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 *
7.1 How to Mesh Your Solid Model
The procedure for generating a mesh of nodes and elements consists of three
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).
- Set the element attributes (described in Section 7.2).
- Set mesh controls (optional). ANSYS offers a large number of mesh
controls, which you can choose from to suit your needs. Review Section
7.3 and Section 7.4 for descriptions of these mesh controls.
- Generate the mesh (described in Section 7.5).
7.1.1 Free or Mapped Mesh?
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
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
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.
- Element type (for example, BEAM3, SHELL61, etc.)
- Real constant set (usually comprising the element's geometric properties,
such as thickness or cross-sectional area)
- Material properties set (such as Young's modulus, thermal conductivity,
- Element coordinate system
- Section ID (for BEAM188 and BEAM189 elements only-see Section 7.5.2)
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
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
For beam meshing with BEAM188 or BEAM189 elements, you can build a table of sections
using the SECTYPE and SECDATA commands (Main Menu>
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
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
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
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.
184.108.40.206 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
- To assign attributes to keypoints:
Main Menu>Preprocessor>-Attributes-Define>All Keypoints
Main Menu>Preprocessor>-Attributes-Define>Picked KPs
- To assign attributes to lines:
Main Menu>Preprocessor>-Attributes-Define>All Lines
Main Menu>Preprocessor>-Attributes-Define>Picked Lines
- To assign attributes to areas:
Main Menu>Preprocessor>-Attributes-Define>All Areas
Main Menu>Preprocessor>-Attributes-Define>Picked Areas
- To assign attributes to volumes:
Main Menu>Preprocessor>-Attributes-Define>All Volumes
Main Menu>Preprocessor>-Attributes-Define>Picked Volumes
220.127.116.11 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:
Main Menu>Preprocessor>-Attributes-Define>Default Attribs
18.104.22.168 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 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
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
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
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.
- Controlling SmartSizing levels
- Setting element size controls
- Specifying element shape
- Specifying meshing type (free or mapped)
- Meshing solid model entities
- Clearing meshes
- Refining meshes
7.3.2 Element Shape
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.
22.214.171.124 Element Shape Specification
To specify element shapes, use either of these methods:
Main Menu>Preprocessor>-Meshing-Mesher Opts
Main Menu>Preprocessor>-Meshing-Mesh>-Volumes-Mapped>4 to 6
There are two factors to consider when specifying element shape: the desired
element shape and the dimension of the model to be meshed.
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:
- When KEY=0, ANSYS meshes with quadrilateral-shaped elements if
Dimension=2D and with hexahedral-shaped elements if Dimension=3D (as
long as the element type supports quadrilateral or hexahedral element
- When KEY=1, ANSYS meshes with triangle-shaped elements if
Dimension=2D and with tetrahedral-shaped elements if Dimension=3D (as
long as the element type supports triangle or tetrahedral element shapes,
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:
Main Menu>Preprocessor>-Meshing-Mesher Opts
As described in Section 126.96.36.199, "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 188.8.131.52 for related
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
Table 7-1 Supported combinations of element shape and meshing type
Table 7-2 explains what happens when you fail to specify values for these
|Mapped If Possible; Otherwise Free
Mesh With SmartSizing On
Table 7-2 Failure to specify element shape and/or meshing type
See the descriptions of the MSHAPE
and MSHKEY commands in the ANSYS Commands Reference for more information.
|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.
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:
- Midside nodes (if any) of elements on a region boundary follow the
curvature of the boundary line or area. This is the default.
- Place midside nodes of all elements so that element edges are straight.
This option allows a coarse mesh along curves. However, the curvature of
the model is not matched.
- Do not create midside nodes (elements have removed midside nodes).
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
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.
184.108.40.206 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
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
220.127.116.11 SmartSizing Controls - Basic versus Advanced
There are two categories of SmartSizing controls: basic and advanced.
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:
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
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:
Main Menu>Preprocessor>-Meshing-Size Cntrls>-SmartSize-Adv
18.104.22.168 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:
- Any element size specifications on lines (LESIZE command or menu path Main
Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-option) will be
used as defined. SmartSizing and the LESIZE command work better together
now than they did in releases prior to ANSYS 5.4. When you use
SmartSizing on lines that are adjacent to lines that have defined element
size specifications, ANSYS always takes the sizes into account before
performing SmartSizing, resulting in a better mesh.
- Any element size specifications at keypoints (KESIZE command or menu path Main
Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints -option) will
be assigned, but may be overridden to accommodate curvature and
proximity of features.
- If a global element size is set (ESIZE
command or menu path Main Menu>Preprocessor>-Meshing-Size
Cntrls>-Global-Size), it will be overridden as necessary to accommodate
curvature and proximity of features. If a consistent element size is desired,
set the global element size and turn SmartSizing off (SMRTSIZE,OFF or menu path Main
Menu> Preprocessor>-Meshing-Size Cntrls>-SmartSize-Basic).
- Default element sizes specified with the DESIZE command (Main Menu>
Preprocessor>-Meshing-Size Cntrls>-Global-Other) are ignored when
SmartSizing is on.
7.3.6 Default Element Sizes for Mapped Meshing
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
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
6. Request a line plot [LPLOT].
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
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
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:
- To control the global element size in terms of the element edge length used
on surface boundaries (lines) or the number of element divisions per line:
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Global-Size
- To control the element sizes near specified keypoints:
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints-All KPs
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints-Picked KPs
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Keypoints-Clr Size
- To control the number of elements on specified lines:
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-All Lines
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-Picked Lines
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Lines-Clr Size
Note-When you use the GUI method to set the number of elements on
specified lines, and any of those lines is connected to one or more meshed
lines, areas, or volumes, ANSYS prompts you to determine whether you
want to clear the meshed entities. If you answer yes to the prompt, ANSYS
clears the meshed entities. (This occurs only when you perform this
operation via the GUI; ANSYS does not prompt you when you use the
command method [LESIZE].)
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).
- Hierarchy used for DESIZE element
sizing. For any given line, element sizes along the line are established as
- Line divisions specified with LESIZE are always honored.
- If line divisions have not been set for the line, KESIZE specifications at its
keypoints (if any) are used.
- If there are no size specifications on the line or on its keypoints, element
sizes are established by the ESIZE
- If none of the above size specifications are set, DESIZE settings will control element
sizes for the line.
- Hierarchy used for SMRTSIZE
element sizing. For any given line, element sizes along the line are
established as follows:
- Line divisions specified with LESIZE are always honored.
- If line divisions have not been set for the line, KESIZE specifications at its
keypoints (if any) are used, but may be overridden to account for
curvature and small geometric features.
- If there are no size specifications on the line or on its keypoints, ESIZE specification will be used as a
starting element size, but may be overridden to account for curvature
and small geometric features.
