Chapter 7: Meshing Your Solid Model

Go to the Next Chapter
Go to the Previous Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index

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

The procedure for generating a mesh of nodes and elements consists of three main steps:

The second step, setting mesh controls, is not always necessary because the default mesh controls are appropriate for many models. If no controls are specified, the program will use the default settings on the DESIZE command to produce a free mesh. As an alternative, you can use the SmartSize feature to produce a better quality free mesh (see Section 7.3.5 later in this chapter).

7.1.1 Free or Mapped Mesh?

Before meshing the model, and even before building the model, it is important to think about whether a free mesh or a mapped mesh is appropriate for the analysis. A free mesh has no restrictions in terms of element shapes, and has no specified pattern applied to it.

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

Before you generate a mesh of nodes and elements, you must first define the appropriate element attributes. That is, you must specify the following:

Note-For beam meshing only, you may also specify orientation keypoints as attributes of a line. Section 7.5.2 describes beam meshing in detail.

7.2.1 Creating Tables of Element Attributes

To assign attributes to your elements, you must first build tables of element attributes. Typical models include element types (ET command or menu path Main Menu>Preprocessor>Element Type>Add/Edit/Delete), real constants (R command or menu path Main Menu>Preprocessor>Real Constants), and material properties (MP and TB family of commands, menu path Main Menu> Preprocessor>Material Props>material option).

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

Once the attribute tables are assembled, you can assign element attributes to different parts of your model by "pointing" to the appropriate entries in the tables. The pointers are simply a set of reference numbers that include a material number (MAT), a real constant set number (REAL), an element type number (TYPE), a coordinate system number (ESYS) and, for beam meshing with BEAM188 or BEAM189, a section ID number (SECNUM). You can either assign the attributes directly to selected solid model entities, or define a default set of attributes that will be used for elements created in subsequent meshing operations.

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

Assigning the element attributes to the solid model entities allows you to pre-assign attributes for each region of your model. By using this method, you can avoid having to reset attributes in the middle of meshing operations. (Clearing a solid model entity of its nodes and elements will not delete attributes assigned directly to the entity.)

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

Command(s):

GUI:

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

Command(s):

GUI:

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

Command(s):

GUI:

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

Command(s):

GUI:

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

7.2.2.2 Assigning Default Attributes

You can assign a set of default attributes by simply pointing to various entries in the attribute tables. The pointers that are in effect at the time you create your elements (that is, when you initiate meshing) are used by the program to assign attributes from the tables to the solid model and to the elements. Attributes assigned directly to the solid model entities (as described above) will override the default attributes. Also, if you clear a solid model entity of its nodes and elements, any attributes that were assigned through default attributes will be deleted.

To assign a set of default attributes:

Command(s):

GUI:

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

In certain cases, the ANSYS program can choose the correct element type for a meshing or extrusion operation, eliminating the need for you to manually switch between element types when the correct choice is obvious.

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

The default mesh controls that the ANSYS program uses may produce a mesh that is adequate for the model you are analyzing. In this case, you will not need to specify any mesh controls. However, if you do use mesh controls, you must set them before meshing your solid model.

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

The ANSYS MeshTool (Main Menu>Preprocessor>MeshTool) provides a convenient path to many of the most common mesh controls, as well as to the most frequently performed meshing operations. The MeshTool is an interactive "tool box," not only because of the numerous functions (or tools) that it contains, but also because once you open it, it remains open until you either close it or you exit PREP7.

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:

This guide covers all of these functions in detail. For details about the MeshTool, access it using the path listed above and click on its Help button.

7.3.2 Element Shape

At a minimum, you should set the allowable element shapes if you plan on meshing with an element type that can take on more than one shape. For instance, many area elements can be both triangular and quadrilateral shaped within the same meshed area. Volume elements can often be either hexahedral (brick) or tetrahedral shaped, but a mixture of the two shapes in the same model is not recommended. (An exception to this involves the use of transitional pyramid elements, which is described in Section 7.3.9 of this manual.)

