Chapter 7: Meshing Your Solid Model

Chapter 1 * Chapter 2 * Chapter 3 * Chapter 4 * Chapter 5 * Chapter 6 * Chapter 7 * Chapter 8 * Chapter 9 * Chapter 10 * Chapter 11 * Chapter 12 * Chapter 13 * Chapter 14

7.1 How to Mesh Your Solid Model

• Set the element attributes (described in Section 7.2).
• Set mesh controls (optional). ANSYS offers a large number of mesh controls, which you can choose from to suit your needs. Review Section 7.3 and Section 7.4 for descriptions of these mesh controls.
• Generate the mesh (described in Section 7.5).

7.1.1 Free or Mapped Mesh?

Compared to a free mesh, a mapped mesh is restricted in terms of the element shape it contains and the pattern of the mesh. A mapped area mesh contains either only quadrilateral or only triangular elements, while a mapped volume mesh contains only hexahedron elements. In addition, a mapped mesh typically has a regular pattern, with obvious rows of elements. If you want this type of mesh, you must build the geometry as a series of fairly regular volumes and/or areas that can accept a mapped mesh.

Figure 7-1 Free and mapped meshes

You use the MSHKEY command or the equivalent GUI path (both of which are described later) to choose a free or a mapped mesh.

Keep in mind that the mesh controls you use will vary depending on whether a free or mapped mesh is desired. The details of free and mapped meshing will be explained later.

7.2 Setting Element Attributes

• Element type (for example, BEAM3, SHELL61, etc.)
• Real constant set (usually comprising the element's geometric properties, such as thickness or cross-sectional area)
• Material properties set (such as Young's modulus, thermal conductivity, etc.)
• Element coordinate system
• Section ID (for BEAM188 and BEAM189 elements only-see Section 7.5.2)

7.2.1 Creating Tables of Element Attributes

A table of coordinate systems can also be assembled using commands such as LOCAL, CLOCAL, etc. (Utility Menu>WorkPlane>Local Coordinate Systems> Create Local CS>option). This table can be used to assign element coordinate systems to elements. (Not all element types can be assigned a coordinate system in this manner. See Section 3.5 of this manual for information about element coordinate systems. For element descriptions, see the ANSYS Elements Reference.)

For beam meshing with BEAM188 or BEAM189 elements, you can build a table of sections using the SECTYPE and SECDATA commands (Main Menu> Preprocessor>Sections).

Note-Orientation keypoints are attributes of a line; they are not element attributes. You cannot create tables of orientation keypoints. See Section 7.2.2 for more information.

The element attribute tables described above can be visualized as shown in Figure 7-2. (For more information on creating your element attribute tables, see Chapter 1 of the ANSYS Basic Analysis Procedures Guide.)

Figure 7-2 Element attribute tables

You can review the contents of the element type, real constant, and material tables by issuing the ETLIST (TYPE table), RLIST (REAL table), or MPLIST (MAT table) commands (or by choosing the equivalent menu path Utility Menu>List> Properties>property type). You can review the coordinate system table by issuing CSLIST (Utility Menu>List>Other>Local Coord Sys). You can review the section table by issuing SLIST (Main Menu>Preprocessor>Sections>List Sections).

7.2.2 Assigning Element Attributes Before Meshing

Note-As stated earlier, although you can assign orientation keypoints as attributes of a line for beam meshing, you cannot build tables of orientation keypoints. Therefore, to assign orientation keypoints as attributes, you must assign them directly to selected lines; you cannot define a default set of orientation keypoints to be used in subsequent meshing operations. See Section 7.5.2 for details about assigning orientation keypoints.

7.2.2.1 Assigning Attributes Directly to the Solid Model Entities

Use the commands and GUI paths listed below to assign attributes directly to solid model entities.

• To assign attributes to keypoints:

KATT

Main Menu>Preprocessor>-Attributes-Define>All Keypoints
Main Menu>Preprocessor>-Attributes-Define>Picked KPs

• To assign attributes to lines:

LATT

Main Menu>Preprocessor>-Attributes-Define>All Lines
Main Menu>Preprocessor>-Attributes-Define>Picked Lines

• To assign attributes to areas:

AATT

Main Menu>Preprocessor>-Attributes-Define>All Areas
Main Menu>Preprocessor>-Attributes-Define>Picked Areas

• To assign attributes to volumes:

VATT

Main Menu>Preprocessor>-Attributes-Define>All Volumes
Main Menu>Preprocessor>-Attributes-Define>Picked Volumes

7.2.2.2 Assigning Default Attributes

To assign a set of default attributes:

Command(s):

TYPE, REAL, MAT, ESYS, SECNUM

Main Menu>Preprocessor>-Attributes-Define>Default Attribs
Main Menu>Preprocessor>-Modeling-Create>Elements>Elem Attributes

7.2.2.3 Automatic Selection of the Dimensionally Correct Element Type

Specifically, if you fail to assign an element type directly to a solid model entity [xATT] and the default element type [TYPE] is not dimensionally correct for the operation that you want to perform, but there is only one dimensionally correct element type in the currently defined element attribute tables, ANSYS will automatically use that element type to proceed with the operation.

The meshing and extrusion operations affected by this feature are KMESH, LMESH, AMESH, VMESH, FVMESH, VOFFST, VEXT, VDRAG, VROTAT, and VSWEEP.

7.3 Mesh Controls

Mesh controls allow you to establish such factors as the element shape, midside node placement, and element size to be used in meshing the solid model. This step is one of the most important of your entire analysis, for the decisions you make at this stage in your model development will profoundly affect the accuracy and economy of your analysis. (See Chapter 2 of this manual for more detailed discussions of some of the factors you should consider as you set mesh controls.)

7.3.1 The ANSYS MeshTool

Although all of the functions available via the MeshTool are also available via the traditional ANSYS commands and menus, using the MeshTool is a valuable shortcut.

The many functions available via the MeshTool include:

• Controlling SmartSizing levels
• Setting element size controls
• Specifying element shape
• Specifying meshing type (free or mapped)
• Meshing solid model entities
• Clearing meshes
• Refining meshes

7.3.2 Element Shape

A Note About Degenerate Element Shapes

Figure 7-3 An example of a degenerate element shape

Although it can be helpful for you to understand this concept, when specifying element shapes before meshing, you do not have to concern yourself with whether a shape is the default or degenerate shape of a particular element. Instead, you can think in more simpler terms of the desired element shape itself (quadrilateral, triangle, hexahedra, or tetrahedra).

For details about degenerate element shapes, see the ANSYS Elements Reference.

7.3.2.1 Element Shape Specification

Command(s):

MSHAPE,KEY,Dimension

Main Menu>Preprocessor>MeshTool
Main Menu>Preprocessor>-Meshing-Mesher Opts
Main Menu>Preprocessor>-Meshing-Mesh>-Volumes-Mapped>4 to 6 sided

There are two factors to consider when specifying element shape: the desired element shape and the dimension of the model to be meshed.

Command Method

• When KEY=0, ANSYS meshes with quadrilateral-shaped elements if Dimension=2D and with hexahedral-shaped elements if Dimension=3D (as long as the element type supports quadrilateral or hexahedral element shapes, respectively).
• When KEY=1, ANSYS meshes with triangle-shaped elements if Dimension=2D and with tetrahedral-shaped elements if Dimension=3D (as long as the element type supports triangle or tetrahedral element shapes, respectively).

GUI Method (Via the MeshTool)

Note-Since element shape specification is closely related to the type of meshing that you request (free or mapped), it may help you to read Section 7.3.3 of this manual ("Choosing Free or Mapped Meshing") before specifying element shape.

In some cases, the MSHAPE command and the appropriate meshing command (AMESH, VMESH, or the equivalent menu path Main Menu>Preprocessor> -Meshing-Mesh>meshing option) are all that you will need to mesh your model. The size of each element will be determined by default element size specifications [SMRTSIZE or DESIZE]. For instance, the model below in Figure 7-4 (left) can be meshed with one VMESH command to produce the mesh shown on the right:

Figure 7-4 Default element sizes

The element sizes that the program chose for the above model may or may not be adequate for the analysis, depending on the physics of the structure. One way to change the mesh would be to change the default SmartSize level [SMRTSIZE] and remesh. For details, see Section 7.3.5 of this manual ("Smart Element Sizing for Free Meshing").

7.3.3 Choosing Free or Mapped Meshing

Command(s):

MSHKEY

Main Menu>Preprocessor>MeshTool
Main Menu>Preprocessor>-Meshing-Mesher Opts

As described in Section 7.3.2.1, "Element Shape Specification," you can use the MeshTool (Main Menu>Preprocessor>MeshTool) to specify meshing type. The MeshTool is the recommended method. Refer to Section 7.3.2.1 for related information.

Together, the settings for element shape [MSHAPE] and meshing type [MSHKEY] affect the resulting mesh. Table 7-1 shows the combinations of element shape and meshing type that the ANSYS program supports.

Table 7-1 Supported combinations of element shape and meshing type

Element Shape	Free Meshing	Mapped Meshing	Mapped If Possible; Otherwise Free Mesh With SmartSizing On
Quadrilateral	Yes	Yes	Yes
Triangle	Yes	Yes	Yes
Hexahedral	No	Yes	No
Tetrahedral	Yes	No	No

Table 7-2 explains what happens when you fail to specify values for these settings.

Table 7-2 Failure to specify element shape and/or meshing type

Your action...	How it affects the mesh...
You issue the MSHAPE command with no arguments.	ANSYS uses quadrilateral-shaped or hexahedral-shaped elements to mesh the model, depending on whether you are meshing an area or a volume.
You do not specify an element shape, but you do specify the type of meshing to be used.	ANSYS uses the default shape of the element to mesh the model. It uses the type of meshing that you specified.
You specify neither an element shape nor the type of meshing to be used.	ANSYS uses the default shape of the element to mesh the model. It uses whichever type of meshing is the default for that shape.

See the descriptions of the MSHAPE and MSHKEY commands in the ANSYS Commands Reference for more information.

7.3.4 Controlling Placement of Midside Nodes

• Midside nodes (if any) of elements on a region boundary follow the curvature of the boundary line or area. This is the default.
• Place midside nodes of all elements so that element edges are straight. This option allows a coarse mesh along curves. However, the curvature of the model is not matched.
• Do not create midside nodes (elements have removed midside nodes).

Command(s):

MSHMID

Main Menu>Preprocessor>-Meshing-Mesher Opts

7.3.5 Smart Element Sizing for Free Meshing

By default, the DESIZE method of element sizing will be used during free meshing (see Section 7.3.6). However, it is recommended that SmartSizing be used instead for free meshing. To turn SmartSizing on, simply specify an element size level on the SMRTSIZE command (see the discussion on basic controls below).

Note-If you use SmartSizing on a model that contains only an area, ANSYS uses the area to calculate the guiding element size that it should use to mesh the model. On the other hand, if you use SmartSizing on a model that contains both an area and a volume, ANSYS uses the volume to calculate the guiding element size for the model. Even if the area in the first model (area only) and the area in the second model (area and volume) are exactly the same, and the SmartSizing setting is the same, the elements that ANSYS uses to mesh the first model will usually not be as coarse as the elements that it uses to mesh the second model. ANSYS does this to prevent volumes from being meshed with too many elements. (However, if you have specified a global element size [ESIZE], the size of the elements will be the same for both models, because ANSYS will use the size that you specified as the guiding element size.)

Note-When you use SmartSizing, we recommend that you specify the desired SmartSizing settings [SMRTSIZE] and then mesh the entire model at once [AMESH,ALL or VMESH,ALL], rather than SmartSizing area by area or volume by volume. SmartSizing a model area by area or volume by volume may result in an unsatisfactory mesh.