- If none of the above size specifications are set, SMRTSIZE settings will control
element sizes for the line.
If you are performing a linear static structural or linear steady-state thermal
analysis, you can let the program establish meshing controls automatically as it
adapts element sizes to drive the estimated error in the analysis below a target
value. This procedure, known as adaptive meshing, is described in Chapter
3 of the ANSYS Advanced Analysis
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:
Main Menu>Preprocessor>-Meshing-Size Cntrls>-Global-Area Cntrls
22.214.171.124 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
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.
126.96.36.199 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 7-10 Area mesh with expansion and transition control (MOPT command)
188.8.131.52 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.
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
Surface Meshing Options
The following options for triangle surface meshing are available:
- Let ANSYS choose which triangle surface mesher to use. This is the
recommended setting and the default. In most cases, ANSYS will choose
the main triangle mesher, which is the Riemann space mesher. If the
chosen mesher fails for any reason, ANSYS invokes the alternate mesher
and re-tries the meshing operation.
To choose this option, issue the command MOPT,AMESH,DEFAULT. In the GUI,
access the Mesher Options dialog box and choose Program Chooses in
the Triangle Mesher option menu.
- Main triangle surface mesher (Riemann space mesher). ANSYS uses the
main mesher, and it does not invoke an alternate mesher if the main
mesher fails. The Riemann space mesher is well suited for most surfaces.
To choose this option, issue the command MOPT,AMESH,MAIN. In the GUI,
access the Mesher Options dialog box and choose Main from the Triangle
Mesher option menu.
- First alternate triangle surface mesher (3-D tri mesher). ANSYS uses the
first alternate triangle mesher, and it does not invoke another mesher if this
mesher fails. This option is not recommended due to speed
considerations. However, for surfaces with degeneracies in parametric
space, this mesher often provides the best results.
To choose this option, issue the command MOPT,AMESH,ALTERNATE. In the
GUI, access the Mesher Options dialog box and choose Alternate from the
Triangle Mesher option menu.
- Second alternate triangle surface mesher (2-D parametric space mesher).
ANSYS uses the second alternate triangle mesher, and it does not invoke
another mesher if this mesher fails. This option is not recommended for
use on surfaces with degeneracies (spheres, cones, and so on) or on
poorly parameterized surfaces because poor meshes may be created.
To choose this option, issue the command MOPT,AMESH,ALT2. In the GUI,
access the Mesher Options dialog box and choose Alternate 2 from the
Triangle Mesher option menu.
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.
- Let ANSYS choose which quadrilateral surface mesher to use. This is the
recommended setting and the default. In most cases, ANSYS will choose
the main quadrilateral mesher, which is the Q-Morph (quad-morphing)
mesher. For very coarse meshes, ANSYS may choose the alternate
quadrilateral mesher instead. If either mesher fails for any reason, ANSYS
invokes the other mesher and re-tries the meshing operation.
To choose this option, issue the command MOPT,QMESH,DEFAULT. In the GUI,
access the Mesher Options dialog box and choose Program Chooses from
the Quad Mesher option menu.
- Main quadrilateral surface mesher (Q-Morph mesher). ANSYS uses the
main mesher, and it does not invoke the alternate mesher if the main
In most cases, the Q-Morph mesher results in higher quality elements (see
Figure 7-11). The Q-Morph mesher is particularly beneficial to users
whose applications require boundary sensitive, highly regular nodes and
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.
Notice that although both meshes shown in Figure 7-11 contain one
triangle element (the triangle elements are shaded in the figure), the
triangle element in Figure 7-11 (a) occurs on the boundary of the area. The
triangle element in Figure 7-11 (b) is an internal element, which is a more
desirable location for it in the mesh.
For the Q-Morph mesher to be able to generate an all-quadrilateral mesh
of an area, the total number of line divisions on the boundaries of the area
must be even. (In most cases, turning on SmartSizing [SMRTSIZE,SIZLVL] will result in an
even total number of line divisions on the boundaries.)
A triangle element (or elements) will result in the area mesh if any of these
statements is true:
1. The total number of line divisions on the boundaries of the area is odd.
2. Quadrilateral element splitting is turned on for error elements [MOPT,SPLIT,ON or MOPT,SPLIT,ERR] and a
quadrilateral element in violation of shape error limits would be created
if ANSYS did not split the element into triangles. (Splitting is on for
error elements by default.)
3. Quadrilateral splitting is turned on for both error and warning elements
[MOPT,SPLIT,WARN], and a
quadrilateral element in violation of shape error and warning limits
would be created if ANSYS did not split the element into triangles.
4. Quadrilateral element splitting is turned on for either a) error elements
or b) error and warning elements, and the area contains a small angle
(< 30°) between adjacent boundary intervals. See Figure 7-12.
To choose this option (Q-Morph mesher), issue the command MOPT,QMESH,MAIN. In the GUI,
access the Mesher Options dialog box and choose Main from the Quad
Mesher option menu.
Figure 7-12 Triangle element created in a small angle of an area when
quadrilateral splitting is turned on
- Alternate quadrilateral surface mesher. ANSYS uses the alternate mesher,
and it does not invoke the main mesher if the alternate mesher fails.
For this mesher to be able to generate an all-quadrilateral mesh of an
area, the total number of line divisions on the boundaries of the area must
be even, and quadrilateral splitting must be turned off [MOPT,SPLIT,OFF].
To choose this option, issue the command MOPT,QMESH,ALTERNATE. In the
GUI, access the Mesher Options dialog box and choose Alternate in the
Quad Mesher option menu. To use this mesher, you must also select
either the first alternate or the second alternate triangle surface mesher.
Tetrahedral Element Meshing Options
The following options for tetrahedral element meshing are available:
- Let ANSYS choose which tetrahedra mesher to use. This is the default.
With this setting, ANSYS uses the main tetrahedra mesher when it can;
otherwise, it uses the alternate tetrahedra mesher. (ANSYS always uses
the alternate tetrahedra mesher when meshing with p-elements.)
To choose this option, issue the command MOPT,VMESH,DEFAULT. In the GUI,
access the Mesher Options dialog box and choose Program Chooses in
the Tet Mesher option menu.
- Main tetrahedra mesher (Delaunay technique mesher). For most models,
this mesher is significantly faster than the alternate mesher.
To choose the main tetrahedra mesher, issue the command MOPT,VMESH,MAIN. In the GUI,
access the Mesher Options dialog box and choose Main in the Tet Mesher
- Alternate tetrahedra mesher (advancing front mesher from Revision 5.2).
This mesher does not support the generation of a tetrahedral volume mesh
from facets [FVMESH]. If this
mesher is selected and you issue the FVMESH command, ANSYS uses the
main tetrahedra mesher to create the mesh from facets and issues a
warning message to notify you.