A Note About Degenerate Element Shapes

This chapter assumes that you are somewhat familiar with the concept of degenerate element shapes. For example, consider the PLANE82 element, which is a two-dimensional structural solid element having eight nodes (I,J,K,L,M,N,O,P). By default, PLANE82 has a quadrilateral shape. However, a triangular-shaped element can be formed by defining the same node number for nodes K, L, and O. Thus PLANE82 can be "degenerated" into a triangle. See Figure 7-3 for an illustration of PLANE82 in both its default and degenerate forms.

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

To specify element shapes, use either of these methods:

Command(s):

GUI:

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

If you are using the MSHAPE command, the value of the Dimension argument (2D or 3D) indicates the dimension of the model to be meshed. The value of the KEY argument (0 or 1) indicates the element shape to be used in the mesh:

GUI Method (Via the MeshTool)

For increased productivity, the MeshTool (described earlier in this chapter) is the recommended method for specifying element shape. You access the MeshTool via the following GUI path: Main Menu>Preprocessor>MeshTool. Using the MeshTool, you simply click on the desired element shape that you want ANSYS to use to mesh the model. From the MeshTool, you can also click on the type of meshing (free or mapped) that you want ANSYS to use. (For more information, see Section 7.3.3, "Choosing Free or Mapped Meshing.") Using the MeshTool makes selecting the shape simple, because it presents only those shapes that are compatible with the type of meshing that you are requesting, as well as with the dimension of the model you are meshing. (See Table 7-1 for the combinations of element shapes and meshing types that ANSYS supports.)

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

In addition to specifying element shape, you may also want to specify the type of meshing (free or mapped) that should be used to mesh your model. You do this by setting the meshing key:

Command(s):

GUI:

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

When meshing with quadratic elements, you can control the placement of midside nodes. Your choices for midside node placement are:

To control midside node placement:

Command(s):

GUI:

Main Menu>Preprocessor>-Meshing-Mesher Opts

7.3.5 Smart Element Sizing for Free Meshing

Smart element sizing (SmartSizing) is a meshing feature that creates initial element sizes for free meshing operations. SmartSizing gives the mesher a better chance of creating reasonably shaped elements during automatic mesh generation. This feature, which is controlled by the SMRTSIZE command, provides a range of settings (from coarse to fine mesh) for meshing both h-method and p-method models.

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

The SmartSizing algorithm first computes estimated element edge lengths for all lines in the areas or volumes being meshed. The edge lengths on these lines are then refined for curvature and proximity of features in the geometry. Since all lines and areas are sized before meshing begins, the quality of the generated mesh is not dependent on the order in which the areas or volumes are meshed. (Remember that for best results, all areas or volumes should be meshed at the same time.)

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

There are two categories of SmartSizing controls: basic and advanced.

Basic Controls

To use the basic controls, you simply specify a mesh size level from 1 (fine mesh) to 10 (coarse mesh). The program automatically sets a series of individual control values that are used to produce the requested size level. To specify the size level, use one of the following methods:

Command(s):

GUI:

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

You may prefer to use the advanced method, which involves setting the individual control quantities manually. This allows you to "tweak" the mesh to better fit your needs. You can change such things as the small hole and small angle coarsening keys, and the mesh expansion and transition factors (see the description of the SMRTSIZE command for a complete list of advanced controls). In addition, you can set a starting element size for SmartSizing with the ESIZE command.

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

Command(s):

GUI:

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

7.3.5.3 Interaction with Other Mesh Controls

Local element sizing controls (discussed later in Section 7.3.7, "Local Mesh Controls") can be used in conjunction with SmartSizing. However, if conflicting element sizes are set, the SmartSizing algorithm will handle them as follows:

7.3.6 Default Element Sizes for Mapped Meshing

The DESIZE command allows you to modify such defaults as: the minimum and maximum number of elements that will be attached to an unmeshed line, maximum spanned angle per element, and minimum and maximum edge length. The DESIZE command (Main Menu>Preprocessor>-Meshing-Size Cntrls> -Global-Other) is always used to control element sizing for mapped meshing. DESIZE settings are also used by default for free meshing. However, it is recommended that you use SmartSizing [SMRTSIZE] instead for free meshing operations.