7.3.5.1 The Advantages of SmartSizing

If quadrilateral elements are being used for area meshing, SmartSizing tries to set an even number of line divisions around each area so that an all-quadrilateral mesh is possible. Triangles will be included in the mesh only if forcing all quadrilaterals would create poorly shaped elements, or if odd divisions exist on boundaries.

7.3.5.2 SmartSizing Controls - Basic versus Advanced

Basic Controls

Command(s):

SMRTSIZE,SIZLVL

Main Menu>Preprocessor>MeshTool
Main Menu>Preprocessor>-Meshing-Size Cntrls>-SmartSize-Basic

Figure 7-5 shows a model meshed with several different SmartSize settings, including the default size level of 6.

Figure 7-5 Varying SmartSize levels for the same model

Advanced Controls

Use one of the following methods to set advanced SmartSizing controls:

Command(s):

SMRTSIZE and ESIZE

Main Menu>Preprocessor>-Meshing-Size Cntrls>-SmartSize-Adv Opts

7.3.5.3 Interaction with Other Mesh Controls

• Any element size specifications on lines (LESIZE command or menu path Main Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-option) will be used as defined. SmartSizing and the LESIZE command work better together now than they did in releases prior to ANSYS 5.4. When you use SmartSizing on lines that are adjacent to lines that have defined element size specifications, ANSYS always takes the sizes into account before performing SmartSizing, resulting in a better mesh.
• Any element size specifications at keypoints (KESIZE command or menu path Main Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints -option) will be assigned, but may be overridden to accommodate curvature and proximity of features.
• If a global element size is set (ESIZE command or menu path Main Menu>Preprocessor>-Meshing-Size Cntrls>-Global-Size), it will be overridden as necessary to accommodate curvature and proximity of features. If a consistent element size is desired, set the global element size and turn SmartSizing off (SMRTSIZE,OFF or menu path Main Menu> Preprocessor>-Meshing-Size Cntrls>-SmartSize-Basic).
• Default element sizes specified with the DESIZE command (Main Menu> Preprocessor>-Meshing-Size Cntrls>-Global-Other) are ignored when SmartSizing is on.

7.3.6 Default Element Sizes for Mapped Meshing

As an example, the mapped mesh on the left in Figure 7-6 was produced with the element size defaults that exist when you enter the program. The mesh on the right was produced by modifying the minimum number of elements (MINL) and the maximum spanned angle per element (ANGL) on the DESIZE command.

Figure 7-6 Changing default element sizes

For larger models, it may be wise to preview the default mesh that will result from the DESIZE specifications. This can be done by viewing the line divisions in a line display. The steps for previewing a default mesh are as follows:

1. Build solid model.

2. Select element type.

3. Select allowable element shapes [MSHAPE].

4. Select mesher (free or mapped) for meshing [MSHKEY].

5. Issue LESIZE,ALL (this adjusts line divisions based on DESIZE specifications).

6. Request a line plot [LPLOT].

For instance:

	·
	·
	·
ET,1,45 	! 8 node hexahedral-shaped element 
MSHAPE,0 	! Use hexahedra 
MSHKEY,1	! Use mapped meshing
LESIZE,ALL 	! Adjust line divisions based on DESIZE 
LPLOT

If the resulting mesh looks as though it will be too coarse, it can be changed by altering the element size defaults:

	·
	·
	·
DESIZE,5,,30,15 	! Change default element sizes 
LESIZE,ALL,,,,,1 	! Adjust line divisions based on DESIZE, force adjustments
LPLOT

7.3.7 Local Mesh Controls

• To control the global element size in terms of the element edge length used on surface boundaries (lines) or the number of element divisions per line:

ESIZE

Main Menu>Preprocessor>-Meshing-Size Cntrls>-Global-Size

• To control the element sizes near specified keypoints:

KESIZE

Main Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints-All KPs
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints-Picked KPs
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints-Clr Size

• To control the number of elements on specified lines:

LESIZE

Main Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-All Lines
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-Picked Lines
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-Clr Size

Note-When you use the GUI method to set the number of elements on specified lines, and any of those lines is connected to one or more meshed lines, areas, or volumes, ANSYS prompts you to determine whether you want to clear the meshed entities. If you answer yes to the prompt, ANSYS clears the meshed entities. (This occurs only when you perform this operation via the GUI; ANSYS does not prompt you when you use the command method [LESIZE].)

• Hierarchy used for DESIZE element sizing. For any given line, element sizes along the line are established as follows:
  • Line divisions specified with LESIZE are always honored.
  • If line divisions have not been set for the line, KESIZE specifications at its keypoints (if any) are used.
  • If there are no size specifications on the line or on its keypoints, element sizes are established by the ESIZE specification.
  • If none of the above size specifications are set, DESIZE settings will control element sizes for the line.
• Hierarchy used for SMRTSIZE element sizing. For any given line, element sizes along the line are established as follows:
  • Line divisions specified with LESIZE are always honored.
  • If line divisions have not been set for the line, KESIZE specifications at its keypoints (if any) are used, but may be overridden to account for curvature and small geometric features.
  • If there are no size specifications on the line or on its keypoints, ESIZE specification will be used as a starting element size, but may be overridden to account for curvature and small geometric features.
  • If none of the above size specifications are set, SMRTSIZE settings will control element sizes for the line.

If you are performing a linear static structural or linear steady-state thermal analysis, you can let the program establish meshing controls automatically as it adapts element sizes to drive the estimated error in the analysis below a target value. This procedure, known as adaptive meshing, is described in Chapter 3 of the ANSYS Advanced Analysis Techniques Guide.

7.3.8 Interior Mesh Controls

Command(s):

MOPT

Main Menu>Preprocessor>-Meshing-Size Cntrls>-Global-Area Cntrls

7.3.8.1 Controlling Mesh Expansion

Figure 7-9 Area mesh without mesh expansion and with mesh expansion

In Figure 7-9, mesh (a) was created based only on the setting of the ESIZE command (Main Menu>Preprocessor>-Meshing-Size Cntrls>-Global-Size). Notice that the elements are well shaped, but that 698 elements are required to fill the area since the elements are uniformly sized. (The model is made of a single area.) Using the expand option (Lab=EXPND) on the MOPT command, mesh (b) was created with far fewer elements because the mesh is allowed to expand from the small element sizes on the boundaries of the area to much larger elements in the interior. Some of the elements of this mesh, however, have poor aspect ratios (for example, those around the small holes). Another weakness of mesh (b) is that the elements change in size (transition) from the small elements to the larger elements, especially near the small holes.

Note-Although this discussion is limited to area mesh expansion [Lab=EXPND], you can also use the MOPT command to control tetrahedra mesh expansion [Lab=TETEXPND]. See the description of the MOPT command in the ANSYS Commands Reference for more information.

7.3.8.2 Controlling Mesh Transitioning

Figure 7-10 Area mesh with expansion and transition control (MOPT command)

7.3.8.3 Controlling Which Mesher ANSYS Uses

Note-Quadrilateral surface meshes will differ based on which triangle surface mesher is selected. This is true because all free quadrilateral meshing algorithms use a triangle mesh as a starting point.

Command(s):

MOPT

Main Menu>Preprocessor>-Meshing-Mesher Opts

Note-The menu path provided above takes you to the Mesher Options dialog box. References to the Mesher Options dialog box appear throughout this section (Section 7.3.8.3).

Surface Meshing Options

• Let ANSYS choose which triangle surface mesher to use. This is the recommended setting and the default. In most cases, ANSYS will choose the main triangle mesher, which is the Riemann space mesher. If the chosen mesher fails for any reason, ANSYS invokes the alternate mesher and re-tries the meshing operation.

To choose this option, issue the command MOPT,AMESH,DEFAULT. In the GUI, access the Mesher Options dialog box and choose Program Chooses in the Triangle Mesher option menu.

• Main triangle surface mesher (Riemann space mesher). ANSYS uses the main mesher, and it does not invoke an alternate mesher if the main mesher fails. The Riemann space mesher is well suited for most surfaces.

To choose this option, issue the command MOPT,AMESH,MAIN. In the GUI, access the Mesher Options dialog box and choose Main from the Triangle Mesher option menu.

• First alternate triangle surface mesher (3-D tri mesher). ANSYS uses the first alternate triangle mesher, and it does not invoke another mesher if this mesher fails. This option is not recommended due to speed considerations. However, for surfaces with degeneracies in parametric space, this mesher often provides the best results.

To choose this option, issue the command MOPT,AMESH,ALTERNATE. In the GUI, access the Mesher Options dialog box and choose Alternate from the Triangle Mesher option menu.

• Second alternate triangle surface mesher (2-D parametric space mesher). ANSYS uses the second alternate triangle mesher, and it does not invoke another mesher if this mesher fails. This option is not recommended for use on surfaces with degeneracies (spheres, cones, and so on) or on poorly parameterized surfaces because poor meshes may be created.

To choose this option, issue the command MOPT,AMESH,ALT2. In the GUI, access the Mesher Options dialog box and choose Alternate 2 from the Triangle Mesher option menu.

• Let ANSYS choose which quadrilateral surface mesher to use. This is the recommended setting and the default. In most cases, ANSYS will choose the main quadrilateral mesher, which is the Q-Morph (quad-morphing) mesher. For very coarse meshes, ANSYS may choose the alternate quadrilateral mesher instead. If either mesher fails for any reason, ANSYS invokes the other mesher and re-tries the meshing operation.

To choose this option, issue the command MOPT,QMESH,DEFAULT. In the GUI, access the Mesher Options dialog box and choose Program Chooses from the Quad Mesher option menu.

• Main quadrilateral surface mesher (Q-Morph mesher). ANSYS uses the main mesher, and it does not invoke the alternate mesher if the main mesher fails.

In most cases, the Q-Morph mesher results in higher quality elements (see Figure 7-11). The Q-Morph mesher is particularly beneficial to users whose applications require boundary sensitive, highly regular nodes and elements.

Notice that although both meshes shown in Figure 7-11 contain one triangle element (the triangle elements are shaded in the figure), the triangle element in Figure 7-11 (a) occurs on the boundary of the area. The triangle element in Figure 7-11 (b) is an internal element, which is a more desirable location for it in the mesh.

For the Q-Morph mesher to be able to generate an all-quadrilateral mesh of an area, the total number of line divisions on the boundaries of the area must be even. (In most cases, turning on SmartSizing [SMRTSIZE,SIZLVL] will result in an even total number of line divisions on the boundaries.)

A triangle element (or elements) will result in the area mesh if any of these statements is true:

1. The total number of line divisions on the boundaries of the area is odd.

2. Quadrilateral element splitting is turned on for error elements [MOPT,SPLIT,ON or MOPT,SPLIT,ERR] and a quadrilateral element in violation of shape error limits would be created if ANSYS did not split the element into triangles. (Splitting is on for error elements by default.)

3. Quadrilateral splitting is turned on for both error and warning elements [MOPT,SPLIT,WARN], and a quadrilateral element in violation of shape error and warning limits would be created if ANSYS did not split the element into triangles.

4. Quadrilateral element splitting is turned on for either a) error elements or b) error and warning elements, and the area contains a small angle (< 30°) between adjacent boundary intervals. See Figure 7-12.

To choose this option (Q-Morph mesher), issue the command MOPT,QMESH,MAIN. In the GUI, access the Mesher Options dialog box and choose Main from the Quad Mesher option menu.

• Alternate quadrilateral surface mesher. ANSYS uses the alternate mesher, and it does not invoke the main mesher if the alternate mesher fails.

For this mesher to be able to generate an all-quadrilateral mesh of an area, the total number of line divisions on the boundaries of the area must be even, and quadrilateral splitting must be turned off [MOPT,SPLIT,OFF].

To choose this option, issue the command MOPT,QMESH,ALTERNATE. In the GUI, access the Mesher Options dialog box and choose Alternate in the Quad Mesher option menu. To use this mesher, you must also select either the first alternate or the second alternate triangle surface mesher.