To choose the alternate tetrahedra mesher, issue the command MOPT,VMESH,ALTERNATE. In the
GUI, access the Mesher Options dialog box and choose Alternate in the Tet
Mesher option menu.
184.108.40.206 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].
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.
220.127.116.11 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
- You are ready to mesh a volume with tetrahedral elements. The volume
immediately adjacent to that volume has already been meshed with
hexahedral elements. The two volumes have been glued together [VGLUE]. (Two volumes for which you
want to create transitional pyramids must share a common area; the
quadrilateral faces from the hexahedral elements must be located on that
- At least one of the areas on a volume has been meshed with quadrilateral
elements. In this situation you simply mesh the volume with tetrahedral
elements, and ANSYS forms the pyramids directly from the quadrilateral
elements. If you want, you can then mesh any adjacent volumes with
Figure 7-13 Creation of transitional pyramid elements at an interface
18.104.22.168 Prerequisites for Automatic Creation of Transitional Pyramid
In order for transitional pyramid elements to be created when you mesh a volume
with tetrahedral elements, you must meet these prerequisites:
- When you set your element attributes, be sure that the element type you
assign to the volume is one that can be degenerated into a pyramid shape;
currently, this list includes SOLID62, SOLID73, VISCO89, SOLID90, SOLID95, SOLID96, SOLID97, and SOLID122. ANSYS does not support
transitional pyramids for any other element types. (See Section 7.2.2 for
information about the methods you can use to set attributes.)
- When you set your meshing controls, activate transitioning and indicate
that you want to degenerate three-dimensional elements.
To activate transitioning (the default), use one of the following methods:
Main Menu>Preprocessor>-Meshing-Mesher Opts
To degenerate three-dimensional elements, use one of the following
Main Menu>Preprocessor>-Meshing-Mesher Opts
If these prerequisites are met and you now mesh the volume with tetrahedral
elements [VMESH], the ANSYS program
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.
- Determines where transitional pyramid elements are appropriate
- Combines and rearranges tetrahedral elements to create pyramid elements
- Inserts the pyramid elements into the mesh
Note-For quadratic pyramid elements that are immediately adjacent to linear
hexahedral elements, ANSYS automatically drops midside nodes at the interface.
This, in fact, occurs when meshing any quadratic element if linear elements are
adjacent in a neighboring volume.
7.3.10 Converting Degenerate Tetrahedral Elements to Their
After creating transitional pyramid elements in a model, you can convert the
20-node degenerate tetrahedral elements in the model to their 10-node
22.214.171.124 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:
- Less random access memory (RAM) is required per element.
- When you are not using the Pre-conditioned Conjugate Gradient (PCG)
equation solver, the files that ANSYS writes during solution are
- Even when you are using the PCG equation solver, you gain a modest
126.96.36.199 Performing a Conversion
To convert 20-node degenerate tetrahedral elements to their 10-node
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
If you are using the TCHG command to
perform the conversion, specify values for the following arguments:
- Use the ELEM1 argument to identify the type of element that you want to
convert. For example, to convert SOLID95
elements, you must specify either SOLID95
or 95 for the value of ELEM1.
- Use the ELEM2 argument to identify the type of element that is the
counterpart to the ELEM1 element. For example, to convert SOLID95 elements, you must specify either SOLID92 or 92 for the value of ELEM2.
- Optionally, you can use the ETYPE2 argument to specify the element
TYPE number for ELEM2. To continue with our example, to assign
element TYPE number 2 to the newly-converted SOLID92 elements,
specify 2 for the value of ETYPE2.
Also see the description of the TCHG
command in the ANSYS Commands Reference.
If you are using the ANSYS GUI to perform the conversion, follow these steps:
1. Choose menu path Main Menu>Preprocessor>-Meshing-Modify Mesh>
Change Tets. The Change Selected Degenerate Hexes to
Non-degenerate Tets dialog box appears.
2. Using the Change From option menu, select a combination of elements.
3. In the TYPE number for ELEM2 field, select the appropriate element TYPE
number for ELEM2. (A single-selection list containing all of the currently
defined element types, along with their corresponding element TYPE
numbers, appears on the dialog box to help you make your selection.) To
make your selection, you can do any one of the following:
- Choose NEXT AVAIL TYPE# from the selection list and click on OK, and
ANSYS uses the next available location in the element attribute tables to
determine the element TYPE number for ELEM2 or, if ELEM2 already
appears in the element attribute tables, ANSYS uses ELEM2's existing
element TYPE number for ETYPE2.
- Choose USER SPECIFIED from the selection list and click on OK. A
second dialog box appears, where you must enter an element TYPE
number and click on OK. ANSYS assigns the element TYPE number
that you enter to ELEM2.
- Choose a valid element TYPE number (if one is available) from the
selection list. Remember that even though all of the currently defined
element types and their assigned element TYPE numbers appear in the
list, not all of them are valid choices (for example, if you are converting
SOLID95 elements to SOLID92 elements, you must choose the
TYPE number for the defined SOLID92
element from the selection list). If no SOLID92 elements are currently defined,
then you have to use one of the other selection methods described
above. Assuming that a valid element TYPE number is available and
you select it, ANSYS will assign that TYPE number to the
188.8.131.52 Other Characteristics of Degenerate Tetrahedral Element
Other characteristics of degenerate tetrahedral element conversions include the
- As a result of the conversion operation, only selected elements of type
ELEM1 are converted to type ELEM2. ANSYS ignores any elements that
are type ELEM1 but are not degenerate tetrahedra; for instance, ANSYS
will ignore SOLID95 elements that have a
hexahedral, pyramidal, or prism shape. For example, assume that you
have a simple model that contains only SOLID95 elements. Some of these elements
are hexahedral, some are tetrahedral, and some are pyramidal. If you
issue the command TCHG,95,92,2,
ANSYS converts only the tetrahedral SOLID95 elements to SOLID92 elements; it leaves the hexahedral
and pyramidal SOLID95 elements
untouched. Since you specified 2 as the value of ETYPE2, ANSYS assigns
element TYPE number 2 to the SOLID92
- Performing a conversion is likely to create circumstances in which more
than one element type is defined for a single volume. Currently, ANSYS
has no way of storing more than one element type per volume. This
limitation may result in incorrect information when you perform a volume
listing operation [VLIST command].
The output listing will fail to indicate that the element type of the converted
elements has changed. Instead, it will indicate the element TYPE number
that was originally assigned to those elements. (On the other hand, the
output of an element listing operation [ELIST command] will indicate the new
element TYPE number.) If you plan to perform a conversion, we
recommend that the conversion be your last step in the modeling and
meshing process; that is, complete any desired mesh refinement, moving
or copying of nodes and elements, and any other desired modeling and
meshing revision processes prior to beginning the conversion.