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
Figure 7-7 Previewing the default mesh



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
Figure 7-8 Previewing the modified mesh



7.3.7 Local Mesh Controls

In many cases, the mesh produced by default element sizes is not appropriate due to the physics of the structure. Examples include models with stress concentrations or singularities. In these cases, you will have to get more involved with the meshing process. You can take more control by using the following element size specifications:

Command(s):

GUI:

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

Command(s):

GUI:

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

Command(s):

GUI:

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

All of the size specifications described above can be used together. If conflicting element sizes are set using more than one of the above commands, a specific hierarchy is observed. The hierarchy will vary slightly, depending on whether the DESIZE or SMRTSIZE method of default element sizing is used.

Note-Line divisions that have been established by KESIZE or ESIZE and a meshing operation will show up as negative numbers in a line listing [LLIST], while line divisions that you set via LESIZE show up as positive numbers. The signs of these numbers affect how ANSYS treats the line divisions if you clear the mesh later (ACLEAR, VCLEAR, etc., or menu path Main Menu>Preprocessor> -Meshing-Clear>entity). If the number of line divisions is positive, ANSYS does not remove the line divisions during the clearing operation; if the number is negative, ANSYS removes the line divisions (which will then show up as zeros in a subsequent line listing).

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

The discussion on meshing specifications has focused thus far on the setting of element sizes on the boundaries of the solid model (LESIZE, ESIZE, etc.). However, you can also control the mesh on the interior of an area where there are no lines to guide the size of the mesh. To do so, use one of the following methods:

Command(s):

GUI:

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

7.3.8.1 Controlling Mesh Expansion

The Lab=EXPND option on the MOPT command can be used to guide the mesh from a fine mesh on the boundary of an area to a coarse mesh on the interior (see Figure 7-9).

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

To improve mesh (b) above, a more gradual transition from small elements on the boundaries to large elements on the interior is needed. The Lab=TRANS option on the MOPT command can be used to control the rate of transitioning from fine to coarse elements. Figure 7-10 shows the same area meshed with MOPT,TRANS,1.3 used in addition to the MOPT setting which produced the previous mesh. This mesh has far fewer elements than mesh (a) of Figure 7-9, yet the transition from small elements to larger elements is fairly smooth. Also, the element aspect ratios are significantly better than the elements in mesh (b) of Figure 7-9.

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

7.3.8.3 Controlling Which Mesher ANSYS Uses

You can also use the MOPT command to control which surface meshers (triangle and quadrilateral) and which tetrahedra mesher ANSYS uses to perform a meshing operation [AMESH, VMESH].

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):

GUI:

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

The following options for triangle surface meshing are available:

The options listed below are available for quadrilateral surface meshing. Keep in mind that 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.

Figure 7-11 Mesh (a) shows a surface that was meshed with the alternate quadrilateral mesher; mesh (b) shows the same surface, this time meshed with the Q-Morph mesher.

Figure 7-12 Triangle element created in a small angle of an area when quadrilateral splitting is turned on

Tetrahedral Element Meshing Options

The following options for tetrahedral element meshing are available:

7.3.8.4 Controlling Tetrahedral Element Improvement

You can use the MOPT command to control the level of tetrahedra improvement that ANSYS performs when the next free volume meshing operation is initiated [VMESH, FVMESH].

Command(s):

GUI:

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

While some regions of a volume may be easy to divide into map-meshable parts, other regions may be geometrically complex. You may use hexahedral elements to fill the map-meshable regions of a volume, and tetrahedral elements to fill the remainder. In some cases, high-gradient regions may require hexahedral elements to capture detail, while for other, less critical regions, tetrahedral elements may be sufficient.

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

ANSYS can create transitional pyramid elements in either of these situations:

Figure 7-13 illustrates the creation of transitional pyramids at the interface of tetrahedral and hexahedral elements. In this example, a simple block is divided by an arbitrary cutting plane. The cutting plane serves as the interface between two volumes-one in which tetrahedral elements were generated, and the other in which hexahedral elements were generated (a). Figure 7-13 (b) provides an exploded view of the transitional pyramids; the tetrahedral elements have been removed.

