Go to the Next Chapter
Go to the Previous Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index
Chapter 1 *
Chapter 2 *
Chapter 3 *
Chapter 4 *
Chapter 5 *
Chapter 6 *
Chapter 7 *
Chapter 8 *
Chapter 9 *
Chapter 10 *
Chapter 11 *
Chapter 12 *
Chapter 13 *
Chapter 14
8.1 Introduction
This chapter describes various methods you can use to revise your model. Topics
include:
- Refining a mesh locally
- Moving and copying nodes and elements
- Keeping track of element faces and orientations
- Revising a meshed model: clearing and deleting
- Understanding solid model cross-reference checking
8.2 Refining a Mesh Locally
There are generally two situations in which you may want to refine a mesh in a
local region: 1) you have meshed a model and you would like a finer mesh in
specific regions of the model, or 2) you have completed the analysis and, based
on the results, would like a more detailed solution in a region of interest. For all
area meshes and for volume meshes composed of tetrahedra, the ANSYS
program allows you to refine the mesh locally around specified nodes, elements,
keypoints, lines, or areas. Meshes composed of volume elements other than
tetrahedra (for example, hexahedra, wedges, and pyramids) cannot be locally
refined.
8.2.1 How to Refine a Mesh
You must follow these two steps to refine a mesh:
1. Select the entity (or set of entities) around which refinement will be done.
2. Specify the level of refinement to be done (in other words, the desired size
of the elements in the refinement region, relative to the size of the original
elements). The refined elements will always be smaller than the original
elements; the local mesh refinement process does not provide mesh
coarsening (LEVEL).
8.2.1.1 Advanced Controls
If you prefer to have more control over the refinement process, you can also set
values for any of the following advanced options:
- You can specify the depth of the mesh refinement region in terms of the
number of elements outward from the indicated entities (DEPTH).
- You can specify the type of postprocessing to be done after the original
elements are split. Postprocessing may include both smoothing and
cleaning, smoothing only, or neither one (POST).
- You can specify whether triangles can be introduced into the mesh during
the refinement of an otherwise all-quadrilateral mesh. In other words, you
can indicate whether quadrilateral elements must be retained (RETAIN).
8.2.2 Refinement Commands and Menu Paths
Use the following xREFINE commands and menu paths to select entities for
refinement and to set refinement controls. (The refinement controls are described
in detail below.)
- To refine around a selected set of nodes, use one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Modify Mesh>-Refine
At->Nodes
- To refine around a selected set of elements, use one of the following
methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Modify Mesh>-Refine
At->Elements
Main Menu>Preprocessor>-Meshing-Modify Mesh>-Refine At->All
- To refine around a selected set of keypoints, use one of the following
methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Modify Mesh>-Refine At->
Keypoints
- To refine around a selected set of lines, use one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Modify Mesh>-Refine At->Lines
- To refine around a selected set of areas, use one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Modify Mesh>-Refine
At->Areas
Figure 8-1 shows examples of mesh refinement around a node [NREFINE], element [EREFINE], keypoint [KREFINE], and line [LREFINE].
Figure 8-1 Examples of local mesh refinement
Figure 8-2 illustrates the use of the AREFINE command to perform tetrahedral
mesh refinement around an area.
Figure 8-2 Tetrahedral mesh refinement around an area [AREFINE]
8.2.2.1 Specifying the Level of Refinement
Use the LEVEL argument to specify how much refinement is to be done. The
value of LEVEL must be an integer from 1 to 5, where a value of 1 provides
minimal refinement, and a value of 5 provides maximum refinement. When
LEVEL=1, the resulting element edges in the refined region are approximately 1/2
the original edge lengths; when LEVEL=5, the resulting element edges are
approximately 1/9 the original edge lengths. The table below lists all of the
possible settings of LEVEL, along with the approximate resulting edge length for
each setting.
| Value of LEVEL Argument
|
Approximate Edge Length
|
| 1
|
1/2
|
| 2
|
1/3
|
| 3
|
1/4
|
| 4
|
1/8
|
| 5
|
1/9
|
Values of LEVEL from 1 to 5 attempt to provide gradually decreasing element
edge lengths. However, be aware that when RETAIN=ON, different values of
LEVEL may provide the same refinement. (For more information, see the
explanation of the RETAIN argument below.) Elements in the layer just outside of
the refinement region (that is, beyond the specified DEPTH) may also be split in
order to transition to the refinement elements.
Note-All values of LEVEL result in smaller elements in the refinement region.