7.3.11 Doing Layer Meshing
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.
- Uniform (or moderately varying) element size along the line.
- Steep transitions in element size and number in the direction normal to the
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.
- The desired element size on the line, either by setting the element size
directly (SIZE), or by setting the number of line divisions (NDIV).
- The line spacing ratio (SPACE, normally 1.0 for layer meshing).
- The thickness of the inner mesh layer (LAYER1). Elements in this layer will
be uniformly-sized, with edge lengths equal to the specified element size
on the line. LAYER1's thickness may be specified with either a factor on
the element size for the line (size factor = 2 produces two rows of
uniformly-sized elements along the line; size factor = 3, three rows, etc.),
or with an absolute length.
- The thickness of the outer mesh layer (LAYER2). The size of elements in
this layer will gradually increase from those in LAYER1 to the global
element size. LAYER2's thickness may be specified with either a mesh
transition factor (transition factor = 2 produces elements which
approximately double in size as the mesh front progresses normal to the
line; transition factor = 3, triple in size, etc.), or with an absolute length.
Note-LAYER2's "thickness" is really the distance over which mesh transition
must occur between elements of LAYER1 size and the global size. Appropriate
values for LAYER2 thus depend on the magnitude of the global-to-LAYER1 size
ratio. If you use a mesh transition factor to specify LAYER2, it must be greater
than 1.0 (implying the next row's size must be larger than the previous) and, for
best results, should be less than 4.0.
Note-For a picked set of lines, layer mesh controls may be set or cleared without
altering the existing line divisions or spacing ratio settings for those lines. In fact,
within this dialog box, blank or zero settings for SIZE/NDIV, SPACE, LAYER1, or
LAYER2 will remain the same (that is, they will not be set to zero or default
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
7.3.14 Listing Layer Mesh Specifications on Lines
To view or print layer meshing size specifications on lines, use one of the
7.4 Controls Used for Free and Mapped
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:
Main Menu>Preprocessor>-Meshing-Mesher Opts
You must also specify that free meshing should be used to mesh the model:
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>
184.108.40.206 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
For more information, see Chapter 9 of the ANSYS Structural Analysis Guide and the
description of the TARGE170 element in the ANSYS Elements Reference.
- You must be meshing a three-sided area. Two of the sides must have only
one element division; the third side can have any number of divisions.
- You must be meshing with the TARGE170
- You must specify that free meshing be used [MSHKEY,0 or MSHKEY,2].
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
Note-Mapped meshing is not supported when hard points are used.
220.127.116.11 Area Mapped Meshing
An area mapped mesh consists of either all quadrilateral elements or all triangular
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
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
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
Figure 7-17 Transferred LESIZE
controls override ESIZE
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
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:
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:
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
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
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
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
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
18.104.22.168 Volume Mapped Meshing
To mesh a volume with all hexahedron elements, the following conditions must be
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
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
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:
! next, concatenate lines for mapped meshing of bounding areas:
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
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:
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
To add areas, use one of the following methods:
Please see the ACCAT, LCCAT, and VMESH command descriptions for more
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 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
22.214.171.124 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:
- The fastest way to delete concatenated lines or areas is by choosing menu
path Main Menu>Preprocessor>-Modeling-Delete>-Del Concats
-Lines or Main Menu>Preprocessor>-Modeling-Delete>-Del Concats
Warning: When you use this method, ANSYS automatically selects all
concatenated lines (or areas) and deletes them without prompting you.
- If you want more control over which concatenated lines or areas are
selected and deleted, use one of these methods:
LSEL,Type,LCCA,,,,,KSWP or ASEL,Type,ACCA,,,,,KSWP
If you are using the Select Entities dialog box, choose both Lines and
Concatenated to select concatenated lines. Choose both Areas and
Concatenated to select concatenated areas. If desired, use the other
controls in the dialog box to refine your selection.
You can then delete all of the selected lines or areas [LDELE,ALL or ADELE,ALL] as necessary.
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 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
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.
- To generate point elements (such as MASS21) at keypoints:
- To generate line elements (such as LINK31)
Also see Section 7.5.2 for information about special beam meshing
- To generate area elements (such as PLANE82) on areas:
3 or 4 sided
Main Menu>Preprocessor>-Meshing-Mesh>-Areas-Target Surf
- To generate volume elements (such as SOLID90) in volumes:
4 to 6 sided
Also see Section 7.5.3 and Section 7.5.5 for information about special
volume meshing procedures.
7.5.2 Generating a Beam Mesh With Orientation Nodes
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:
Main Menu>Preprocessor>-Attributes-Define>All Lines
Main Menu>Preprocessor>-Attributes-Define>Picked Lines
126.96.36.199 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
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).
188.8.131.52 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 184.108.40.206 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.
220.127.116.11 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
- When specifying a value for the TYPE argument on the LATT command, be sure that the
element type you assign to the line is one that supports beam meshing
with orientation. Currently, this list includes BEAM4, BEAM24, BEAM44, BEAM161, BEAM188, and BEAM189.
- Use the KB and KE arguments on the LATT command to assign beginning
and ending orientation keypoints. If you are meshing with BEAM24, BEAM161, BEAM188, or BEAM189 elements, you are required to
define at least one orientation keypoint when you set your attributes for
meshing. When ANSYS generates the mesh [LMESH], each beam element along
the line will have two end nodes and one orientation node. Specifying
orientation keypoints when meshing with BEAM4 and BEAM44 elements is optional. If you specify
orientation keypoints for these elements, each beam element along the
meshed line will have two end nodes and one orientation node. If you
do not specify orientation keypoints for BEAM4 and BEAM44, each beam element will have two
end nodes, but no orientation node (that is, ANSYS will generate the
mesh using standard line meshing).
- If you are using BEAM188 elements or
BEAM189 elements, use the SECNUM
argument on the LATT command to
assign a section ID number.
4. Use the LMESH command to mesh
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
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
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.
18.104.22.168 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
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
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
- In Figure 7-30 (a), only a beginning orientation keypoint was assigned. The
keypoint is 0° from the y axis at a distance of 10 units in the y direction.
The beam exhibits constant orientation.
- In Figure 7-30 (b), only a beginning orientation keypoint was assigned. The
keypoint is 30° from the y axis at a radius of 10 units. The beam exhibits
- In Figure 7-30 (c), both a beginning and an ending orientation keypoint
were assigned. The keypoints are 90° apart, causing a 90° twist in the
beam. Due to the linear interpolation that is used to determine the location
of the orientation nodes, a line biasing with small divisions at each end was
used to cause the nodes to be located closer to the vectors made by the
- In Figure 7-30 (d), the orientation keypoints are 180° apart, and this time
the beam flips. Assigning these keypoints causes a discontinuity because
the interpolation of the two vectors is linear.