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

7.3.9.2 Prerequisites for Automatic Creation of Transitional Pyramid Elements

In order for transitional pyramid elements to be created when you mesh a volume with tetrahedral elements, you must meet these prerequisites:

Command(s):

GUI:

Main Menu>Preprocessor>-Meshing-Mesher Opts

Command(s):

GUI:

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:

ANSYS creates transitional pyramid elements by default; if you prefer not to have transitional pyramid elements inserted into your mesh, issue the MOPT,PYRA,OFF command.

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

After creating transitional pyramid elements in a model, you can convert the 20-node degenerate tetrahedral elements in the model to their 10-node non-degenerate counterparts.

7.3.10.1 Benefits of Converting Degenerate Tetrahedral Elements

The process described in Section 7.3.9 permits the formation of pyramids only when you use an element type that supports degenerate tetrahedral and pyramidal shapes. Depending on your application, you may find that this prerequisite is too limiting.

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:

7.3.10.2 Performing a Conversion

To convert 20-node degenerate tetrahedral elements to their 10-node non-degenerate counterparts:

Command(s):

GUI:

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:

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:

7.3.10.3 Other Characteristics of Degenerate Tetrahedral Element Conversions

Other characteristics of degenerate tetrahedral element conversions include the following:

7.3.11 Doing Layer Meshing

The ANSYS program's layer meshing feature (currently, for 2-D areas only) enables you to generate line-graded free meshes having either of the following:

Such meshes are suitable for simulating CFD boundary layer effects, electromagnetic skin layer effects, etc.

7.3.12 Setting Layer Meshing Controls via the GUI

If you are using the ANSYS GUI, you set layer mesh controls on a picked set of lines by choosing Main Menu>Preprocessor>Mesh Tool, which displays the MeshTool panel. Pressing the Set button next to "Layer" opens a picking dialog for selecting lines, followed by the "Area Layer Mesh Controls on Picked Lines" dialog box. On it, you may specify any of the following.

Note-The thickness of LAYER1 should be greater than or equal to the specified element size for the line. If you use a size factor to specify LAYER1, it must be greater than or equal to 1.0.

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

The LESIZE command specifies layer meshing controls and other element size characteristics. For information about this command, see the ANSYS Commands Reference.

7.3.14 Listing Layer Mesh Specifications on Lines

To view or print layer meshing size specifications on lines, use one of the following:

Command(s):

GUI:

Utility Menu>List>Lines

7.4 Controls Used for Free and Mapped Meshing

In the previous sections, we have described various meshing controls that are available to you. Now we will focus on which controls are appropriate for free meshing, and which are appropriate for mapped meshing.

7.4.1 Free Meshing

In free meshing operations, no special requirements restrict the solid model. Any model geometry, even if it is irregular, can be meshed.

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):

GUI:

Main Menu>Preprocessor>-Meshing-Mesher Opts

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

Command(s):

GUI:

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

A special type of free meshing, called fan type meshing, is available for certain contact analysis cases that involve the meshing of three-sided areas with the TARGE170 element. When two of the three sides have only one element division, and the third side has any number of divisions, the result will be a fan type mesh. (The LESIZE command is used to set element divisions.) Fan type meshing ensures that ANSYS uses the minimum number of triangles to fill the area, which is important for contact problems. Consider the example shown in Figure 7-15, in which two of the sides have only one element division, while the third side has four.

Figure 7-15 Example of fan type meshing

Conditions for Fan Type Meshing

Remember that to use fan type meshing, the following conditions must be satisfied:

For more information, see Chapter 9 of the ANSYS Structural Analysis Guide and the description of the TARGE170 element in the ANSYS Elements Reference.

7.4.2 Mapped Meshing

You can specify that the program use all quadrilateral area elements, all triangle area elements, or all hexahedral (brick) volume elements to generate a mapped mesh. Mapped meshing requires that an area or volume be "regular;" that is, it must meet certain criteria.

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

An area mapped mesh consists of either all quadrilateral elements or all triangular elements.

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

You must specify equal numbers of line divisions on opposite edges of the area (or define line divisions to match one of the transition patterns) to achieve a mapped mesh. You do not necessarily have to specify line divisions on all lines. As long as mapped meshing has been requested [MSHKEY,1], the program will transfer line divisions from one line to the opposite line, and on into adjacent areas being meshed [AMESH]. The program will also produce matched line divisions from KESIZE or ESIZE specifications, when possible.