Tetrahedral Element Meshing Options

• Let ANSYS choose which tetrahedra mesher to use. This is the default. With this setting, ANSYS uses the main tetrahedra mesher when it can; otherwise, it uses the alternate tetrahedra mesher. (ANSYS always uses the alternate tetrahedra mesher when meshing with p-elements.)

To choose this option, issue the command MOPT,VMESH,DEFAULT. In the GUI, access the Mesher Options dialog box and choose Program Chooses in the Tet Mesher option menu.

• Main tetrahedra mesher (Delaunay technique mesher). For most models, this mesher is significantly faster than the alternate mesher.

To choose the main tetrahedra mesher, issue the command MOPT,VMESH,MAIN. In the GUI, access the Mesher Options dialog box and choose Main in the Tet Mesher option menu.

• Alternate tetrahedra mesher (advancing front mesher from Revision 5.2). This mesher does not support the generation of a tetrahedral volume mesh from facets [FVMESH]. If this mesher is selected and you issue the FVMESH command, ANSYS uses the main tetrahedra mesher to create the mesh from facets and issues a warning message to notify you.

To choose the alternate tetrahedra mesher, issue the command MOPT,VMESH,ALTERNATE. In the GUI, access the Mesher Options dialog box and choose Alternate in the Tet Mesher option menu.

7.3.8.4 Controlling Tetrahedral Element Improvement

Command(s):

MOPT,TIMP,Value

Main Menu>Preprocessor>-Meshing-Mesher Opts

Levels for tetrahedra improvement range from 1 to 6, with level 1 offering only minimal improvement, level 5 offering the maximum amount of improvement for linear tetrahedral meshes, and level 6 offering the maximum amount of improvement for quadratic tetrahedral meshes. The minimal level of improvement [MOPT,TIMP,1] is supported by the main tetrahedra mesher only [MOPT,VMESH,MAIN]. If the alternate tetrahedra mesher [MOPT,VMESH,ALTERNATE] is invoked when improvement is set to level 1, ANSYS automatically performs tetrahedra improvement at level 3 instead. You can also turn tetrahedra improvement off, but doing so is not recommended because it often leads to poorly shaped elements and meshing failures. For more details about each improvement level, see the description of the MOPT command in the ANSYS Commands Reference.

Note-In most cases, the default levels that ANSYS uses for tetrahedra improvement will give you satisfactory results. However, there may be times when you want to request additional improvement of a given tetrahedral element mesh by using the VIMP command. See Section 7.6.5 for details about how to request additional improvement and when doing so would benefit you.

7.3.9 Creating Transitional Pyramid Elements

Unfortunately, using a mix of hexahedral and tetrahedral element shapes leads to nonconformities in a mesh, and the finite element method requires that elements within a mesh conform. You can avoid the problems that may arise from this situation by following the guidelines outlined below. By instructing ANSYS to automatically create pyramid elements at their interface, you can easily maintain mathematical continuity between hexahedral and tetrahedral element types.

7.3.9.1 Situations in which ANSYS Can Create Transitional Pyramids

• You are ready to mesh a volume with tetrahedral elements. The volume immediately adjacent to that volume has already been meshed with hexahedral elements. The two volumes have been glued together [VGLUE]. (Two volumes for which you want to create transitional pyramids must share a common area; the quadrilateral faces from the hexahedral elements must be located on that common area.)
• At least one of the areas on a volume has been meshed with quadrilateral elements. In this situation you simply mesh the volume with tetrahedral elements, and ANSYS forms the pyramids directly from the quadrilateral elements. If you want, you can then mesh any adjacent volumes with hexahedral elements.

Figure 7-13 Creation of transitional pyramid elements at an interface

7.3.9.2 Prerequisites for Automatic Creation of Transitional Pyramid Elements

• When you set your element attributes, be sure that the element type you assign to the volume is one that can be degenerated into a pyramid shape; currently, this list includes SOLID62, SOLID73, VISCO89, SOLID90, SOLID95, SOLID96, SOLID97, and SOLID122. ANSYS does not support transitional pyramids for any other element types. (See Section 7.2.2 for information about the methods you can use to set attributes.)
• When you set your meshing controls, activate transitioning and indicate that you want to degenerate three-dimensional elements.

To activate transitioning (the default), use one of the following methods:

MOPT,PYRA,ON

Main Menu>Preprocessor>-Meshing-Mesher Opts

To degenerate three-dimensional elements, use one of the following methods:

MSHAPE,1,3D

Main Menu>Preprocessor>-Meshing-Mesher Opts

If these prerequisites are met and you now mesh the volume with tetrahedral elements [VMESH], the ANSYS program automatically:

• Determines where transitional pyramid elements are appropriate
• Combines and rearranges tetrahedral elements to create pyramid elements
• Inserts the pyramid elements into the mesh

Note-For quadratic pyramid elements that are immediately adjacent to linear hexahedral elements, ANSYS automatically drops midside nodes at the interface. This, in fact, occurs when meshing any quadratic element if linear elements are adjacent in a neighboring volume.

7.3.10 Converting Degenerate Tetrahedral Elements to Their Non-degenerate Forms

7.3.10.1 Benefits of Converting Degenerate Tetrahedral Elements

For example, if you are working on a structural application, you are limited to using SOLID95 elements wherever transitional pyramid elements are required. Solving an analysis that involves 20-node, degenerate SOLID95 elements (and storing those elements) uses more solution time and memory than would the same analysis using SOLID92 elements. (SOLID92 elements are the 10-node, non-degenerate counterpart to SOLID95 elements.)

In this example, converting SOLID95 elements to SOLID92 elements provides these benefits:

• Less random access memory (RAM) is required per element.
• When you are not using the Pre-conditioned Conjugate Gradient (PCG) equation solver, the files that ANSYS writes during solution are considerably smaller.
• Even when you are using the PCG equation solver, you gain a modest speed advantage.

7.3.10.2 Performing a Conversion

Command(s):

TCHG,ELEM1,ELEM2,ETYPE2

Main Menu>Preprocessor>-Meshing-Modify Mesh>Change Tets

Regardless of whether you use the command or the GUI method, you are limited to converting the combinations of elements that are presented in Table 7-3.

Table 7-3 Allowable combinations of ELEM1 and ELEM2

Physical Properties	Value of ELEM1	Value of ELEM2
Structural Solid	SOLID95 or 95	SOLID92 or 92
Thermal Solid	SOLID90 or 90	SOLID87 or 87
Electrostatic Solid	SOLID122 or 122	SOLID123 or 123

If you are using the TCHG command to perform the conversion, specify values for the following arguments:

• Use the ELEM1 argument to identify the type of element that you want to convert. For example, to convert SOLID95 elements, you must specify either SOLID95 or 95 for the value of ELEM1.
• Use the ELEM2 argument to identify the type of element that is the counterpart to the ELEM1 element. For example, to convert SOLID95 elements, you must specify either SOLID92 or 92 for the value of ELEM2.


• Optionally, you can use the ETYPE2 argument to specify the element TYPE number for ELEM2. To continue with our example, to assign element TYPE number 2 to the newly-converted SOLID92 elements, specify 2 for the value of ETYPE2.

Also see the description of the TCHG command in the ANSYS Commands Reference.

If you are using the ANSYS GUI to perform the conversion, follow these steps:

1. Choose menu path Main Menu>Preprocessor>-Meshing-Modify Mesh> Change Tets. The Change Selected Degenerate Hexes to Non-degenerate Tets dialog box appears.

2. Using the Change From option menu, select a combination of elements.

3. In the TYPE number for ELEM2 field, select the appropriate element TYPE number for ELEM2. (A single-selection list containing all of the currently defined element types, along with their corresponding element TYPE numbers, appears on the dialog box to help you make your selection.) To make your selection, you can do any one of the following:

• Choose NEXT AVAIL TYPE# from the selection list and click on OK, and ANSYS uses the next available location in the element attribute tables to determine the element TYPE number for ELEM2 or, if ELEM2 already appears in the element attribute tables, ANSYS uses ELEM2's existing element TYPE number for ETYPE2.
• Choose USER SPECIFIED from the selection list and click on OK. A second dialog box appears, where you must enter an element TYPE number and click on OK. ANSYS assigns the element TYPE number that you enter to ELEM2.
• Choose a valid element TYPE number (if one is available) from the selection list. Remember that even though all of the currently defined element types and their assigned element TYPE numbers appear in the list, not all of them are valid choices (for example, if you are converting SOLID95 elements to SOLID92 elements, you must choose the TYPE number for the defined SOLID92 element from the selection list). If no SOLID92 elements are currently defined, then you have to use one of the other selection methods described above. Assuming that a valid element TYPE number is available and you select it, ANSYS will assign that TYPE number to the newly-converted elements.

7.3.10.3 Other Characteristics of Degenerate Tetrahedral Element Conversions

• As a result of the conversion operation, only selected elements of type ELEM1 are converted to type ELEM2. ANSYS ignores any elements that are type ELEM1 but are not degenerate tetrahedra; for instance, ANSYS will ignore SOLID95 elements that have a hexahedral, pyramidal, or prism shape. For example, assume that you have a simple model that contains only SOLID95 elements. Some of these elements are hexahedral, some are tetrahedral, and some are pyramidal. If you issue the command TCHG,95,92,2, ANSYS converts only the tetrahedral SOLID95 elements to SOLID92 elements; it leaves the hexahedral and pyramidal SOLID95 elements untouched. Since you specified 2 as the value of ETYPE2, ANSYS assigns element TYPE number 2 to the SOLID92 elements.
• Performing a conversion is likely to create circumstances in which more than one element type is defined for a single volume. Currently, ANSYS has no way of storing more than one element type per volume. This limitation may result in incorrect information when you perform a volume listing operation [VLIST command]. The output listing will fail to indicate that the element type of the converted elements has changed. Instead, it will indicate the element TYPE number that was originally assigned to those elements. (On the other hand, the output of an element listing operation [ELIST command] will indicate the new element TYPE number.) If you plan to perform a conversion, we recommend that the conversion be your last step in the modeling and meshing process; that is, complete any desired mesh refinement, moving or copying of nodes and elements, and any other desired modeling and meshing revision processes prior to beginning the conversion.

7.3.11 Doing Layer Meshing

• Uniform (or moderately varying) element size along the line.
• Steep transitions in element size and number in the direction normal to the line.

7.3.12 Setting Layer Meshing Controls via the GUI

• The desired element size on the line, either by setting the element size directly (SIZE), or by setting the number of line divisions (NDIV).
• The line spacing ratio (SPACE, normally 1.0 for layer meshing).
• The thickness of the inner mesh layer (LAYER1). Elements in this layer will be uniformly-sized, with edge lengths equal to the specified element size on the line. LAYER1's thickness may be specified with either a factor on the element size for the line (size factor = 2 produces two rows of uniformly-sized elements along the line; size factor = 3, three rows, etc.), or with an absolute length.
• The thickness of the outer mesh layer (LAYER2). The size of elements in this layer will gradually increase from those in LAYER1 to the global element size. LAYER2's thickness may be specified with either a mesh transition factor (transition factor = 2 produces elements which approximately double in size as the mesh front progresses normal to the line; transition factor = 3, triple in size, etc.), or with an absolute length.

Note-LAYER2's "thickness" is really the distance over which mesh transition must occur between elements of LAYER1 size and the global size. Appropriate values for LAYER2 thus depend on the magnitude of the global-to-LAYER1 size ratio. If you use a mesh transition factor to specify LAYER2, it must be greater than 1.0 (implying the next row's size must be larger than the previous) and, for best results, should be less than 4.0.

Note-For a picked set of lines, layer mesh controls may be set or cleared without altering the existing line divisions or spacing ratio settings for those lines. In fact, within this dialog box, blank or zero settings for SIZE/NDIV, SPACE, LAYER1, or LAYER2 will remain the same (that is, they will not be set to zero or default values).