- Figure 7-30 (e) provides a remedy to the problem illustrated in Figure 7-30
(d). Here one line was divided into two, with the ending orientation
keypoint for L1 and the beginning orientation keypoint for L2 being
assigned to the same keypoint. A 180° twist is achieved.
22.214.171.124 Other Considerations for Beam Meshing With Orientation
Other things to consider when meshing beams with orientation nodes include the
- Caution: If you issue the CDWRITE command after
generating a beam mesh with orientation nodes, the database file will
contain all of the nodes for every beam element, including the orientation
nodes. However, the orientation keypoints that were specified for the line
[LATT] are no longer associated with
the line and are not written out to the geometry file. The line does not
recognize that orientation keypoints were ever assigned to it, and the
orientation keypoints do not "know" that they are orientation keypoints.
Thus, the CDWRITE command
does not support (for beam meshing) any operation that relies on solid
model associativity. For example, meshing the areas adjacent to the
meshed line, plotting the line that contains orientation nodes, or clearing
the line that contains orientation nodes may not work as expected. This
limitation also exists for the IGESOUT command. See the
descriptions of the CDWRITE
command and the IGESOUT
command in the ANSYS Commands
Reference for more information.
- Since orientation is not required for 2-D beam elements, the beam
meshing procedure described in this section does not support 2-D beam
- Any operation on a line (copying the line, moving the line, and so on) will
destroy the keypoint attributes.
- If an orientation keypoint is deleted, ANSYS issues a warning message.
- If an orientation keypoint is moved, it remains an orientation keypoint.
However, if an orientation keypoint is redefined (K,NPT,X,Y,Z), ANSYS no longer recognizes it
as an orientation keypoint.
7.5.3 Generating a Volume Mesh From Facets
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:
Main Menu>Preprocessor>-Meshing-Mesh>-Tet Mesh From-Area
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
Additional considerations for using xMESH commands include the following:
- Sometimes you may need to mesh the solid model with a variety of
elements of different dimensionalities. For example, you may need to
"reinforce" a shell model (area elements) with beams (line elements), or
overlay one of the faces of a 3-D solid model (volume elements) with
surface effect (area) elements. You can do so by using the appropriate
meshing operations [KMESH, LMESH, AMESH, and VMESH] in any desired order. Make
sure, however, that you set the appropriate element attributes (discussed
earlier in this chapter) before meshing.
- No matter which volume mesher you choose [MOPT,VMESH,Value], it may produce
different meshes on different hardware platforms when meshing volumes
with tetrahedral elements [VMESH,
FVMESH]. Therefore, you should
be cautious when evaluating results at a specific node or element. The
location of these entities may change if the input created on one platform is
later run on a different platform.
- The adaptive meshing macro [ADAPT] is an alternative meshing
method that automatically refines the mesh based on mesh discretization
errors. See Chapter 3 of the ANSYS
Advanced Analysis Techniques Guide for more information on this
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.
126.96.36.199 Benefits of Volume Sweeping
Volume sweeping provides these benefits:
- Unlike other methods for extruding a meshed area into a meshed volume
[VROTAT, VEXT, VOFFST, and VDRAG commands], volume sweeping
[VSWEEP] is intended for use in
existing unmeshed volumes. Thus it is particularly useful in these
- You have imported a solid model that was created in another program,
and you want to mesh it in ANSYS.
- You want to create a hexahedral mesh for an irregular volume. You now
only have to break up the volume into a series of discrete sweepable
regions, as opposed to in the past, when it was necessary for you to
break up the volume into discrete map-meshable regions.
- You either want to create a different mesh than the one that was created
by one of the other extrusion methods, or you forgot to create a mesh
during one of those operations.
- Volume sweeping allows you to use any area elements to mesh the source
area. The other extrusion methods mentioned above require the initial area
mesh to be a mesh of shell elements.
- If you do not mesh the source area prior to volume sweeping, ANSYS
meshes it for you when you invoke the volume sweeper. The other
extrusion methods require you to mesh the area yourself before you invoke
them. If you do not, the other extrusion methods create the volume, but no
area or volume mesh is generated.
188.8.131.52 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:
- One or more of the volume's side areas contains more than one loop; in
other words, there is a hole in a side area.
- The volume contains more than one shell; in other words, there is an
internal void within the volume. (A shell is the volumetric equivalent of
an area loop-a set of entities that defines a continuous closed
boundary. The SHELL column in a volume listing [VLIST] indicates the number of shells
in the volume.)
- The source area and the target area are not opposite one another in the
volume's topology. (By definition, the target area must be opposite the
Note-Even if you have satisfied these requirements, there may be times
when the shape of a volume causes the volume sweeper to create poorly
shaped elements. For help, see Section 184.108.40.206.
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:
- Use the EXTOPT,ESIZE,Val1,Val2
command to specify the number of element divisions (and if desired, the
spacing ratio or bias) to be used along the volume's side lines (where
Val1 is the number of element divisions and Val2 is the bias). Note that
the number of element divisions and bias that you specify with EXTOPT will apply to all of the
volume's unmeshed side lines. For any side line that has been
pre-meshed or that has other sizing specifications associated with it (via
LESIZE), the values set by EXTOPT are ignored. Using the EXTOPT command or its menu
path is the preferred method for setting these values.
Main Menu>Preprocessor>-Meshing-Mesh>-Volume Sweep-Sweep
Figure 7-31 Specifying number of element divisions, source area, and
target area for volume sweeping
- On one or more of the volume's side lines, use the LESIZE command to specify the
number of element divisions for that particular line. This method also
permits you to specify a bias that the volume sweeper will honor [LESIZE,,,,,SPACE]; however, the
bias applies only to the line that you identify on the LESIZE command. Regardless of
how element divisions are set for all of the other side lines (for example,
through pre-meshing or additional LESIZE specifications), all of the
volume's side lines must have the same number of element divisions.
- Generate a mapped mesh on one of the side areas or within a volume or
area that is adjacent to a side area or side line.
- Generate a mesh of beam elements on one of the side lines [LMESH].
4. Determine which of the areas bounding the volume will be the source area,
and which will be the target area. ANSYS uses the pattern of the area
elements on the source area (which can be quadrilateral and/or triangular
elements) to fill the volume with hexahedral and/or wedge elements. (If
you have not pre-meshed the area prior to volume sweeping, ANSYS
automatically generates "temporary" area elements. It does not save these
area elements in the database; they are discarded as soon as the pattern
for the swept volume is determined.) The target area is simply the area
that is opposite the source area. See Figure 7-31 above, which illustrates
one way that a user might set the element divisions, source area, and
target area for a volume sweeping operation.
Note-In some cases, your choice of source and target areas will
determine whether the sweeping operation succeeds or fails. See Section
220.127.116.11 for details.