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
Please see the MSHKEY, ESIZE, LESIZE, and AMESH command descriptions for more information.

Line Concatenation

If an area is bounded by more than four lines, you can combine [LCOMB] or concatenate [LCCAT] some of the lines to reduce the total number of lines to four. Whenever LCOMB is permitted (that is, when lines are tangent and are attached to the same areas), it is generally preferred over LCCAT. LCOMB can also be used for non-tangent lines, but a node will not necessarily be generated at the kink in the line.

To concatenate lines:

Command(s):

GUI:

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):

GUI:

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

The AMAP command offers the easiest way to obtain a mapped mesh. AMAP (Main Menu>Preprocessor>-Meshing-Mesh>-Areas-Mapped>By Corners) uses specified keypoints as corners and internally concatenates all lines between the keypoints. The area is automatically meshed with all quadrilateral or all triangular elements (a MSHKEY specification is not required). The same rules about meshing controls apply for AMAP as for mapped meshing by line concatenation.

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

Another way to create a mapped area mesh is to specify line divisions on opposite sides of the area such that the divisions permit a transition mapped quadrilateral mesh. Transition mapped quadrilateral meshing is only applicable to four-sided areas (with or without concatenation). Some examples are shown in Figure 7-21.

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

Transition mapped meshing is also valid for mapped area meshes of triangle elements. As with transition mapped quadrilateral meshing, transition mapped triangle meshing is only applicable to four-sided areas, and the specified line divisions must match one of the patterns shown in Figure 7-22. To achieve a transition mapped triangle mesh, you must also use an element type that supports a triangular shape, set the meshing key to mapped [MSHKEY,1], and set the shape specification to allow triangles [MSHAPE,1,2D].

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

To mesh a volume with all hexahedron elements, the following conditions must be satisfied:

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

As with lines, you can add [AADD] or concatenate [ACCAT] areas if you need to reduce the number of areas bounding a volume for mapped meshing. If there are also lines bounding the concatenated areas, the lines must be concatenated as well. You must concatenate the areas first, then follow with line concatenations. This procedure is illustrated by the sample input listing that appears below:

! first, concatenate areas for mapped volume meshing:
ACCAT,...
! next, concatenate lines for mapped meshing of bounding areas:
LCCAT,...
LCCAT,...
VMESH,...
Note-Whenever AADD is permitted (that is, when areas are flat and coplanar), it is generally preferred over ACCAT. (Line divisions will be transferred from one edge to another as described earlier.)

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):

GUI:

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):

GUI:

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

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

Transition Mapped Hexahedral Meshing

You can create a mapped volume mesh by specifying line divisions on opposite edges of the volume such that the divisions permit a transition mapped hexahedral mesh. Transition mapped hexahedral meshing is only applicable to six-sided volumes (with or without concatenation). Some examples are shown in Figure 7-26.

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

Concatenation is solely intended to be used as an aid to mapped meshing; it is not a Boolean "add" operation. Concatenation should be the last step you undertake before you execute a mapped mesh of your solid model, because the output entity obtained from a concatenation cannot be used in any subsequent solid modeling operation (other than meshing, clearing, or deleting). For example, a line created by an LCCAT operation cannot have any solid model loads applied to it; nor can it be part of any Boolean operation; nor can it be copied, dragged, rotated [xGEN, xDRAG, xROTAT], etc.; nor can it be used in another concatenation.

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

Command(s):

GUI:

Utility Menu>Select>Entities

Although you need to be aware of the restrictions on output entities listed earlier in this section, no such restrictions affect the input entities in a concatenation. However, the input entities will become "lost" or "detached," so far as higher-level entities are concerned. That is, if an area is bounded by five lines (L1-L5), and two of those lines are concatenated (LCCAT,1,2 => L6), the program will no longer recognize lines L1 and L2 as being attached to that area. However, you can reattach L1 and L2 to the area by deleting L6 to undo the concatenation. (See Figure 7-28.)