The figures below illustrate a layered mesh.

Figure 7-14 Line-graded layer mesh showing uniform element size along the line and steep transitions in element size and number normal to the line

To delete layer mesh control specifications from a picked set of lines, choose the Clear button beside "Layer" on the MeshTool. Existing line divisions and spacing ratios for the set of lines will remain the same.

7.3.13 Setting Layer Meshing Controls via Commands

7.3.14 Listing Layer Mesh Specifications on Lines

Command(s):

LLIST

Utility Menu>List>Lines

7.4 Controls Used for Free and Mapped Meshing

7.4.1 Free Meshing

The element shapes used will depend on whether you are meshing areas or volumes. For area meshing, a free mesh can consist of only quadrilateral elements, only triangular elements, or a mixture of the two. For volume meshing, a free mesh is usually restricted to tetrahedral elements. Pyramid-shaped elements may also be introduced into the tetrahedral mesh for transitioning purposes. (See Section 7.3.9 for information about pyramid-shaped elements.)

If your chosen element type is strictly triangular or tetrahedral (for example, PLANE2 and SOLID92), the program will use only that shape during meshing. However, if the chosen element type allows more than one shape (for example, PLANE82 or SOLID95), you can specify which shape (or shapes) to use by one of the following methods:

Command(s):

MSHAPE

Main Menu>Preprocessor>-Meshing-Mesher Opts

You must also specify that free meshing should be used to mesh the model:

Command(s):

MSHKEY,0

Main Menu>Preprocessor>-Meshing-Mesher Opts

For area elements that support more than one shape, a mixed shape mesh (which is usually quad-dominant) will be produced by default. An all triangle mesh can be requested [MSHAPE,1,2D and MSHKEY,0], but is not recommended if lower-order elements are being used.

Note-There may be times when it is important to you to have an all-quadrilateral mesh. Free meshing of an area results in an all-quadrilateral mesh when the total number of line divisions on the boundaries of the area is even, and the quality of the quadrilateral elements produces no errors. You can increase the chances that the area's boundaries will have an even total number of line divisions by turning SmartSizing on and letting it determine the appropriate element divisions (rather than setting the number of element divisions on any of the boundaries manually [LESIZE]). You should also make sure that quadrilateral splitting is off [MOPT,SPLIT,OFF] to keep ANSYS from splitting poorly shaped quadrilateral elements into triangles. (Quadrilateral splitting is turned on for error elements by default. See the description of the MOPT command for details.)

To achieve a free volume mesh, you should choose an element type that allows only a tetrahedral shape, or use an element that supports multiple shapes and set the shape option to tetrahedral only [MSHAPE,1,3D and MSHKEY,0].

For free meshing operations, element sizes are produced based on the current settings of the DESIZE command, along with ESIZE, KESIZE, and LESIZE. If SmartSizing is turned on, the element sizes will be determined by the SMRTSIZE command along with ESIZE, KESIZE, and LESIZE. (SmartSizing is recommended for free meshing.) You can find all of these meshing controls under both Main Menu>Preprocessor>MeshTool and Main Menu>Preprocessor> -Meshing-Size Cntrls.

7.4.1.1 Fan Type Meshing and the TARGE170 Element

Figure 7-15 Example of fan type meshing

Conditions for Fan Type Meshing

• You must be meshing a three-sided area. Two of the sides must have only one element division; the third side can have any number of divisions.
• You must be meshing with the TARGE170 element.
• You must specify that free meshing be used [MSHKEY,0 or MSHKEY,2].

7.4.2 Mapped Meshing

For mapped meshing, element sizes are produced based on the current settings of DESIZE, along with ESIZE, KESIZE, and LESIZE settings (Main Menu> Preprocessor>-Meshing-Size Cntrls>-ManualSize-option). SmartSizing [SMRTSIZE] cannot be used for mapped meshing.

Note-Mapped meshing is not supported when hard points are used.

7.4.2.1 Area Mapped Meshing

Note-Mapped triangle meshing refers to the process in which ANSYS takes a map-meshable area and meshes it with triangular elements, based on a pattern you specify. This type of meshing is particularly useful for analyses that involve the meshing of rigid contact elements. (See Chapter 9 of the ANSYS Structural Analysis Guide for details about contact analyses.)

For an area to accept a mapped mesh, the following conditions must be satisfied:

a. The area must be bounded by either three or four lines (with or without concatenation).

b. The area must have equal numbers of element divisions specified on opposite sides, or have divisions matching one of the transition mesh patterns (see Figure 7-22).

c. If the area is bounded by three lines, the number of element divisions must be even and equal on all sides.

d. The meshing key must be set to mapped [MSHKEY,1]. This setting results in a mapped mesh of either all quadrilateral elements or all triangle elements, depending on the current element type and/or the setting of the element shape key [MSHAPE].

e. If your goal is a mapped triangle mesh, you can also specify the pattern ANSYS uses to create the mesh of triangular elements [MSHPATTERN]. If you do not specify a pattern, ANSYS chooses one for you. See the MSHPATTERN command description in the ANSYS Commands Reference for an illustration of the available patterns.

Figure 7-16 shows a basic area mapped mesh of all quadrilateral elements, and a basic area mapped mesh of all triangular elements.

Figure 7-16 Area mapped meshes

If an area is bounded by more than four lines, it cannot be map meshed. However, some of the lines can be combined or "concatenated" to reduce the total number of lines to four. Line concatenation is discussed later in this section.

A suggested alternative to using line concatenation is to use the AMAP command to map mesh an area by picking three or four corners of the area. This method internally concatenates all lines between the keypoints. (Simplified area mapped meshing is described later in this section.)

Line Divisions for Mapped Meshing

The same hierarchy that applied to LESIZE, ESIZE, etc. will also apply to transferred line divisions. Thus, in the example shown in Figure 7-17, LESIZE line divisions transferred from line 1 to line 3 will override explicitly defined ESIZE line divisions.

Figure 7-17 Transferred LESIZE controls override ESIZE controls

MSHKEY,1	! mapped mesh
ESIZE,,10	! 10 divisions set by ESIZE
LESIZE,1,,,20	! 20 divisions specified for line 1
AMESH,1	! 20 line divisions will be transferred onto line 3

Line Concatenation

To concatenate lines:

Command(s):

LCCAT

Main Menu>Preprocessor>-Meshing-Mesh>-Areas-Mapped> -Concatenate-Lines

Note-The LCCAT command is not supported for models that you import using the IGES default function [IOPTN,IGES,DEFAULT]. However, you can use the LNMERGE command to concatenate lines in models imported from CAD files.

To combine lines:

Command(s):

LCOMB

Main Menu>Preprocessor>-Modeling-Operate>-Booleans-Add>Lines

Consider the example of Figure 7-18, in which an area is bounded by six lines. Two of the lines can be combined, and two others concatenated, to produce an area bounded by four lines, suitable for mapped meshing.

Figure 7-18 Line combination and concatenation can enable mapped meshing

A node will be generated wherever there is a keypoint attached to a line, area, or volume. Therefore, a concatenated line will have at least as many divisions as are defined implicitly by the keypoints on that line. The program will not allow you to transfer a smaller number of divisions onto such a line. Also, if a global element size [ESIZE] is specified, it applies to your original lines, not to your concatenated lines.

Figure 7-19 ESIZE applies to original (not concatenated) lines

Line divisions cannot be directly assigned to concatenated lines. However, divisions can be assigned to combined lines [LCOMB]. Therefore, there is some advantage to using line combination instead of concatenation.

Simplified Area Mapped Meshing

Consider the example presented earlier for concatenation, but now meshed with the AMAP method. Notice that there are multiple lines between several of the picked keypoints. After picking the area, keypoints 1, 3, 4, and 6 can be picked in any order, and the mapped mesh is automatically created.

Figure 7-20 Simplified mapped meshing (AMAP)

No line concatenation is needed prior to the AMAP operation; the concatenation is done internally and then deleted. The area's line list is left unchanged.

Note-The AMAP command is not supported for models that you import using the IGES default import function [IOPTN,IGES,DEFAULT].

Transition Mapped Quadrilateral Meshing

Figure 7-21 Examples of transition mapped quadrilateral meshes

To achieve a transition mapped quadrilateral mesh, you must use an element type that supports a quadrilateral shape, set the meshing key to mapped [MSHKEY,1], and set the shape specification to allow quadrilaterals [MSHAPE,0,2D]. (If you want a transition mapped triangle mesh, see the next section.) In addition, specified line divisions must match one of the patterns shown in Figure 7-22.

Figure 7-22 Applicable transition patterns-transition mapped quadrilateral meshes

The quad-dominant free mesher [MSHAPE,0 and MSHKEY,0] automatically looks for four-sided regions that match these transition patterns. If a match is found, the area is meshed with a transition mapped quadrilateral mesh, unless the resulting elements are of poor quality (in which case a free mesh will be produced).

Transition Mapped Triangle Meshing

Figure 7-23 (b) illustrates a transition mapped triangle mesh. When you request a mapped triangle mesh, ANSYS actually begins by map meshing the area with quadrilateral elements, and then it automatically splits the quadrilateral elements into triangles. Figure 7-23 (a) shows the quadrilateral mesh that was used as the basis for the triangle mesh shown in Figure 7-23 (b). Figure 7-23 (c) illustrates the triangle mesh, with the quadrilateral elements superimposed over it. The dotted lines represent the boundaries of the quadrilateral elements that ANSYS split into triangles.

Figure 7-23 Relationship between a transition mapped quadrilateral mesh and a transition mapped triangle mesh

7.4.2.2 Volume Mapped Meshing

a. The volume must take the shape of a brick (bounded by six areas), wedge or prism (five areas), or tetrahedron (four areas).

b. The volume must have equal numbers of element divisions specified on opposite sides, or have divisions matching one of the transition mesh patterns for hexahedral meshes. See Figure 7-24 for examples of element divisions that will produce a mapped mesh for different volume shapes. Transition mesh patterns for hexahedral meshes are described later in this section.

c. The number of element divisions on triangular areas must be even if the volume is a prism or tetrahedron.

Figure 7-24 Examples of element divisions for mapped volume meshing

Area Concatenation

! first, concatenate areas for mapped volume meshing:
ACCAT,...
! next, concatenate lines for mapped meshing of bounding areas:
LCCAT,...
LCCAT,...
VMESH,...

As shown in the sample input listing above, line concatenations [LCCAT] are normally required after area concatenations [ACCAT]. However, if both areas that are concatenated are bounded by four lines (no concatenated lines), the line concatenation operations will be done automatically. Thus, because the areas in Figure 7-25 are both bounded by four lines, line concatenation [LCCAT] is not required. Also note that deleting the concatenated area does not automatically delete the associated concatenated lines.

Figure 7-25 Area concatenation used for mapped volume meshing. The lines are automatically concatenated by the area concatenation operation [ACCAT] because both areas are bounded by four lines.

To concatenate areas, use one of the following methods:

Command(s):

ACCAT

Main Menu>Preprocessor>Concatenate>Areas

Main Menu>Preprocessor>Mesh>Mapped>Areas

Note-The ACCAT command is not supported for models that you import using the IGES default import function [IOPTN,IGES,DEFAULT]. However, you can use the ARMERGE command to merge two or more areas in models imported from CAD files. Be aware that when you use the ARMERGE command in this way, locations of deleted keypoints between combined lines are unlikely to have nodes on them!

To add areas, use one of the following methods:

Command(s):

AADD

Main Menu>Preprocessor>-Modeling-Operate>-Booleans-Add> Areas

Please see the ACCAT, LCCAT, and VMESH command descriptions for more information.

Transition Mapped Hexahedral Meshing

Figure 7-26 Examples of transition mapped hexahedral meshes

To achieve a transition mapped hexahedral mesh, you must use an element type that supports a hexahedral shape. If you previously set the element shape specification to mesh with tetrahedral-shaped elements [MSHAPE,1,3D], you must now set the shape specification to allow hexahedron [MSHAPE,0,3D]. In addition, specified line divisions must match one of the patterns shown in Figure 7-27.