5. Optionally, mesh the source, target, and/or side area(s).
The results of a volume sweeping operation will differ depending on
whether you have meshed any of the areas (source, target, and/or side
areas) in your model prior to sweeping.
Typically, you will generate a mesh for the source area yourself, before you
sweep the volume. If you have not meshed the source area, ANSYS will
mesh it internally when you invoke the volume sweeping operation (as
described above in Step 4.
Consider the following information when deciding whether to "pre-mesh"
- If you want the source area to be meshed with a mapped quadrilateral
mesh or a mapped triangle mesh, pre-mesh.
- If you want the source area to be meshed with smart element sizing [SMRTSIZE], pre-mesh.
- If you do not pre-mesh, ANSYS always uses the free mesher to
generate the mesh. (On simple areas, the free mesh that ANSYS
generates may be identical to the mapped mesh it would have
generated using the mapped mesher, but this is not guaranteed.)
- If you do not pre-mesh, ANSYS uses the element shape setting [MSHAPE] to determine the
element shape it uses to mesh the source area (MSHAPE,0,2D results in
quadrilateral elements; MSHAPE,1,2D results in triangular
- The sweeping operation will fail if hard points are present on an area or
line that is associated with the volume, unless you pre-mesh the area or
line containing the hard point.
- If you pre-mesh both the source area and the target area, the area
meshes must match. However, the source area mesh and the target
area mesh do not have to be mapped meshes.
- Prior to sweeping, all of the volume's side areas must be either map
meshed or 4-sided. (There is an exception to this rule: You must
always pre-mesh-with a mapped mesh-any 4-sided area that started
out with more than 4 sides and then became 4-sided as a result of line
concatenation.) In addition, one line of each unmeshed side area must
be on the source area, and one line must be on the target area.
Figure 7-32 Sweeping a volume with different source and target area
- The sweeping operation will succeed when the topology of the source
area is different from the topology of the target area, as long as you
pre-mesh (with a mapped mesh) those side areas of the volume that are
causing the topology of the source area and the target area to differ.
See Figure 7-32 for an example.
See Section 18.104.22.168 for more information about the characteristics of the
volume sweeping feature.
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
22.214.171.124 Invoking the Volume Sweeper
To invoke the volume sweeper:
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.
- Use the VNUM argument to identify the volume that you want to sweep.
- Use the SRCA argument to identify the source area.
- Use the TRGA argument to identify the target area.
- Optionally, use the LSMO argument to specify whether ANSYS should
perform line smoothing during the sweeping operation.
If you are using the ANSYS GUI to sweep a volume, follow these steps:
1. Choose menu path Main Menu>Preprocessor>-Meshing-Mesh>
-Volume Sweep-Sweep. The Volume Sweeping picker appears.
2. Pick the volume that you want to sweep and click on Apply.
3. Pick the source area and click on Apply.
4. Pick the target area. Click on OK to close the picker.
Note-When using the ANSYS GUI to sweep a volume, you cannot control
whether line smoothing occurs. ANSYS does not perform line smoothing when
volume sweeping is invoked from the GUI.
126.96.36.199 Strategies for Avoiding Shape Failures During Volume
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
3. Use shape checking as a diagnostic tool to determine which region of the
model is causing the sweep failure. To do this, reduce the shape checking
level to warning mode [SHPP,WARN],
so that elements that violate error limits result in warning messages rather
than element failures. Then reinvoke the sweeping operation. Use the
resulting warning messages to identify the region of the model that contains
the bad elements, and then clear the bad element mesh [VCLEAR]. Turn shape checking back
on [SHPP,ON]. Next, modify the
region of the model that contained the bad elements. Finally, mesh the
volume again with a subsequent sweep operation. Here are some
suggestions for modifying the model:
- Divide the volume into two or more volumes [VSBA,VSBW], which will shorten the length
of the sweep direction. Try dividing the volume near the region where
the poorly shaped elements occur. Afterwards, invoke VSWEEP for each of the resulting
- If the elements flagged by SHPP,WARN appear to be stretched
within thin sections of the target area as in Figure 7-34 (c), try dividing
the side areas in that region along the direction of the sweep. Use these
2. Divide one of the lines on the source area and one of the lines on
the target area by adding keypoints at the desired division
locations [LDIV]. See Figure
3. Copy the line divisions from the new lines on the source area to
the corresponding new lines on the target area as described in
Figure 7-34 (e). (The "new lines" are those that were created by
Step 2.) You can copy line divisions easily via the MeshTool.
Choose menu path Main Menu>Preprocessor>MeshTool. On
the MeshTool, press the Copy button to open the picker. Use the
picker to copy the line divisions-including spacing ratios-from
one line to the other.
4. Manually map mesh the side area that was affected by Step 2.
See Figure 7-34 (f).
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
5. Reinvoke the volume sweeper.
Figure 7-34 (c), Figure 7-34 (d), and Figure 7-34 (g) show the results of three
different sweeping operations, and illustrate how you can use some of the
strategies described above to affect the quality of a swept mesh. In all three
cases, the user started with the same volume, which is shown in Figure 7-34 (a).
Figure 7-34 (b) illustrates the source mesh that was used during the sweep.
Again, in all three cases, the user generated this source mesh prior to invoking
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
Figure 7-34 Strategies for avoiding stretched elements
188.8.131.52 Other Characteristics of Volume Sweeping
Other characteristics of volume sweeping include the following:
- The source area and the target area do not have to be flat or parallel.
- If the topology of the source area and the topology of the target area are
the same, the sweeping operation will often succeed even if the shape of
the source area is different from the shape of the target area. However,
drastically different shapes can cause element shape failures.
- During volume sweeping, ANSYS can create either linear or quadratic
elements. It can sweep quadratic area elements into linear volume
elements, and it can sweep linear area elements into quadratic volume
elements. (However, when ANSYS sweeps linear area elements into
quadratic volume elements, mid-nodes are not added to the edges of the
source area. This will result in an element shape failure if you are using
quadratic volume elements that do not support dropped mid-nodes.)
- If you have pre-meshed the source, target, and/or side areas, you can
issue the EXTOPT,ACLEAR,1
command prior to sweeping and ANSYS will automatically clear the area
elements from any selected source, target, or side area after the swept
volume mesh is created. (Note-In the GUI, choose menu path Main
Menu> Preprocessor>-Meshing-Mesh> -Volume Sweep-Sweep Opts
to access a dialog box where you can toggle this clearing option on and
off.) The areas that you want to clear must be selected for clearing of the
area meshes to occur.
- Volume sweeping does not require your model to have a constant cross
section. However, if the cross section varies, it should vary linearly from
one end of the sweep to the other for best results.
- During volume sweeping, ANSYS ignores any settings that are specified for
the SMRTSIZE command.