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

Once you have built your solid model, established element attributes, and set meshing controls, you are ready to generate the finite element mesh. First, however, it is usually good practice to save your model before you initiate mesh generation:

Command(s):

GUI:

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 mesh the model, you must use a meshing operation that is appropriate for the entity type being meshed. You can mesh keypoints, lines, areas, and volumes using the commands and GUI paths described below.

Command(s):

GUI:

Main Menu>Preprocessor>-Meshing-Mesh>Keypoints

Command(s):

GUI:

Main Menu>Preprocessor>-Meshing-Mesh>Lines

Command(s):

GUI:

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

Command(s):

GUI:

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

7.5.2 Generating a Beam Mesh With Orientation Nodes

You can assign orientation keypoints as attributes of a line for beam meshing, just as you would assign a real constant set number, or a material property set number. The orientation keypoints are independent of the line that is to be meshed. Based on the location of these keypoints, ANSYS will automatically create orientation nodes along with the beam elements. Line meshing with automatic generation of orientation nodes is supported for elements BEAM4, BEAM24, BEAM44, BEAM161, BEAM188, and BEAM189.

To assign orientation keypoints as attributes of a line:

Command(s):

GUI:

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

If a line is bounded by two keypoints (KP1 and KP2) and two orientation keypoints (KB and KE) have also been defined as attributes of the line, the orientation vector at the beginning of the line extends from KP1 to KB, and the orientation vector at the end of the line extends from KP2 to KE. ANSYS computes the orientation nodes by interpolating the orientation as given by the above two orientation vectors.

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

The direction in which beam sections are oriented will affect the beam element mesh and the analysis results. Beam meshing with orientation nodes gives you control over these effects. Section 7.5.2.4 provides examples of various ways to align the beam sections.

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

This section describes how to generate a beam mesh with orientation nodes, using either command input or the ANSYS GUI. It assumes that you have already defined the geometry and element attribute tables for your model, and you are now ready to assign specific attributes to a line for beam meshing. This section does not attempt to cover other aspects of a typical beam analysis. For detailed information about beam analysis and a sample problem illustrating the generation of a beam mesh with orientation nodes, see Chapter 8 of the ANSYS Advanced Analysis Techniques Guide.

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.

3. Set the number of element divisions to be generated along the line mesh [LESIZE].

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

You can define one orientation keypoint or two orientation keypoints as attributes of a line. If you define two, you can assign both of them to the same location in your model.

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.

Figure 7-30 Constant orientation vs. pre-twist

7.5.2.5 Other Considerations for Beam Meshing With Orientation Nodes

Other things to consider when meshing beams with orientation nodes include the following:

7.5.3 Generating a Volume Mesh From Facets

In addition to using VMESH to generate volume elements, you can generate a volume mesh from a set of detached exterior area elements (facets). For example, this capability is useful in situations where you cannot mesh a particular area. In such a situation, first mesh the areas that can be meshed. Next, define the remaining area elements using direct generation. (Elements that you define using direct generation are considered to be detached elements, because they have no solid model associativity.) Finally, use one of the methods below to generate nodes and tetrahedral volume elements from the detached area elements:

Command(s):

GUI:

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

Additional considerations for using xMESH commands include the following:

7.5.5 Generating a Volume Mesh By Sweeping

Using volume sweeping, you can fill an existing unmeshed volume with elements by sweeping the mesh from a bounding area (called the "source area") throughout the volume. If the source area mesh consists of quadrilateral elements, the volume is filled with hexahedral elements. If the area consists of triangles, the volume is filled with wedges. If the area consists of a combination of quadrilateral and triangular elements, the volume is filled with a combination of hexahedral and wedge elements. The swept mesh is fully associated with the volume.

7.5.5.1 Benefits of Volume Sweeping

Volume sweeping provides these benefits:

7.5.5.2 What to Do Before You Sweep a Volume

Follow these steps before you invoke the volume sweeper:

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

2. Make sure that you have defined the appropriate 2-D and 3-D element types [ET]. For example, if you are going to pre-mesh the source area, and you want the swept volume to contain quadratic hexahedral elements, you should mesh the source area with quadratic 2-D elements.

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:

Command(s):

GUI:

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

Figure 7-31 Specifying number of element divisions, source area, and target area for volume sweeping

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.