Note-Even if you specify free meshing [MSHKEY,0], ANSYS automatically looks for six-sided volumes that match these transition patterns. If a match is found, the volume will be meshed with a transition mapped hexahedral mesh, unless the resulting elements are of poor quality (in which case the mesh will fail).

Note-As indicated in Figure 7-27, some of the edges of the volumes are hidden (edges N5, N9, and N10). Edge N5 is opposite edge N8; edge N9 is opposite edge N1; and edge N10 is opposite edge N2.

Figure 7-27 Applicable transition patterns-transition mapped hexahedral meshes

7.4.2.3 Some Notes about Concatenated Lines and Areas

You can readily "undo" a concatenation by simply deleting the line or area produced by the concatenation:

• The fastest way to delete concatenated lines or areas is by choosing menu path Main Menu>Preprocessor>-Modeling-Delete>-Del Concats -Lines or Main Menu>Preprocessor>-Modeling-Delete>-Del Concats -Areas.

Warning: When you use this method, ANSYS automatically selects all concatenated lines (or areas) and deletes them without prompting you.

• If you want more control over which concatenated lines or areas are selected and deleted, use one of these methods:

LSEL,Type,LCCA,,,,,KSWP or ASEL,Type,ACCA,,,,,KSWP

Utility Menu>Select>Entities

If you are using the Select Entities dialog box, choose both Lines and Concatenated to select concatenated lines. Choose both Areas and Concatenated to select concatenated areas. If desired, use the other controls in the dialog box to refine your selection.

You can then delete all of the selected lines or areas [LDELE,ALL or ADELE,ALL] as necessary.

Figure 7-28 Input lines in a concatenation become "detached" until the concatenation is undone

If you find that concatenation becomes too restrictive for your intended modeling operations, you can usually obtain a mapped mesh by some other means, such as by subdividing an area or volume into appropriately-bounded entities. Boolean operations will often be helpful for subdividing an entity in this fashion.

See the descriptions of the ASEL, LSEL, ACCAT, LCCAT, ADELE, and LDELE commands in the ANSYS Commands Reference for details.

7.5 Meshing Your Solid Model

Command(s):

SAVE

Utility Menu>File>Save as Jobname.db

You may also want to turn on the "mesh accept/reject" prompt by picking Main Menu>Preprocessor>-Meshing-Mesher Opts. This feature, which is available only through the GUI, allows you to easily discard an undesirable mesh. (For more information, see Section 7.6.)

7.5.1 Generating the Mesh Using xMESH Commands

• To generate point elements (such as MASS21) at keypoints:

KMESH

Main Menu>Preprocessor>-Meshing-Mesh>Keypoints

• To generate line elements (such as LINK31) on lines:

LMESH

Main Menu>Preprocessor>-Meshing-Mesh>Lines

Also see Section 7.5.2 for information about special beam meshing procedures.

• To generate area elements (such as PLANE82) on areas:

AMESH, AMAP

Main Menu>Preprocessor>-Meshing-Mesh>-Areas-Mapped>
3 or 4 sided
Main Menu>Preprocessor>-Meshing-Mesh>-Areas-Free
Main Menu>Preprocessor>-Meshing-Mesh>-Areas-Target Surf
Main Menu>Preprocessor>-Meshing-Mesh>-Areas-Mapped>
By Corners

• To generate volume elements (such as SOLID90) in volumes:

VMESH

Main Menu>Preprocessor>-Meshing-Mesh>-Volumes-Mapped>
4 to 6 sided
Main Menu>Preprocessor>-Meshing-Mesh>-Volumes-Free

Also see Section 7.5.3 and Section 7.5.5 for information about special volume meshing procedures.

7.5.2 Generating a Beam Mesh With Orientation Nodes

To assign orientation keypoints as attributes of a line:

Command(s):

LATT

Main Menu>Preprocessor>-Attributes-Define>All Lines
Main Menu>Preprocessor>-Attributes-Define>Picked Lines

7.5.2.1 How ANSYS Determines the Location of Orientation Nodes

Note-Although this discussion refers to them as "orientation nodes," elsewhere you may see this type of node referred to as an off-node, third node (for linear beam elements only), or fourth node (for quadratic beam elements only).

7.5.2.2 Benefits of Beam Meshing With Orientation Nodes

If your analysis uses BEAM188 or BEAM189 elements, you can use the ANSYS program's cross section data definition, analysis, and visualization capabilities for these elements. You can assign a section ID number as an attribute of a line [LATT]. The section ID number identifies the cross section used by the beam elements that will be generated when you mesh the line. The orientation nodes, which ANSYS automatically generates based on orientation keypoints that you specify [LATT], determine the section orientations for the beam elements. For detailed information about beam analysis and cross sections, see Chapter 8 of the ANSYS Advanced Analysis Techniques Guide.

7.5.2.3 Generating a Beam Mesh With Orientation Nodes

If you are using the command method to generate the beam mesh, include these commands in your input:

1. Use the LSEL command to select the lines that you want to mesh with orientation nodes.

2. Use the LATT command to associate element attributes with the selected, unmeshed line(s). Specify values for the MAT, REAL, TYPE, ESYS, KB, KE, and SECNUM arguments.

• When specifying a value for the TYPE argument on the LATT command, be sure that the element type you assign to the line is one that supports beam meshing with orientation. Currently, this list includes BEAM4, BEAM24, BEAM44, BEAM161, BEAM188, and BEAM189.
• Use the KB and KE arguments on the LATT command to assign beginning and ending orientation keypoints. If you are meshing with BEAM24, BEAM161, BEAM188, or BEAM189 elements, you are required to define at least one orientation keypoint when you set your attributes for meshing. When ANSYS generates the mesh [LMESH], each beam element along the line will have two end nodes and one orientation node. Specifying orientation keypoints when meshing with BEAM4 and BEAM44 elements is optional. If you specify orientation keypoints for these elements, each beam element along the meshed line will have two end nodes and one orientation node. If you do not specify orientation keypoints for BEAM4 and BEAM44, each beam element will have two end nodes, but no orientation node (that is, ANSYS will generate the mesh using standard line meshing).
• If you are using BEAM188 elements or BEAM189 elements, use the SECNUM argument on the LATT command to assign a section ID number.

See Section 7.5.2.4 for examples that illustrate various ways of assigning orientation keypoints. See Chapter 8 of the ANSYS Advanced Analysis Techniques Guide for details about cross sections.

4. Use the LMESH command to mesh the line(s).

5. After meshing a beam, always use the /ESHAPE,1 command to verify the beam's orientation graphically.

6. You can use the LLIST,,,,ORIENT command to list the selected line(s), along with any assigned orientation keypoints and section data.

If you are using the ANSYS GUI to generate the beam mesh, follow these steps:

1. Choose menu path Main Menu>Preprocessor>MeshTool. The MeshTool appears.

2. In the Element Attributes section of the MeshTool, select Lines from the option menu on the left and then click on Set. The Line Attributes picker appears.

3. In the ANSYS Graphics window, click the line(s) to which you want to assign attributes (including orientation keypoints) and then click on OK in the Line Attributes picker. The Line Attributes dialog box appears.

4. In the Line Attributes dialog box, assign MAT, REAL, TYPE, ESYS, and/or SECT attributes as desired, click the Pick Orientation Keypoint(s) option so that Yes appears, and click on OK. The Line Attributes picker reappears.

5. In the ANSYS Graphics window, pick the orientation keypoint(s) and then click on OK in the Line Attributes picker.

6. Back in the MeshTool, set any desired element size controls. Then initiate the line mesh operation by choosing Lines from the Mesh option menu and clicking on MESH. The Mesh Lines picker appears.

7. In the ANSYS Graphics window, pick the line(s) that you want to mesh and then click on OK in the Mesh Lines picker. ANSYS meshes the beam.

8. After the beam is meshed, always verify the beam's orientation graphically. Choose menu path Utility Menu>PlotCtrls>Style>Size and Shape. Click the /ESHAPE option to turn it on and click on OK. The meshed beam appears.

9. You can list the selected line(s), along with any defined orientation keypoints and section data. To do so, choose menu path Utility Menu>List>Lines. The LLIST Listing Format dialog box appears. Choose Orientation KP and then click on OK.

7.5.2.4 Examples of Beam Meshing With Orientation Nodes

Figure 7-29 shows three examples. For each example, a beginning orientation keypoint and an ending orientation keypoint have been defined at the same location. The examples illustrate how you can assign different orientation keypoints to align selected beam sections within a structure in different directions.

Figure 7-29 Placement of orientation keypoints and element orientation

If you specify one orientation keypoint for a line, ANSYS generates beam elements along the line with a constant orientation. If you specify different orientation keypoints at each end of the line, ANSYS generates a pre-twisted beam.

Figure 7-30 illustrates some differences between beam meshing with constant orientation as opposed to beam meshing with pre-twist.

• In Figure 7-30 (a), only a beginning orientation keypoint was assigned. The keypoint is 0° from the y axis at a distance of 10 units in the y direction. The beam exhibits constant orientation.
• In Figure 7-30 (b), only a beginning orientation keypoint was assigned. The keypoint is 30° from the y axis at a radius of 10 units. The beam exhibits constant orientation.
• In Figure 7-30 (c), both a beginning and an ending orientation keypoint were assigned. The keypoints are 90° apart, causing a 90° twist in the beam. Due to the linear interpolation that is used to determine the location of the orientation nodes, a line biasing with small divisions at each end was used to cause the nodes to be located closer to the vectors made by the keypoints.
• In Figure 7-30 (d), the orientation keypoints are 180° apart, and this time the beam flips. Assigning these keypoints causes a discontinuity because the interpolation of the two vectors is linear.
• Figure 7-30 (e) provides a remedy to the problem illustrated in Figure 7-30 (d). Here one line was divided into two, with the ending orientation keypoint for L1 and the beginning orientation keypoint for L2 being assigned to the same keypoint. A 180° twist is achieved.

7.5.2.5 Other Considerations for Beam Meshing With Orientation Nodes

• Caution: If you issue the CDWRITE command after generating a beam mesh with orientation nodes, the database file will contain all of the nodes for every beam element, including the orientation nodes. However, the orientation keypoints that were specified for the line [LATT] are no longer associated with the line and are not written out to the geometry file. The line does not recognize that orientation keypoints were ever assigned to it, and the orientation keypoints do not "know" that they are orientation keypoints. Thus, the CDWRITE command does not support (for beam meshing) any operation that relies on solid model associativity. For example, meshing the areas adjacent to the meshed line, plotting the line that contains orientation nodes, or clearing the line that contains orientation nodes may not work as expected. This limitation also exists for the IGESOUT command. See the descriptions of the CDWRITE command and the IGESOUT command in the ANSYS Commands Reference for more information.
• Since orientation is not required for 2-D beam elements, the beam meshing procedure described in this section does not support 2-D beam elements.
• Any operation on a line (copying the line, moving the line, and so on) will destroy the keypoint attributes.
• If an orientation keypoint is deleted, ANSYS issues a warning message.
• If an orientation keypoint is moved, it remains an orientation keypoint. However, if an orientation keypoint is redefined (K,NPT,X,Y,Z), ANSYS no longer recognizes it as an orientation keypoint.

7.5.3 Generating a Volume Mesh From Facets

Command(s):

FVMESH

Main Menu>Preprocessor>-Meshing-Mesh>-Tet Mesh From-Area Elements

Note-The main tetrahedra mesher [MOPT,VMESH,MAIN] is the only tetrahedra mesher that supports the generation of a volume mesh from facets; the alternate tetrahedra mesher [MOPT,VMESH,ALTERNATE] does not.