However, if you do not pre-mesh the source area, ANSYS will use the KESIZE, ESIZE, or DESIZE command setting (as
appropriate) to mesh the source area. Also note the following information
about the ESIZE command. The ESIZE,,NDIV setting may be used to
determine the number of element divisions that will be created along the
volume's side lines during sweeping. However, this is not the preferred
method because if the source area is not pre-meshed, the number of
element divisions specified by NDIV will apply to all of the source area lines
as well. The preferred method is to use the EXTOPT command (as described
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
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
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:
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.
- Turn element shape checking off entirely or to warning-only mode
- Turn individual shape tests off and on
- View a summary of shape test results
- View current shape parameter limits
- Change shape parameter limits
- Retrieve element shape parameter data
- Understand the circumstances under which ANSYS retests existing
elements, and why doing so is necessary
- Decide whether element shapes are acceptable
184.108.40.206 Turning Element Shape Checking Off Entirely or to
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:
- When you are generating an area mesh [AMESH], but your ultimate intention is
to generate a volume mesh [VMESH] of quadratic tetrahedrons with
that area as one of the volume's faces. Note that the tetrahedra mesher
can fix meshes in which area elements have poor Jacobian ratios. Thus, if
you are generating an area mesh for an area that will be a face on a
volume in a subsequent volume meshing operation, it may make sense to
turn element shape checking to warning-only mode, mesh the area, turn
element shape checking on, and then mesh the volume.
- When you are importing a mesh [CDREAD]. If "bad" elements exist in
a mesh that you want to import and element shape checking is turned on,
ANSYS may bring the mesh into the database with "holes" where the bad
elements should be (or it may not import the mesh at all). Since neither of
these outcomes is desirable, you may want to turn element shape checking
either off or to warning-only mode prior to importing a mesh. After you
import, we suggest that you turn shape checking back on and recheck the
elements [CHECK,ESEL,WARN or
Note-Once elements are in the database, performing element shape
checking will not delete them. If any elements in violation of error limits are
selected when you initiate a solution [SOLVE], ANSYS issues an error
message and does not process the solution.
- When you are using direct generation and you are creating elements that
you know will be temporarily invalid. For example, you may be creating a
wedge-shaped element that has coincident nodes. You know that you
need to merge the coincident nodes [NUMMRG] in order to get valid
elements. In this case, it would make sense to turn off element shape
checking, complete the desired operations (such as merging nodes in this
example), turn element shape checking on, and then check the elements
for completeness [CHECK].
220.127.116.11 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
For example, the command SHPP,OFF,WARP turns off all warping factor
- Use the Lab argument to indicate whether you want to turn tests off or on.
Specify OFF to turn tests off; specify ON to turn tests on.
- Use the VALUE1 argument to indicate which tests you want to turn off or
on. You can specify ANGD (SHELL28
corner angle deviation tests), ASPECT (aspect ratio tests), PARAL
(deviation from parallelism of opposite edges tests), MAXANG (maximum
corner angle tests), JACRAT (Jacobian ratio tests), or WARP (warping
factor tests). You can also specify ALL to turn all tests off or on.
In the GUI, you can toggle the tests off and on by choosing menu path Main
Menu>Preprocessor>Checking Ctrls>Toggle Checks. When the Toggle Shape
Checks dialog box appears, click the individual tests off or on as desired; then
click on OK.
18.104.22.168 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 %
22.214.171.124 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 126.96.36.199 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
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
WARNING TOLERANCE (31) = 30.00000
ERROR TOLERANCE (32) = 1000.000
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
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
188.8.131.52 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:
- Perhaps you are not particularly concerned about aspect ratio measures.
You can turn off all aspect ratio testing by including the command SHPP,OFF,ASPECT in your
START5x.ANS file. If that seems too drastic for your situation, you may
choose to specify SHPP,MODIFY,1,1000 instead. Doing so
radically loosens the warning limit for aspect ratio tests, without turning off
the tests entirely.
- Suppose that you are using the sequential method of coupled-field
analysis to perform a thermal-stress analysis. You plan to use SHELL57 elements for the thermal analysis
first, and then SHELL63 elements (with
nonlinear geometry on) for the structural analysis. If you build your model
initially with SHELL57 elements, ANSYS will
test the elements against loose warping limits (that is, a warning tolerance
of 0.1, and an error tolerance of 1.0-refer to the sample output provided in
Section 184.108.40.206 for a complete list of default limits). In contrast, the default
warping limits for SHELL63 elements with
nonlinear geometry on are very tight (a warning tolerance of 0.00001, and
an error tolerance of 0.01). Since ANSYS will test the elements against
loose limits for the thermal analysis, the tests may not turn up any elements
that are in violation of the nonlinear SHELL63 limits. However, for the structural
analysis, ANSYS will test the elements again when you switch the element
type to SHELL63 [ETCHG,TTS] and turn on nonlinear
Because the limits will be much tighter for the second analysis, elements
that caused no problems for the thermal analysis may produce warnings or
errors in the structural analysis. You might be faced with a choice between
a) accepting poor structural elements, which could compromise the quality
of your analysis results, or b) revising the mesh and starting over with a
new thermal solution. One way to prevent this situation is to build the
model initially with SHELL63 elements with
NLGEOM on; switch to SHELL57 elements for the thermal solution;
then switch back to SHELL63 elements for
the structural solution. Another alternative is for you to reset the warping
limits for SHELL57 elements as tight as
those for SHELL63 elements with NLGEOM on. You could accomplish
this with the commands SHPP,MODIFY,53,0.00001 and SHPP,MODIFY,54,0.01.
220.127.116.11 Retrieving Element Shape Parameter Data
You can use the *GET and *VGET commands to retrieve element shape
*GET, Par, ELEM, ENTNUM, SHPAR,
Note-You cannot use the GUI paths for these commands to retrieve element
shape parameter data.
*VGET, ParR, ELEM, ENTNUM,
SHPAR, IT1NUM,,, KLOOP
For example, the command *GET,A,ELEM,3,SHPAR,ASPE returns the
calculated aspect ratio of element number 3 and stores it in a parameter named
A. The command *VGET,A(1),ELEM,3,SHPAR,ASPE returns the
aspect ratio of element number 3 and stores it in the first location of A. Retrieval
continues with elements numbered 4, 5, 6, and so on, until successive array
locations are filled.
See the descriptions of the *GET and *VGET commands in the ANSYS Commands Reference for more information.
18.104.22.168 Understanding Circumstances Under Which ANSYS Retests
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
- When you change the element type [ET,,Ename or ETCHG,Cnv] or one of its key options
- When you change the element TYPE number of an element [EMODIF].
- When you change the large deformation key [NLGEOM,Key] for SHELL63 elements.