5. Optionally, mesh the source, target, and/or side area(s).

Figure 7-32 Sweeping a volume with different source and target area topologies

Figure 7-33 (a) shows an example of a model that contains two volumes adjacent to one another. Because of the model's geometry, it is necessary to sweep the volumes in different directions, as shown in Figure 7-33 (b).

Figure 7-33 Sweeping adjacent volumes in different directions

7.5.5.3 Invoking the Volume Sweeper

To invoke the volume sweeper:

Command(s):

GUI:

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:

See the description of the VSWEEP command in the ANSYS Commands Reference for details about these arguments.

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

If a volume sweeping operation fails due to bad element shapes, try one or more of the strategies listed below. We recommend that you try these strategies in the order in which they are listed.

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:

4. If the elements flagged by SHPP,WARN are stretched within thin sections of the target area, but the previous strategy does not work, clear the mesh and then reinvoke the volume sweeper with line smoothing turned on [VSWEEP,,,,1]. See Figure 7-34 (d). (This setting is not recommended for large models due to speed considerations.)

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

Other characteristics of volume sweeping include the following:

7.5.6 Aborting a Mesh Operation

When meshing is initiated, an ANSYS status window appears. The window displays a message concerning the current status of the meshing operation, and also displays a scale showing the percentage of the meshing operation that is complete. Both the message and the percentage scale are updated periodically as the operation proceeds.

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

"Badly shaped" elements can, on occasion, cause very poor analytical results. For this reason, the ANSYS program performs element shape checking to warn you whenever any operation creates an element having a poor shape. Unfortunately, however, there are few universal criteria that can be used to identify a "poorly shaped" element. In other words, an element that gives poor results in one analysis might give perfectly acceptable results in another analysis. Thus, you must realize that the criteria that the ANSYS program uses to identify poor element shapes are somewhat arbitrary. The fact that you receive even hundreds of element shape warnings does not necessarily mean that element shapes will cause any inaccuracy of results. (Conversely, if you do not receive any warnings about element shapes, that does not guarantee accurate results.) As in so many aspects of finite element analysis, the final determination of whether or not your element shapes are acceptable for your application remains your responsibility.

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):

GUI:

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

The sections that follow cover how to:

Note-The ANSYS Theory Reference provides detailed information about the shape tests that ANSYS performs and explains the logic that was used to determine each test's default warning and error limits.

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

As stated above, ANSYS performs element shape checking by default. When element shape checking occurs, any new element-regardless of how it was created-is tested against existing shape parameter warning and error limits. If the element violates any of the error limits, it not only produces an error message, but also either (a) causes a meshing failure, or (b) for element creation other than AMESH or VMESH, is not stored.

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:

7.5.7.2 Turning Individual Shape Tests Off and On

Rather than turn off shape checking entirely, you can selectively control which tests are off and which are on.

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

For example, the command SHPP,OFF,WARP turns off all warping factor tests.

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

The output below, which is from the SHPP,SUMMARY command, provides a summary of shape test results for all selected elements.

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

The output below, which is from the SHPP,STATUS command, lists the element shape parameters and default shape parameter limits in ANSYS 5.5. By default, when an element's shape falls outside of these limits, a warning or error condition occurs. See Section 7.5.7.5 for information about how to change the 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

If the ANSYS program's default shape parameter limits do not suit your purposes, you can change them by using either the command method [SHPP,MODIFY,VALUE1,VALUE2] or the GUI.

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

The ANSYS program's element shape checking controls provide the flexibility to fit varied analysis needs. For example:

7.5.7.6 Retrieving Element Shape Parameter Data

You can use the *GET and *VGET commands to retrieve element shape parameter data:

Command(s):

Note-You cannot use the GUI paths for these commands to retrieve element shape parameter data.

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

Certain types of changes that you make to defined elements can invalidate prior element shape testing. ANSYS is designed to trap these types of changes and retest the affected elements automatically. Circumstances under which ANSYS retests existing elements include:

Note-There is a distinction between the element type and that element type's TYPE number. The element type is the true name of the element (for example, BEAM4 or SHELL63, sometimes shortened to simply 4 or 63). The element type's TYPE number is an arbitrary number that is locally assigned to a particular element type; you use the TYPE number to reference the element type when assigning attributes to your model.