The local mesh refinement process does not provide mesh coarsening.
8.2.2.2 Specifying the Depth of Refinement
By default, the mesh is refined one element outward from the chosen entities
(except for element refinement, which uses DEPTH=0 as the default), and the
elements are split one time (that is, the element edges are divided in half, since
LEVEL=1 by default).
8.2.2.3 Specifying Postprocessing for the Refinement Region:
Smoothing and Cleanup
As part of the refinement process, you can specify the type of postprocessing
ANSYS does after the original elements are split. You can choose smoothing and
cleaning (the default), smoothing only, or neither one.
- If you want ANSYS to do smoothing and cleaning, set POST=CLEAN (or
choose Cleanup & Smooth in the GUI).
- If you want ANSYS to do only smoothing, set POST=SMOOTH (or choose
Smooth in the GUI).
- If you do not want ANSYS to do either type of postprocessing, set
POST=OFF (or choose Off in the GUI).
Smoothing: By default, nodes in the refinement region are smoothed (that is,
their locations are adjusted) to improve the element shapes. Node locations will
be adjusted subject to the following constraints:
- Nodes at keypoints will not move.
- Nodes on lines will move only on the line.
- Nodes within areas will remain on the surface.
- If the mesh has been detached from the solid model (MODMSH,DETACH or menu path
Main Menu>Preprocessor>Checking Ctrls>Model Checking),
smoothing will not be done.
You can turn node smoothing off for all nodes by setting POST=OFF for the
refinement command being used. (Doing so turns cleanup off as well.)
Cleanup: When cleanup is turned on (POST=CLEAN), the ANSYS program
performs cleanup operations (in 2-D models) on all of the elements that are
associated with any affected geometric entities. In 3-D models, ANSYS performs
cleanup only on those elements that are in or directly adjacent to the refinement
region. Cleanup operations improve the quality of the elements. If the mesh has
been detached from the solid model, (MODMSH,DETACH or menu path Main
Menu>Preprocessor>Checking Ctrls>Model Checking), cleanup will not be
done on area meshes, but it will be done on tetrahedral volume meshes.
When you are refining a quadrilateral mesh, cleanup operations attempt to
eliminate triangles from the refinement transition region. If poorly-shaped
quadrilateral elements remain after the cleanup operations have optimized
element quality, ANSYS splits the elements into triangles. You can prevent this
splitting of quadrilateral elements by setting RETAIN=ON (the default). Figure 8-3
illustrates the cleanup of an all-quadrilateral mesh.
Note-You can turn cleanup off by setting POST=OFF or POST=SMOOTH for the
refinement command being used.
Figure 8-3 Cleanup of an all-quadrilateral mesh
8.2.2.4 Specifying Whether Quadrilateral Elements Should Be Retained
Note-The ANSYS program ignores the RETAIN argument when you are refining
anything other than a quadrilateral mesh.
By default, RETAIN=ON, which means that the refinement process will not
introduce triangular elements into an otherwise all-quadrilateral mesh. When
RETAIN=OFF and POST=SMOOTH or OFF, the resulting refinement region may
contain triangles in order to maintain transitioning. When RETAIN=OFF and
POST=CLEAN, triangles are minimized; however, they may not be completely
eliminated-a minimal number of triangles may remain in the transition region in
order to provide good element quality.
Note-If an area is meshed with a mixture of quadrilateral and triangular
elements, the quadrilateral elements will not be maintained in the refinement
region even when RETAIN=ON.
Since quadrilateral meshes are much more constrained than triangular meshes,
increasing or decreasing the value of the LEVEL argument may not provide the
desired increase or decrease in the level of refinement when RETAIN=ON. In
addition, even when quadrilateral elements can be maintained, the quality of
some of them may be poor, especially with a higher value of LEVEL. By setting
RETAIN=OFF, however, some triangles may be introduced into the mesh. This
may not be desirable, especially if you are using lower-order elements. You can
keep these triangles out of the point of interest by doing one of the following:
- Refine with a larger DEPTH; that is, at a larger radius from the point of
interest.
- Refine with POST=CLEAN. This setting for the POST argument minimizes
the number of triangles as much as possible.
- Refine using another method (for example, use local mesh controls and
remesh).
8.2.3 Transfer of Attributes and Loads
Element attributes associated with the "parent" element are automatically
transferred to all of the "child" elements. These attributes include element type,
material properties, real constants, and element coordinate systems (see Chapter
7 for details on element attributes).