Note-The FVMESH command and its corresponding menu path do not support multiple "volumes." If you have multiple volumes in your model, select the surface elements for one "volume," while making sure that the surface elements for the other volumes are deselected. Then use FVMESH to generate a mesh for the first volume. Continue this procedure by selecting one volume at a time and meshing it, until all of the volumes in the model have been meshed.

7.5.4 Additional Considerations for Using xMESH Commands

• Sometimes you may need to mesh the solid model with a variety of elements of different dimensionalities. For example, you may need to "reinforce" a shell model (area elements) with beams (line elements), or overlay one of the faces of a 3-D solid model (volume elements) with surface effect (area) elements. You can do so by using the appropriate meshing operations [KMESH, LMESH, AMESH, and VMESH] in any desired order. Make sure, however, that you set the appropriate element attributes (discussed earlier in this chapter) before meshing.
• No matter which volume mesher you choose [MOPT,VMESH,Value], it may produce different meshes on different hardware platforms when meshing volumes with tetrahedral elements [VMESH, FVMESH]. Therefore, you should be cautious when evaluating results at a specific node or element. The location of these entities may change if the input created on one platform is later run on a different platform.
• The adaptive meshing macro [ADAPT] is an alternative meshing method that automatically refines the mesh based on mesh discretization errors. See Chapter 3 of the ANSYS Advanced Analysis Techniques Guide for more information on this feature.

7.5.5 Generating a Volume Mesh By Sweeping

7.5.5.1 Benefits of Volume Sweeping

• Unlike other methods for extruding a meshed area into a meshed volume [VROTAT, VEXT, VOFFST, and VDRAG commands], volume sweeping [VSWEEP] is intended for use in existing unmeshed volumes. Thus it is particularly useful in these situations:
  • You have imported a solid model that was created in another program, and you want to mesh it in ANSYS.
  • You want to create a hexahedral mesh for an irregular volume. You now only have to break up the volume into a series of discrete sweepable regions, as opposed to in the past, when it was necessary for you to break up the volume into discrete map-meshable regions.
  • You either want to create a different mesh than the one that was created by one of the other extrusion methods, or you forgot to create a mesh during one of those operations.
• Volume sweeping allows you to use any area elements to mesh the source area. The other extrusion methods mentioned above require the initial area mesh to be a mesh of shell elements.
• If you do not mesh the source area prior to volume sweeping, ANSYS meshes it for you when you invoke the volume sweeper. The other extrusion methods require you to mesh the area yourself before you invoke them. If you do not, the other extrusion methods create the volume, but no area or volume mesh is generated.

7.5.5.2 What to Do Before You Sweep a Volume

1. Determine whether the volume's topology can be swept. The volume cannot be swept if any of these statements is true:

• One or more of the volume's side areas contains more than one loop; in other words, there is a hole in a side area.
• The volume contains more than one shell; in other words, there is an internal void within the volume. (A shell is the volumetric equivalent of an area loop-a set of entities that defines a continuous closed boundary. The SHELL column in a volume listing [VLIST] indicates the number of shells in the volume.)
• The source area and the target area are not opposite one another in the volume's topology. (By definition, the target area must be opposite the source area.)

Note-Even if you have satisfied these requirements, there may be times when the shape of a volume causes the volume sweeper to create poorly shaped elements. For help, see Section 7.5.5.4.

3. Determine how you want to control the number of element layers that will be created during the sweeping operation; that is, the number of elements that will be created along the length of the sweep direction (see Figure 7-31). You can use any of these methods to control this number:

• Use the EXTOPT,ESIZE,Val1,Val2 command to specify the number of element divisions (and if desired, the spacing ratio or bias) to be used along the volume's side lines (where Val1 is the number of element divisions and Val2 is the bias). Note that the number of element divisions and bias that you specify with EXTOPT will apply to all of the volume's unmeshed side lines. For any side line that has been pre-meshed or that has other sizing specifications associated with it (via LESIZE), the values set by EXTOPT are ignored. Using the EXTOPT command or its menu path is the preferred method for setting these values.

EXTOPT,ESIZE,Val1,Val2

Main Menu>Preprocessor>-Meshing-Mesh>-Volume Sweep-Sweep Opts

• On one or more of the volume's side lines, use the LESIZE command to specify the number of element divisions for that particular line. This method also permits you to specify a bias that the volume sweeper will honor [LESIZE,,,,,SPACE]; however, the bias applies only to the line that you identify on the LESIZE command. Regardless of how element divisions are set for all of the other side lines (for example, through pre-meshing or additional LESIZE specifications), all of the volume's side lines must have the same number of element divisions.
• Generate a mapped mesh on one of the side areas or within a volume or area that is adjacent to a side area or side line.
• Generate a mesh of beam elements on one of the side lines [LMESH].

4. Determine which of the areas bounding the volume will be the source area, and which will be the target area. ANSYS uses the pattern of the area elements on the source area (which can be quadrilateral and/or triangular elements) to fill the volume with hexahedral and/or wedge elements. (If you have not pre-meshed the area prior to volume sweeping, ANSYS automatically generates "temporary" area elements. It does not save these area elements in the database; they are discarded as soon as the pattern for the swept volume is determined.) The target area is simply the area that is opposite the source area. See Figure 7-31 above, which illustrates one way that a user might set the element divisions, source area, and target area for a volume sweeping operation.

Note-In some cases, your choice of source and target areas will determine whether the sweeping operation succeeds or fails. See Section 7.5.5.4 for details.

The results of a volume sweeping operation will differ depending on whether you have meshed any of the areas (source, target, and/or side areas) in your model prior to sweeping.

Typically, you will generate a mesh for the source area yourself, before you sweep the volume. If you have not meshed the source area, ANSYS will mesh it internally when you invoke the volume sweeping operation (as described above in Step 4.

Consider the following information when deciding whether to "pre-mesh" before sweeping:

• If you want the source area to be meshed with a mapped quadrilateral mesh or a mapped triangle mesh, pre-mesh.
• If you want the source area to be meshed with smart element sizing [SMRTSIZE], pre-mesh.
• If you do not pre-mesh, ANSYS always uses the free mesher to generate the mesh. (On simple areas, the free mesh that ANSYS generates may be identical to the mapped mesh it would have generated using the mapped mesher, but this is not guaranteed.)
• If you do not pre-mesh, ANSYS uses the element shape setting [MSHAPE] to determine the element shape it uses to mesh the source area (MSHAPE,0,2D results in quadrilateral elements; MSHAPE,1,2D results in triangular elements).
• The sweeping operation will fail if hard points are present on an area or line that is associated with the volume, unless you pre-mesh the area or line containing the hard point.
• If you pre-mesh both the source area and the target area, the area meshes must match. However, the source area mesh and the target area mesh do not have to be mapped meshes.
• Prior to sweeping, all of the volume's side areas must be either map meshed or 4-sided. (There is an exception to this rule: You must always pre-mesh-with a mapped mesh-any 4-sided area that started out with more than 4 sides and then became 4-sided as a result of line concatenation.) In addition, one line of each unmeshed side area must be on the source area, and one line must be on the target area.

• The sweeping operation will succeed when the topology of the source area is different from the topology of the target area, as long as you pre-mesh (with a mapped mesh) those side areas of the volume that are causing the topology of the source area and the target area to differ. See Figure 7-32 for an example.

See Section 7.5.5.5 for more information about the characteristics of the volume sweeping feature.

Figure 7-33 Sweeping adjacent volumes in different directions

7.5.5.3 Invoking the Volume Sweeper

Command(s):

VSWEEP,VNUM,SRCA,TRGA,LSMO

Main Menu>Preprocessor>-Meshing-Mesh>-Volume Sweep-Sweep

If you are using the VSWEEP command to sweep a volume, specify values for the following arguments:

• Use the VNUM argument to identify the volume that you want to sweep.
• Use the SRCA argument to identify the source area.
• Use the TRGA argument to identify the target area.
• Optionally, use the LSMO argument to specify whether ANSYS should perform line smoothing during the sweeping operation.

If you are using the ANSYS GUI to sweep a volume, follow these steps:

1. Choose menu path Main Menu>Preprocessor>-Meshing-Mesh> -Volume Sweep-Sweep. The Volume Sweeping picker appears.

2. Pick the volume that you want to sweep and click on Apply.

3. Pick the source area and click on Apply.

4. Pick the target area. Click on OK to close the picker.

Note-When using the ANSYS GUI to sweep a volume, you cannot control whether line smoothing occurs. ANSYS does not perform line smoothing when volume sweeping is invoked from the GUI.

7.5.5.4 Strategies for Avoiding Shape Failures During Volume Sweeping

1. Switch the source and target areas and reinvoke the volume sweeper. For example, if you specify area A1 as your source area and area A2 as your target area, and the sweep operation fails, try again using A2 as the source area and A1 as the target area.

2. Choose an entirely different set of source and target areas and reinvoke the volume sweeper. (Some volumes can be swept in more than one direction.) For example, if area A1 and area A2 do not work, try using A5 and A6.

3. Use shape checking as a diagnostic tool to determine which region of the model is causing the sweep failure. To do this, reduce the shape checking level to warning mode [SHPP,WARN], so that elements that violate error limits result in warning messages rather than element failures. Then reinvoke the sweeping operation. Use the resulting warning messages to identify the region of the model that contains the bad elements, and then clear the bad element mesh [VCLEAR]. Turn shape checking back on [SHPP,ON]. Next, modify the region of the model that contained the bad elements. Finally, mesh the volume again with a subsequent sweep operation. Here are some suggestions for modifying the model:

• Divide the volume into two or more volumes [VSBA,VSBW], which will shorten the length of the sweep direction. Try dividing the volume near the region where the poorly shaped elements occur. Afterwards, invoke VSWEEP for each of the resulting volumes.
• If the elements flagged by SHPP,WARN appear to be stretched within thin sections of the target area as in Figure 7-34 (c), try dividing the side areas in that region along the direction of the sweep. Use these steps:

1. Clear the mesh [VCLEAR].

2. Divide one of the lines on the source area and one of the lines on the target area by adding keypoints at the desired division locations [LDIV]. See Figure 7-34 (e).

3. Copy the line divisions from the new lines on the source area to the corresponding new lines on the target area as described in Figure 7-34 (e). (The "new lines" are those that were created by Step 2.) You can copy line divisions easily via the MeshTool. Choose menu path Main Menu>Preprocessor>MeshTool. On the MeshTool, press the Copy button to open the picker. Use the picker to copy the line divisions-including spacing ratios-from one line to the other.

4. Manually map mesh the side area that was affected by Step 2. See Figure 7-34 (f).

5. Reinvoke the volume sweeper.

Figure 7-34 (c), Figure 7-34 (d), and Figure 7-34 (g) show the results of three different sweeping operations, and illustrate how you can use some of the strategies described above to affect the quality of a swept mesh. In all three cases, the user started with the same volume, which is shown in Figure 7-34 (a). Figure 7-34 (b) illustrates the source mesh that was used during the sweep. Again, in all three cases, the user generated this source mesh prior to invoking volume sweeping.

The differences in the results are due to the additional actions (if any) that the user took prior to sweeping. To get the results shown in Figure 7-34 (c), the user invoked volume sweeping without using any of the strategies described above. Notice the stretched elements that appear on the target area. For the results shown in Figure 7-34 (d), the user invoked volume sweeping with line smoothing turned on [VSWEEP,,,,1]. In this case, the element shapes are better than those shown in Figure 7-34 (c); however, they are not as good as those shown in Figure 7-34 (g). For the results in Figure 7-34 (g), the user divided lines [LDIV] on the source and target area and map meshed the affected side area prior to sweeping. Notice the significant improvement in the shape of the elements on the target area.

Figure 7-34 Strategies for avoiding stretched elements

7.5.5.5 Other Characteristics of Volume Sweeping

• The source area and the target area do not have to be flat or parallel.