7.5.7.8 Deciding Whether Element Shapes Are Acceptable

Here are some suggestions to help you decide whether you should be concerned about an element shape warning:

To check element shapes in an existing mesh (an ANSYS mesh or a mesh imported from a CAD program), use the CHECK command (Main Menu> Preprocessor>-Meshing-Sel Bad Elems).

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

If you decide that the generated mesh is not appropriate, you can easily change the mesh by one of the following methods:

Details of these methods are discussed below.

7.6.1 Remeshing the Model

You can remesh a meshed model by resetting element size controls and initiating the meshing operation [AMESH or VMESH]. This is the simplest way to change your mesh. The accept/reject prompt is not required, and the mesh does not need to be cleared in order to remesh it.

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

As mentioned earlier, you can activate the mesh accept/reject prompt in the GUI by picking Main Menu>Preprocessor>-Meshing-Mesher Opts before meshing. (The prompt is turned off by default.) When activated, the prompt appears after each meshing operation and allows you to either accept or reject the generated mesh. If the mesh is rejected, all nodes and elements will be cleared from the meshed entities. You can then reset any of the meshing controls and remesh the model.

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

Clearing the mesh of nodes and elements is not always required before remeshing. However, you do have to clear the mesh in order to respecify LESIZE settings. You also have to clear the mesh if you want to change the underlying solid model.

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

If you are generally satisfied with a mesh but would like to have more elements in a particular region, you can refine the mesh locally around selected nodes [NREFINE], elements [EREFINE], keypoints [KREFINE], lines [LREFINE], or areas [AREFINE]. The elements surrounding the chosen entities will be split to create new elements. You control the refinement process by specifying:

You can access local mesh refinement in the GUI by picking Main Menu> Preprocessor>-Meshing-Modify Mesh>-Refine At-entity. You can also do overall refinement by using the command ESEL,ALL or by picking the menu path Main Menu>Preprocessor>-Meshing-Modify Mesh>-Refine At-All. See Chapter 8 of this manual for details on refining a mesh locally.

7.6.5 Improving the Mesh (Tetrahedral Element Meshes Only)

The tetrahedral mesh improvement feature enables you to improve a given tetrahedral mesh. ANSYS performs this improvement through face swapping, node smoothing, and other techniques that it uses to reduce the number of poorly-shaped tetrahedral elements (in particular, the number of sliver tetrahedral elements)-as well as the overall number of elements-in the mesh. It also improves the overall quality of the mesh.

7.6.5.1 Automatic Invocation of Tetrahedral Mesh Improvement

In many cases, you won't need to take any action to obtain the benefits offered by the tetrahedral mesh improvement feature. As described earlier in Section 7.3.8.4, the ANSYS program invokes the feature automatically as a postprocessing step of its volume meshers. Tetrahedral mesh improvement also occurs automatically during the creation of transitional pyramid elements (described in Section 7.3.9) and the refinement of tetrahedral element meshes (described in Chapter 8).

7.6.5.2 User Invocation of Tetrahedral Mesh Improvement

Although tetrahedral mesh improvement often occurs automatically, there are certain situations in which you'll find it useful to request additional improvement for a given tetrahedral mesh:

Tetrahedral mesh improvement is an iterative process. Each time that processing completes, a special window appears to report the improvement statistics from that iteration, along with diagnostic messages. If you want to try to improve the mesh further, you can reissue your request repeatedly, until either the statistics indicate a satisfactory mesh, or until it converges and no more noticeable improvement is made.

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

Command(s):

GUI:

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

Command(s):

GUI:

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

7.6.5.3 Restrictions on Tetrahedral Mesh Improvement

The following restrictions apply to tetrahedral mesh improvement:

7.6.5.4 Other Characteristics of Tetrahedral Mesh Improvement

Other characteristics of tetrahedral mesh improvement include:

Please see the TIMP and VIMP command descriptions for more information.

7.7 Some Hints and Cautions

7.7.1 Cautions

Regions That Are Flattened or Have Excessively Sharp Corners: Areas or volumes that are flattened or have a sharp interior corner can commonly experience a meshing failure.

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


Go to the beginning of this chapter