Loads and boundary conditions applied to the solid model are transferred to
nodes and elements when the solution is initiated (or when loads are manually
transferred with the SBCTRAN or DTRAN commands). Therefore, solid model
loads will be correctly applied to the new nodes and elements created during
refinement. However, loads and boundary conditions applied at the node and
element level (finite element loads) cannot be transferred to new nodes and
elements created during refinement. If you have such loads in a region selected
for refinement, the program will not allow refinement to take place unless the
loads are first deleted. Therefore, it is recommended that you apply loads only to
the solid model rather than directly to nodes and elements if you anticipate using
mesh refinement.
Note-Since solid model loading is not applicable for an explicit dynamics analysis
(that is, the ANSYS/LS-DYNA product), mesh refinement must be performed
before the application of loads in this type of analysis.
8.2.4 Other Characteristics of Mesh Refinement
Other characteristics of mesh refinement include the following:
- The new elements and nodes created during refinement (including midside
nodes) are projected to the underlying solid model geometry. (See Figure
8-4.)
- When using the option to refine around nodes [NREFINE], midside nodes that are
included in the selected set are ignored.
- Mesh refinement will not cross area and volume boundaries. That is, if the
specified DEPTH goes beyond the edges of the meshed area or volume,
the adjacent area and/or volume meshes won't change (see Figure 8-5).
However, if an entity picked for refinement (node, element, keypoint, or
line) is on the boundary, or entities are picked on both sides of the
boundary, then refinement will extend into the adjacent area or volume.
- Mesh refinement will take place only in elements that are currently selected
(see Figure 8-6).
- Refinement can be used on a mesh that has been detached from the solid
model (MODMSH,DETACH or
menu path Main Menu>Preprocessor> Checking Ctrls>Model
Checking). In this case, the refinement will not be stopped by area
boundaries. Also, the nodes and elements will not be projected to the solid
model and none of the postprocessing specified with the POST argument
will be done.
- When cleanup is turned on (POST=CLEAN) during the refinement of a
tetrahedral mesh, ANSYS automatically performs a high level of cleanup
operations (that is, a level equivalent to VIMP,,,2) in the refinement region only. If
you receive shape error messages during refinement, turn off shape
checking [SHPP,OFF], perform
refinement again [xREFINE], and then request tetrahedral element
improvement at the highest level [VIMP,,,3].
- If you use the LESIZE command to
specify divisions for lines and those lines are later affected by the
refinement process, ANSYS will change the line divisions for the affected
lines (that is, the numbers of divisions on the lines not only increase, but
also show up as negative numbers in a subsequent line listing [LLIST]).
Note-The presence of the negative sign affects 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).
Figure 8-4 Nodes and elements are projected to underlying geometry
Figure 8-5 Mesh refinement will not cross area boundaries
Figure 8-6 Only selected elements are refined
8.2.5 Restrictions on Mesh Refinement
The following restrictions apply to mesh refinement:
- Although local refinement can be used for all area meshes, it can be used
for only those volume meshes that are composed of tetrahedra. Meshes
composed of volume elements other than tetrahedra (for example,
hexahedra, wedges, and pyramids) cannot be locally refined.
- If the model contains contact elements in the region selected to refine, you
cannot use local mesh refinement. In this case, refine the mesh before
defining contact elements (or, delete the contact elements, refine the mesh,
then reapply the contact elements).
- Local mesh refinement does not support elements that are generated on
the free faces of existing elements [ESURF]. Instead of using refinement
on these elements, delete the surface elements, refine the underlying
elements, and then generate the surface elements again.
- If beam elements exist adjacent to the refinement region, refinement
cannot be done. In order to refine in this area, the beam elements should
be deleted and redefined after refinement is performed.
- If loads are applied directly to the nodes and elements in a model,
refinement cannot be done. In this case, you must delete the loads in
order to refine the mesh. (To avoid this situation, it is recommended that
you apply loads to the solid model instead of the finite element model.)
- Local mesh refinement cannot be done if initial conditions at nodes [IC], coupled nodes [CP family of commands], or constraint
equations [CE family of commands] exist
in the model. If any of these exist, you must remove them before
refinement can be done.
- Local mesh refinement is not recommended for an explicit dynamics model
(that is, when using the ANSYS/LS-DYNA product) since the small
elements resulting from refinement may dramatically reduce the time step
size.
- The KSCON command is not
supported. For any area that was meshed with the KSCON command, midside nodes will
be placed at the middle of the edges when refinement is done.