- When you define a shell thickness [R]
after you define an element, or you change an existing shell thickness [RMODIF] or the REAL number of a
shell element [EMODIF].
22.214.171.124 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).
- Never ignore an element shape warning. Always investigate the effect that
a "poorly" shaped element might have on your analysis results.
- Recognize that structural stress analyses that have the goal of determining
stress at particular locations will typically suffer more severe effects from
"poorly" shaped elements than will other types of analyses (deflection or
nominal stress, modal, thermal, magnetic, etc.).
- If any "poorly" shaped elements are located in a critical region (such as
near a critical stress point), their effect is more likely to be detrimental.
- "Poorly" shaped higher-order (midside-noded) elements will generally
produce better results than will similarly shaped linear elements. The
default ANSYS shape parameter limits are more restrictive on linear
elements than on higher-order elements.
- Verification of analysis results by comparison with other analyses, test data,
or hand calculations is essential regardless of whether elements produce
shape warnings. If such verification indicates that you have high-quality
results, there is little reason to worry about shape warnings.
- Some of the best quantitative measures of an element's acceptability are
the error measures based on the element-to-element discontinuity in a
stress or thermal gradient field. (See Chapter 5 of the ANSYS Basic Analysis Procedures Guide. An
element that produces shape warnings and shows a high error measure
compared to its neighbors is suspect.)
Refer to the description of the SHPP
command in the ANSYS Commands Reference
for more information about element shape checking.
7.6 Changing the Mesh
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.
- Remesh with new element size specifications.
- Use the accept/reject prompt to discard the mesh, then remesh.
- Clear the mesh, redefine mesh controls, and remesh.
- Refine the mesh locally.
- Improve the mesh (for tetrahedral element meshes only).
7.6.1 Remeshing the Model
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
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.
- The level of refinement to be done (in other words, the desired size of the
elements in the refinement region, relative to the size of the original
- The depth of surrounding elements that will be remeshed, in terms of the
number of elements outward from the selected entity
- The type of postprocessing to be done after the original elements are split
(smoothing and cleaning, smoothing only, or neither)
- Whether triangles can be introduced into the mesh during the refinement of
an otherwise all-quadrilateral mesh
7.6.5 Improving the Mesh (Tetrahedral Element Meshes Only)
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.
126.96.36.199 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 188.8.131.52,
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
184.108.40.206 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.
- When tetrahedra improvement is invoked automatically during a volume
meshing operation [VMESH],
ANSYS uses a linear tetrahedral shape metric for improvement. This
means that ANSYS ignores midside nodes that may be present within the
elements. However, when you request tetrahedra improvement of a given
mesh as documented below, ANSYS takes the midside nodes into account.
Thus, for meshes of quadratic (midside-noded) tetrahedral elements,
requesting additional tetrahedra improvement [VIMP] after the mesh is created [VMESH] can help to remove, or at least
reduce, the number of element shape test warning messages that are
produced and to improve the overall quality of the mesh.
- Since imported tetrahedral meshes have not received the benefits of the
tetrahedral mesh improvement that ANSYS often performs automatically,
imported tetrahedral meshes are likely candidates for user-invoked
You can request improvement of two "types" of tetrahedral elements:
- You can request improvement of tetrahedral elements that are not
associated with a volume. (Typically, this option is useful for an imported
tetrahedral mesh for which no geometry information is attached.) Use one
of these methods:
Main Menu>Preprocessor>-Meshing-Modify Mesh>Improve Tets>
- You can request improvement of tetrahedral elements that are in a selected
volume or volumes. (You might want to use this option to further improve a
volume mesh created in ANSYS [VMESH].) Use one of these methods:
Main Menu>Preprocessor>-Meshing-Modify Mesh>Improve Tets>
220.127.116.11 Restrictions on Tetrahedral Mesh Improvement
The following restrictions apply to tetrahedral mesh improvement:
- The mesh must consist of either all linear elements or all quadratic
- For all of the elements in the mesh to be eligible for tetrahedral mesh
improvement, they must all have the same attributes, including element
type. (The element type must be tetrahedral, but the tetrahedral elements
may be the degenerated form of hexahedral elements.) After tetrahedral
mesh improvement, ANSYS reassigns the attributes from the old set of
elements to the new set of elements.
Note-Tetrahedral mesh improvement is possible in a mesh of mixed
element shapes (as opposed to types). For example, as stated earlier,
improvement occurs automatically during the creation of transitional
pyramid elements at the interface between hexahedral and tetrahedral
element types. However, in a mixed mesh, only the tetrahedral elements
- Loading has an effect on whether tetrahedral mesh improvement is
possible. Tetrahedral mesh improvement is possible when loading occurs
in either of these ways:
- When loads have been applied to the element faces or nodes on the
boundary of the volume only
- When loads have been applied to the solid model (and have been
transferred to the finite element mesh)
Tetrahedral mesh improvement is not possible when loading occurs in
either of these ways:
- When loads have been applied to the element faces or nodes within the
interior of a volume
- When loads have been applied to the solid model (and have been
transferred to the finite element mesh), but have also been applied to the
element faces or nodes within the interior of a volume
Note-In the last two loading situations, ANSYS issues a warning message
to notify you that you must remove the loads if you want tetrahedral mesh
improvement to occur.
- If node or element components are defined, you will be asked whether you
want to proceed with mesh improvement. If you choose to proceed, you
must update any affected components.
18.104.22.168 Other Characteristics of Tetrahedral Mesh Improvement
Other characteristics of tetrahedral mesh improvement include:
Please see the TIMP and VIMP command descriptions for more
- Element numbering and node numbering are modified.
- Generally, if ANSYS encounters an error or a user abort occurs, it leaves
the mesh unchanged. However, ANSYS may save a partially improved
mesh after an abort if you verify the save when ANSYS prompts you. If
you have requested improvement for multiple volumes [VIMP], the abort applies only to the
current volume mesh that is being improved; all previously improved
volume meshes are already saved. (The same applies when an error
occurs after the first of multiple volumes is improved.)
7.7 Some Hints and Cautions
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
7.7.2 Further Hints
- A tetrahedron meshing failure can be quite time consuming. One relatively
quick way that you can make a preliminary check for a possible tetrahedron
meshing failure is by meshing the surfaces of a volume with six-noded
triangles. If this surface triangle mesh contains no sudden size transitions
(admittedly often a difficult judgement) and produces no curvature or
aspect ratio warnings, tetrahedron meshing failure is much less likely than
if these conditions are not met. (Be sure to clear or deactivate the triangle
elements before using the analysis model.)
- Avoid subtracting meshed entities from your model whenever possible.
However, if you subtract entities that have been meshed and an
undesirable mesh mismatch results, you can recover by clearing the mesh
and remeshing the entities.
Go to the beginning of this chapter