the element type selected from the element type drop-down by enabling the selector and then clicking a surface.

set all

Set all visible surfaces to the element type selected from the element type drop-down.

mesh type

Select the element type to apply to surfaces when using the set surf and set all options.

Figure 4. Tria Elements		Figure 5. Quad Elements
	Figure 6. Mixed Elements. Density 10 at top, density 5 at bottom.
Figure 7. R-Tria Elements		Figure 8. Quad Only Elements. Density 10 at top, 5 at bottom.

Note: In certain cases quads may still use a small number of tria elements when the mesh quality using only quads would not be acceptable. Quads only never uses trias, regardless of the resulting mesh quality.

If you use the mixed (quads and trias) element type, the automesher uses a modified map as rectangle meshing scheme. The modification makes transitions between differing element densities through the use of triangles. This tends to produce mesh patterns that are more regular in appearance.

mesh method

Change the mesh mapping method assigned to the selected surface(s).

toggle surf: Change the mesh mapping method assigned to the selected surface by enabling the selector and then clicking the icon in the center of the surface to cycle through the available mesh mapping methods.

Figure 10. Mesh Mapping Icons on Surface
set surf: Set specific surfaces to the mesh mapping method selected from the mesh mapping method drop-down by enabling the selector and then clicking a surface.
set all: Set all visible surfaces to the mesh mapping method selected from the mesh mapping method drop-down.
mesh method: Select the mesh mapping method to apply to surfaces when using the set surf and set all options.

Figure 11. Example: Mesh Mapping Methods; Note: When using autodecide, the mesh mapping method will change automatically to one of the other types after clicking mesh. This is because autodecide chooses the best option from the other types before the mesh is applied.
Even if you do not use autodecide, the meshing engine may change the mapping method if it is clearly inappropriate for the surface being meshed. For example, it will not apply triangular mapping to a uniformly square surface, but instead will change the mapping method to triangular.

set

set surf: Apply the flow and map settings to specific surfaces by enabling the selector and then clicking a surface.
set all: Apply the flow and map settings to all surfaces.

flow: align

Produce a more orthogonal quad-dominant mesh.

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.

map: smoothing

Perform an automatic cleanup pass on the generated mesh in an effort to improve the overall element quality.

local view

Open the Local View menu to access display tools that are customized for use in the Automeshing Secondary panel.

Biasing Subpanel

Use the Biasing subpanel to apply linear, exponential, or bellcurve biasing to individual edges of a surface.

Option	Action
adjust: edge	Change the biasing factor for an edge. When this selector is enabled: Left-click an edge to increase the biasing factor; right-click to decrease the number. Click-and-drag the numerical biasing factor to increase or decrease it. Dragging upwards increases and dragging downwards decreases. Figure 16. Increase Biasing Factor
calculate: edge	Set an edge's biasing factor to the specified intensity value by enabling the selector and clicking an edge.
revert: edge	Revert an edge in the opposite direction by enabling the selector and clicking the edge.
recalc all	Set all edge's biasing factor to the specified intensity value.
intensity=	Specify a biasing factor. This value will be applied to the edge(s) selected using the calculate: edge or recalc all options.
link opposite edges	Changes applied to one linked edge will be applied to the opposite edge of simple chains when edges are clicked.
set	set edge Assign the biasing style selected from the bias style drop-down to specific edges by enabling the selector and then clicking the desired edge's biasing indicator. Biasing Indicators Linear Exponential Bellcurve set all to Assign the biasing style selected from the bias style drop-down to all edges.
bias style	Select the biasing style to apply to edges when using the set edge and set all to options. Figure 17. Example: Bias Style
local view	Open the Local View menu to access display tools that are customized for use in the Automeshing Secondary panel.

Checks Subpanel

Use the Checks subpanel to use the functions of the Check Elements panel on a newly-generated mesh before storing it in the database. The tests are the same as on the Check Elements panel, and elements that fail a quality test are highlighted in red. Only displayed elements are tested; the display of elements is controlled by the local view panel. The Checks subpanel operates on a by-face method. The active highlighted face serves as a frame of reference for meshing, smoothing, and display operations. To select another face, select the face's icon in the modeling window.

In this subpanel, you can specify minimum or maximum values for element quality criteria according to several measures. The final mesh will attempt to adhere to the requirements set on this panel by producing elements that do not violate these quality criteria.

The criteria includes warpage, aspect, skew, min angle and max angle (quads only), length, jacobian, and min angle/max angle (trias only).

Open the Local View menu to access display tools that are customized for use in the Automeshing Secondary panel.

Local View Menu

The Local View menu contains displays tools that are customized for the Automeshing Secondary panel. All the options orient the view, keeping the current surface centered in the window. You may also choose to suppress the display of nodes and elements.

The details and checks subpanels contain an expanded Local View menu with additional tools, which can be used to change the view with the focus staying centered on the highlighted face. You may also suppress the display of nodes or elements separately for the highlighted face and for the remaining faces of the surface.

cw, ccw: Rotate the view clockwise or counterclockwise around the center of the surface, ignoring everything else in the HyperMesh database.
left, right, top, bottom, rear, front: Set the view to look from that direction, and then fills the screen with the surface.
fill surf: Size the selected surface(s) to fill the modeling window.
elemts, nodes, all nodes: Control the display of elements and nodes.

Tip:

The ability to hide elements of other faces is particularly useful when you have a complicated surface with several faces and the some surfaces are interfering with your view.
It can be helpful to display all of the elements of the other faces and hide those of one face. In this way, you can look inside a complicated object.

Command Buttons

Button	Action
mesh	Scan through all of the faces in the current frame of reference for ones that have not yet been meshed or have a mesh that is out of date with respect to the user-specified parameters, and then attempt to bring them up to date. If the current subpanel is density, mesh style, type, or biasing, the current frame of reference is the entire surface. If the current subpanel is details or checks, the current frame of reference is the highlighted face.
reject	Discard a generated mesh of one selected face or of all of the faces of the current domain.
smooth	Apply a mesh smoothing algorithm to each face in the current frame of reference.
undo	Return the nodes on the mesh to the positions they were in before the last time you applied a smooth to that mesh for each face in the current frame of reference.
abort	Exit the Automeshing Secondary panel without saving any elements or nodes to the database. If the module was entered from a surface creation panel, any surface that may have been created is discarded.
return	Exit the Automeshing Secondary panel, and save elements or nodes to the database.