• If the topology of the source area and the topology of the target area are the same, the sweeping operation will often succeed even if the shape of the source area is different from the shape of the target area. However, drastically different shapes can cause element shape failures.
• During volume sweeping, ANSYS can create either linear or quadratic elements. It can sweep quadratic area elements into linear volume elements, and it can sweep linear area elements into quadratic volume elements. (However, when ANSYS sweeps linear area elements into quadratic volume elements, mid-nodes are not added to the edges of the source area. This will result in an element shape failure if you are using quadratic volume elements that do not support dropped mid-nodes.)

• If you have pre-meshed the source, target, and/or side areas, you can issue the EXTOPT,ACLEAR,1 command prior to sweeping and ANSYS will automatically clear the area elements from any selected source, target, or side area after the swept volume mesh is created. (Note-In the GUI, choose menu path Main Menu> Preprocessor>-Meshing-Mesh> -Volume Sweep-Sweep Opts to access a dialog box where you can toggle this clearing option on and off.) The areas that you want to clear must be selected for clearing of the area meshes to occur.
• Volume sweeping does not require your model to have a constant cross section. However, if the cross section varies, it should vary linearly from one end of the sweep to the other for best results.

• During volume sweeping, ANSYS ignores any settings that are specified for the SMRTSIZE command. However, if you do not pre-mesh the source area, ANSYS will use the KESIZE, ESIZE, or DESIZE command setting (as appropriate) to mesh the source area. Also note the following information about the ESIZE command. The ESIZE,,NDIV setting may be used to determine the number of element divisions that will be created along the volume's side lines during sweeping. However, this is not the preferred method because if the source area is not pre-meshed, the number of element divisions specified by NDIV will apply to all of the source area lines as well. The preferred method is to use the EXTOPT command (as described earlier).

7.5.6 Aborting a Mesh Operation

A STOP button is located at the bottom of the status window. Picking the STOP button aborts the mesh operation and causes incomplete meshes to be discarded. Areas or volumes that are completely meshed before STOP is picked will be retained. The solid model and finite element model will be left as they were before meshing was initiated.

You will see the meshing status window only when working in GUI mode. (Status windows will appear by default, but can be turned off by issuing /UIS,ABORT,OFF.) In non-GUI mode, a mesh abort is triggered by the system "break" function (CTRL-C or CTRL-P on most systems).

Note-If a session log file (Jobname.LOG) from an interactive session that included an intentional mesh abort is used as input for another ANSYS session, the results will not likely be the same as they were for the interactive session since the abort will not be reproduced in the subsequent runs.

7.5.7 Element Shape Checking

ANSYS 5.5 detects and flags all element shape warning and error conditions at the time of element creation, before storing each element. This is in contrast to ANSYS 5.3 and earlier releases, in which much of the testing occurred just prior to solution.

Although ANSYS performs element shape checking by default, a number of options for controlling element shape checking are available. Although most of the options are described in the sections that follow, you should refer to the SHPP command description in the ANSYS Commands Reference for additional information. Use either of these methods to modify shape checking:

Command(s):

SHPP

Main Menu>Preprocessor>Checking Ctrls>Shape Checking
Main Menu>Preprocessor>Checking Ctrls>Toggle Checks

The sections that follow cover how to:

• Turn element shape checking off entirely or to warning-only mode
• Turn individual shape tests off and on
• View a summary of shape test results
• View current shape parameter limits
• Change shape parameter limits
• Retrieve element shape parameter data
• Understand the circumstances under which ANSYS retests existing elements, and why doing so is necessary
• Decide whether element shapes are acceptable

7.5.7.1 Turning Element Shape Checking Off Entirely or to Warning-Only Mode

In certain cases, it may be desirable to turn element shape checking off, or to turn it on in warning-only mode. Turning element shape checking off [SHPP,OFF,ALL] deactivates shape checking entirely. When element shape checking is turned on in warning-only mode [SHPP,WARN], shape checking occurs, but elements that violate error limits now only give warnings and do not cause either a meshing or element storage failure.

In the GUI, you can run shape checking in warning-only mode or turn it off entirely by choosing menu path Main Menu>Preprocessor>Checking Ctrls>Shape Checking. When the Shape Checking Controls dialog box appears, choose either "On w/Warning msg" or "Off"; then click on OK.

Situations in which we recommend that you turn shape checking off or run it in warning-only mode include:

• When you are generating an area mesh [AMESH], but your ultimate intention is to generate a volume mesh [VMESH] of quadratic tetrahedrons with that area as one of the volume's faces. Note that the tetrahedra mesher can fix meshes in which area elements have poor Jacobian ratios. Thus, if you are generating an area mesh for an area that will be a face on a volume in a subsequent volume meshing operation, it may make sense to turn element shape checking to warning-only mode, mesh the area, turn element shape checking on, and then mesh the volume.
• When you are importing a mesh [CDREAD]. If "bad" elements exist in a mesh that you want to import and element shape checking is turned on, ANSYS may bring the mesh into the database with "holes" where the bad elements should be (or it may not import the mesh at all). Since neither of these outcomes is desirable, you may want to turn element shape checking either off or to warning-only mode prior to importing a mesh. After you import, we suggest that you turn shape checking back on and recheck the elements [CHECK,ESEL,WARN or CHECK,ESEL,ERR].

Note-Once elements are in the database, performing element shape checking will not delete them. If any elements in violation of error limits are selected when you initiate a solution [SOLVE], ANSYS issues an error message and does not process the solution.

• When you are using direct generation and you are creating elements that you know will be temporarily invalid. For example, you may be creating a wedge-shaped element that has coincident nodes. You know that you need to merge the coincident nodes [NUMMRG] in order to get valid elements. In this case, it would make sense to turn off element shape checking, complete the desired operations (such as merging nodes in this example), turn element shape checking on, and then check the elements for completeness [CHECK].

7.5.7.2 Turning Individual Shape Tests Off and On

To use the command method to toggle the tests off and on, issue the command SHPP,Lab,VALUE1:

• Use the Lab argument to indicate whether you want to turn tests off or on. Specify OFF to turn tests off; specify ON to turn tests on.
• Use the VALUE1 argument to indicate which tests you want to turn off or on. You can specify ANGD (SHELL28 corner angle deviation tests), ASPECT (aspect ratio tests), PARAL (deviation from parallelism of opposite edges tests), MAXANG (maximum corner angle tests), JACRAT (Jacobian ratio tests), or WARP (warping factor tests). You can also specify ALL to turn all tests off or on.

In the GUI, you can toggle the tests off and on by choosing menu path Main Menu>Preprocessor>Checking Ctrls>Toggle Checks. When the Toggle Shape Checks dialog box appears, click the individual tests off or on as desired; then click on OK.

7.5.7.3 Viewing a Summary of Shape Test Results

In the GUI, you can view a summary listing by choosing menu path Main Menu>Preprocessor>Checking Ctrls>Shape Checking. When the Shape Checking Controls dialog box appears, choose "Summary" in the option menu; then click on OK.

SUMMARIZE SHAPE TESTING FOR ALL SELECTED ELEMENTS

 ------------------------------------------------------------------------------
            <<<<<<          SHAPE TESTING SUMMARY           >>>>>>
            <<<<<<        FOR ALL SELECTED ELEMENTS         >>>>>>
 ------------------------------------------------------------------------------
                    --------------------------------------
                    |  Element count       214 PLANE82   |
                    --------------------------------------

  Test                Number tested  Warning count  Error count    Warn+Err %
  ----                -------------  -------------  -----------    ----------
  Aspect Ratio                214              0             0         0.00 %
  Maximum Angle               214             59             0        27.57 %
  Jacobian Ratio              214              0             0         0.00 %

  Any                         214             59             0        27.57 %
 ------------------------------------------------------------------------------

7.5.7.4 Viewing Current Shape Parameter Limits

In the GUI, you can view a status listing by choosing menu path Main Menu> Preprocessor>Checking Ctrls>Shape Checking. When the Shape Checking Controls dialog box appears, choose "Status" in the option menu; then click on OK.

Note-As stated above, this output shows the default shape parameter limits in ANSYS. If you modify any of these limits or turn off any of the individual shape tests, your output will differ accordingly.

Note-In most cases in the output below, "FACE" also means "cross-section of solid element." For example, the ASPECT RATIO limits apply to both faces and cross-sections of tetrahedra, hexahedra (bricks), pyramids, and wedges.

 ASPECT RATIO (EXCEPT FLOTRAN OR EMAG)
    QUAD OR TRIANGLE ELEMENT OR FACE
         WARNING TOLERANCE ( 1) =   20.00000    
         ERROR TOLERANCE   ( 2) =   1000000.    
 DEVIATION FROM 90 DEGREE CORNER ANGLE
    SHELL28 SHEAR/TWIST PANEL
         WARNING TOLERANCE ( 7) =   5.000000    
         ERROR TOLERANCE   ( 8) =   30.00000    
 DEVIATION FROM PARALLEL OPPOSITE EDGES IN DEGREES    (EXCEPT FLOTRAN OR EMAG)
    QUAD ELEMENT OR FACE WITHOUT MIDSIDE NODES
         WARNING TOLERANCE (11) =   70.00000    
         ERROR TOLERANCE   (12) =   150.0000    
    QUAD OR QUAD FACE WITH MIDSIDE NODES
         WARNING TOLERANCE (13) =   100.0000    
         ERROR TOLERANCE   (14) =   170.0000    
 MAXIMUM CORNER ANGLE IN DEGREES (EXCEPT FLOTRAN OR EMAG)
    TRIANGLE ELEMENT OR FACE
         WARNING TOLERANCE (15) =   165.0000    
         ERROR TOLERANCE   (16) =   179.9000    
    QUAD ELEMENT OR FACE WITHOUT MIDSIDE NODES
         WARNING TOLERANCE (17) =   155.0000    
         ERROR TOLERANCE   (18) =   179.9000    
    QUAD ELEMENT OR FACE WITH MIDSIDE NODES
         WARNING TOLERANCE (19) =   165.0000    
         ERROR TOLERANCE   (20) =   179.9000    
 JACOBIAN RATIO
    H-METHOD ELEMENT
         WARNING TOLERANCE (31) =   30.00000    
         ERROR TOLERANCE   (32) =   1000.000    
    P-METHOD ELEMENT
         WARNING TOLERANCE (33) =   30.00000    
         ERROR TOLERANCE   (34) =   40.00000    
 QUAD ELEMENT OR FACE WARPING FACTOR
    SHELL43, SHELL143, SHELL163, SHELL181
         WARNING TOLERANCE (51) =   1.000000    
         ERROR TOLERANCE   (52) =   5.000000    
    INFIN47, INTER115, SHELL57, SHELL157,
    SHELL63 WITH NLGEOM OFF AND KYOPT1 NOT = 1
         WARNING TOLERANCE (53) =  0.1000000    
         ERROR TOLERANCE   (54) =   1.000000    
    SHELL41, OR SHELL63 WITH KYOPT1=1
         WARNING TOLERANCE (55) =  0.4000000E-04
         ERROR TOLERANCE   (56) =  0.4000000E-01
    SHELL28
         WARNING TOLERANCE (57) =  0.1000000    
         ERROR TOLERANCE   (58) =   1.000000    
    SHELL63 WITH NLGEOM ON AND KYOPT1 NOT = 1
         WARNING TOLERANCE (59) =  0.1000000E-04
         ERROR TOLERANCE   (60) =  0.1000000E-01
    3D SOLID ELEMENT FACE
         WARNING TOLERANCE (67) =  0.2000000    
         ERROR TOLERANCE   (68) =  0.4000000    

 ELEMENT SHAPE CHECKING IS ON WITH DEFAULT LIMITS

7.5.7.5 Changing Shape Parameter Limits

For information about how to use the command method, see the description of the SHPP command in the ANSYS Commands Reference.

The GUI method is the simplest, and thus preferred, method for changing shape parameter limits. Follow these steps:

1. Choose menu path Main Menu>Preprocessor>Checking Ctrls>Shape Checking. The Shape Checking Controls dialog box appears.

2. Click the Change Settings option so that Yes appears.

3. Click on OK. The Change Shape Check Settings dialog box appears.

4. For any limit that you wish to change, enter a new limit. Use the scroll bar to move up and down within the list of limits.

5. When finished entering new limits, click on OK.

Examples of Changing Shape Parameter Limits

• Perhaps you are not particularly concerned about aspect ratio measures. You can turn off all aspect ratio testing by including the command SHPP,OFF,ASPECT in your START5x.ANS file. If that seems too drastic for your situation, you may choose to specify SHPP,MODIFY,1,1000 instead. Doing so radically loosens the warning limit for aspect ratio tests, without turning off the tests entirely.
• Suppose that you are using the sequential method of coupled-field analysis to perform a thermal-stress analysis. You plan to use SHELL57 elements for the thermal analysis first, and then SHELL63 elements (with nonlinear geometry on) for the structural analysis. If you build your model initially with SHELL57 elements, ANSYS will test the elements against loose warping limits (that is, a warning tolerance of 0.1, and an error tolerance of 1.0-refer to the sample output provided in Section 7.5.7.4 for a complete list of default limits). In contrast, the default warping limits for SHELL63 elements with nonlinear geometry on are very tight (a warning tolerance of 0.00001, and an error tolerance of 0.01). Since ANSYS will test the elements against loose limits for the thermal analysis, the tests may not turn up any elements that are in violation of the nonlinear SHELL63 limits. However, for the structural analysis, ANSYS will test the elements again when you switch the element type to SHELL63 [ETCHG,TTS] and turn on nonlinear geometry [NLGEOM,ON]. Because the limits will be much tighter for the second analysis, elements that caused no problems for the thermal analysis may produce warnings or errors in the structural analysis. You might be faced with a choice between a) accepting poor structural elements, which could compromise the quality of your analysis results, or b) revising the mesh and starting over with a new thermal solution. One way to prevent this situation is to build the model initially with SHELL63 elements with NLGEOM on; switch to SHELL57 elements for the thermal solution; then switch back to SHELL63 elements for the structural solution. Another alternative is for you to reset the warping limits for SHELL57 elements as tight as those for SHELL63 elements with NLGEOM on. You could accomplish this with the commands SHPP,MODIFY,53,0.00001 and SHPP,MODIFY,54,0.01.

7.5.7.6 Retrieving Element Shape Parameter Data

Command(s):

*GET, Par, ELEM, ENTNUM, SHPAR, IT1NUM
*VGET, ParR, ELEM, ENTNUM, SHPAR, IT1NUM,,, KLOOP

For example, the command *GET,A,ELEM,3,SHPAR,ASPE returns the calculated aspect ratio of element number 3 and stores it in a parameter named A. The command *VGET,A(1),ELEM,3,SHPAR,ASPE returns the aspect ratio of element number 3 and stores it in the first location of A. Retrieval continues with elements numbered 4, 5, 6, and so on, until successive array locations are filled.

See the descriptions of the *GET and *VGET commands in the ANSYS Commands Reference for more information.

7.5.7.7 Understanding Circumstances Under Which ANSYS Retests Existing Elements

• When you change the element type [ET,,Ename or ETCHG,Cnv] or one of its key options [KEYOPT].
• When you change the element TYPE number of an element [EMODIF].
• When you change the large deformation key [NLGEOM,Key] for SHELL63 elements.
• When you define a shell thickness [R] after you define an element, or you change an existing shell thickness [RMODIF] or the REAL number of a shell element [EMODIF].

7.5.7.8 Deciding Whether Element Shapes Are Acceptable

• Never ignore an element shape warning. Always investigate the effect that a "poorly" shaped element might have on your analysis results.
• Recognize that structural stress analyses that have the goal of determining stress at particular locations will typically suffer more severe effects from "poorly" shaped elements than will other types of analyses (deflection or nominal stress, modal, thermal, magnetic, etc.).
• If any "poorly" shaped elements are located in a critical region (such as near a critical stress point), their effect is more likely to be detrimental.
• "Poorly" shaped higher-order (midside-noded) elements will generally produce better results than will similarly shaped linear elements. The default ANSYS shape parameter limits are more restrictive on linear elements than on higher-order elements.
• Verification of analysis results by comparison with other analyses, test data, or hand calculations is essential regardless of whether elements produce shape warnings. If such verification indicates that you have high-quality results, there is little reason to worry about shape warnings.
• Some of the best quantitative measures of an element's acceptability are the error measures based on the element-to-element discontinuity in a stress or thermal gradient field. (See Chapter 5 of the ANSYS Basic Analysis Procedures Guide. An element that produces shape warnings and shows a high error measure compared to its neighbors is suspect.)

Refer to the description of the SHPP command in the ANSYS Commands Reference for more information about element shape checking.

7.6 Changing the Mesh

• Remesh with new element size specifications.
• Use the accept/reject prompt to discard the mesh, then remesh.
• Clear the mesh, redefine mesh controls, and remesh.
• Refine the mesh locally.
• Improve the mesh (for tetrahedral element meshes only).

7.6.1 Remeshing the Model

However, there are some restrictions to using this method. You can change element size specifications controlled by the KESIZE, ESIZE, SMRTSIZE, and DESIZE commands, but you cannot change size specifications assigned directly to lines [LESIZE]. If you want the option of changing LESIZE settings before remeshing, use the mesh accept/reject prompt instead of this method.

This remesh option is available only when meshing is performed interactively through the GUI. If you are using command input, you must first clear the mesh before remeshing (see Section 7.6.3 for more information).

7.6.2 Using the Mesh Accept/Reject Prompt

The accept/reject prompt is available for area and volume meshing. The advantage of using the prompt is that you do not have to manually clear the mesh [ACLEAR and VCLEAR].

7.6.3 Clearing the Mesh

To clear the mesh from keypoints [KCLEAR], lines [LCLEAR], areas [ACLEAR], or volumes [VCLEAR], pick Main Menu>Preprocessor>-Meshing-Clear>entity type in the GUI. (For more information on the clearing operation, see Section 8.5.1 of this manual.)

7.6.4 Refining the Mesh Locally

• The level of refinement to be done (in other words, the desired size of the elements in the refinement region, relative to the size of the original elements)
• The depth of surrounding elements that will be remeshed, in terms of the number of elements outward from the selected entity
• The type of postprocessing to be done after the original elements are split (smoothing and cleaning, smoothing only, or neither)
• Whether triangles can be introduced into the mesh during the refinement of an otherwise all-quadrilateral mesh

7.6.5 Improving the Mesh (Tetrahedral Element Meshes Only)

7.6.5.1 Automatic Invocation of Tetrahedral Mesh Improvement

7.6.5.2 User Invocation of Tetrahedral Mesh Improvement

• When tetrahedra improvement is invoked automatically during a volume meshing operation [VMESH], ANSYS uses a linear tetrahedral shape metric for improvement. This means that ANSYS ignores midside nodes that may be present within the elements. However, when you request tetrahedra improvement of a given mesh as documented below, ANSYS takes the midside nodes into account. Thus, for meshes of quadratic (midside-noded) tetrahedral elements, requesting additional tetrahedra improvement [VIMP] after the mesh is created [VMESH] can help to remove, or at least reduce, the number of element shape test warning messages that are produced and to improve the overall quality of the mesh.
• Since imported tetrahedral meshes have not received the benefits of the tetrahedral mesh improvement that ANSYS often performs automatically, imported tetrahedral meshes are likely candidates for user-invoked improvement.

You can request improvement of two "types" of tetrahedral elements:

• You can request improvement of tetrahedral elements that are not associated with a volume. (Typically, this option is useful for an imported tetrahedral mesh for which no geometry information is attached.) Use one of these methods:

TIMP

Main Menu>Preprocessor>-Meshing-Modify Mesh>Improve Tets> Detached Elems

• You can request improvement of tetrahedral elements that are in a selected volume or volumes. (You might want to use this option to further improve a volume mesh created in ANSYS [VMESH].) Use one of these methods:

VIMP

Main Menu>Preprocessor>-Meshing-Modify Mesh>Improve Tets> Volumes

7.6.5.3 Restrictions on Tetrahedral Mesh Improvement

• The mesh must consist of either all linear elements or all quadratic elements.
• For all of the elements in the mesh to be eligible for tetrahedral mesh improvement, they must all have the same attributes, including element type. (The element type must be tetrahedral, but the tetrahedral elements may be the degenerated form of hexahedral elements.) After tetrahedral mesh improvement, ANSYS reassigns the attributes from the old set of elements to the new set of elements.

Note-Tetrahedral mesh improvement is possible in a mesh of mixed element shapes (as opposed to types). For example, as stated earlier, improvement occurs automatically during the creation of transitional pyramid elements at the interface between hexahedral and tetrahedral element types. However, in a mixed mesh, only the tetrahedral elements are improved.

• Loading has an effect on whether tetrahedral mesh improvement is possible. Tetrahedral mesh improvement is possible when loading occurs in either of these ways:
  • When loads have been applied to the element faces or nodes on the boundary of the volume only
  • When loads have been applied to the solid model (and have been transferred to the finite element mesh)

Tetrahedral mesh improvement is not possible when loading occurs in either of these ways:

• When loads have been applied to the element faces or nodes within the interior of a volume
• When loads have been applied to the solid model (and have been transferred to the finite element mesh), but have also been applied to the element faces or nodes within the interior of a volume

Note-In the last two loading situations, ANSYS issues a warning message to notify you that you must remove the loads if you want tetrahedral mesh improvement to occur.

• If node or element components are defined, you will be asked whether you want to proceed with mesh improvement. If you choose to proceed, you must update any affected components.

7.6.5.4 Other Characteristics of Tetrahedral Mesh Improvement

• Element numbering and node numbering are modified.
• Generally, if ANSYS encounters an error or a user abort occurs, it leaves the mesh unchanged. However, ANSYS may save a partially improved mesh after an abort if you verify the save when ANSYS prompts you. If you have requested improvement for multiple volumes [VIMP], the abort applies only to the current volume mesh that is being improved; all previously improved volume meshes are already saved. (The same applies when an error occurs after the first of multiple volumes is improved.)

7.7 Some Hints and Cautions

7.7.1 Cautions

Figure 7-35 Avoiding sharp corners

Extreme Element Size Transition: Poor element quality will often occur if you specify too extreme a transition in element sizes.

Figure 7-36 Avoiding extreme element size transitions

Excessive Element Curvature: When using midside-node structural elements to model a curved boundary, you should usually make sure that you make your mesh dense enough that no single element spans more than 15° of arc per element length. If you do not need detailed stress results in the vicinity of a curved boundary, you can force the creation of straight-sided elements [MSHMID,1] in a coarse mesh along curved edges and faces. In cases where a curved-sided element will create an inverted element, the tetrahedra mesher automatically changes it to a straight-sided element and outputs a warning.

Figure 7-37 Use of MSHMID,1 to force straight-sided elements

RV53

7.7.2 Further Hints

• A tetrahedron meshing failure can be quite time consuming. One relatively quick way that you can make a preliminary check for a possible tetrahedron meshing failure is by meshing the surfaces of a volume with six-noded triangles. If this surface triangle mesh contains no sudden size transitions (admittedly often a difficult judgement) and produces no curvature or aspect ratio warnings, tetrahedron meshing failure is much less likely than if these conditions are not met. (Be sure to clear or deactivate the triangle elements before using the analysis model.)
• Avoid subtracting meshed entities from your model whenever possible. However, if you subtract entities that have been meshed and an undesirable mesh mismatch results, you can recover by clearing the mesh and remeshing the entities.

Go to the beginning of this chapter