- If element or node components are defined, you will be asked whether you
want to proceed with the refinement. If you choose to proceed, you must
update any affected components.
8.3 Moving and Copying Nodes and Elements
In the normal solid modeling procedure, you will ordinarily complete your entire
solid model before generating your finite element mesh. However, if repetitive
geometric features appear in your model, you might sometimes find it more
efficient to model and mesh just one representative portion of your model, and
then copy that meshed region as many times as needed to complete the model.
(It is usually much less expensive to copy an existing mesh than to generate a
new mesh.) A certain amount of forethought is generally required if you are to
accomplish this procedure successfully.
The general procedure for copying a meshed region is to use the commands for
generating and transferring areas and volumes, which are described below.
When a meshed solid model entity is copied using one of these commands, all the
attached lower-order entities, as well as the node and element mesh, are copied
along with that entity.
- To generate additional areas from a pattern of areas, use one of the
following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Copy>Areas
Main Menu>Preprocessor>-Modeling-Move / Modify>-Areas-Areas
- To generate additional volumes from a pattern of volumes, use one of the
following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Copy>Volumes
Main Menu>Preprocessor>-Modeling-Move / Modify>Volumes
- To generate areas from an area pattern by symmetry reflection, use one of
the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Reflect>Areas
- To generate volumes from a volume pattern by symmetry reflection, use
one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Reflect>Volumes
- To transfer a pattern of areas to another coordinate system, use one of the
following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Move / Modify>Transfer
Coord>Areas
- To transfer a pattern of volumes to another coordinate system, use one of
the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Move / Modify>Transfer
Coord>Volumes
You must plan ahead to ensure that the interfaces between copied regions will
match up node for node. For example, if you freely meshed a volume, the pattern
of nodes on the right end would not necessarily match the pattern of nodes on the
left end. If the original part and its copy were to be joined such that the right end
of one part interfaced with the left end of the other part, a seam of discontinuity
would be created where the two mismatched faces touched.
It is relatively easy to create matching node patterns along the line edges of
meshed areas: simply specify the same number of line divisions and division
spacings on both sides of the original part. Volumes are not so straightforward,
however. You will need to use a trick to force matching node patterns on two
faces of a meshed volume. Before meshing with volume elements, mesh one of
the matching faces with dummy area elements, then copy that meshed area to the
other matching face. (Depending on how you originally created your volume, you
might or might not have some cleaning up to do at this point. If you wind up with
duplicate coincident areas, you should redefine your volume in terms of the new
meshed area, and delete the original volume.) The volume can then be meshed
with solid elements. After the volume meshing is complete, you should delete the
dummy area elements. (You can do this fairly cleanly using selecting and either
the ACLEAR command or menu path
Main Menu>Preprocessor>-Modeling- Clear>Areas.)
Having created meshed regions which will match up at their interfaces, you can
now copy the part, such that the repeated regions just touch. Even though these
regions will have matching nodes at the interfaces, the degrees of freedom at
these nodes will remain independent; that is, a seam of discontinuity will exist in
your model at the interface. You should execute NUMMRG,ALL to eliminate this
discontinuity. It is usually good practice to follow these operations with a NUMCMP command (Main
Menu>Preprocessor>Numbering Ctrls>Compress Numbers).
Figure 8-7 Generating meshed volumes with matching node patterns
at interfaces
8.4 Keeping Track of Element Faces and
Orientations
If your model contains shell elements, and if you apply surface loads, you will
need to keep track of the element faces in order to be able to define the proper
direction for your loads. In general, shell surface loads will be applied to element
face one, and will be positive in accordance with the right-hand rule (following the
I,J,K,L nodal sequence, as illustrated below). If you create your shell elements by
meshing a solid model area, the normal direction of the elements will be
consistent with the normal direction of the area (the area's normal direction can be
determined by issuing the ALIST command
or by executing menu path Utility Menu>List>Areas; the direction of the
sequence of lines defining that area will define the normal direction by the
right-hand rule).
Figure 8-8 Positive normal direction as defined by the right-hand rule
There are several ways that you can conduct graphical checks:
- You can conduct a quick graphical check of the positive normal direction for
shell elements by issuing a /NORMAL command (Utility
Menu>PlotCtrls> Style>Shell Normals), followed by an EPLOT command (Utility Menu>
Plot>Elements).
- You can turn PowerGraphics ON. PowerGraphics displays the "top" and
"bottom" of shells with different colors.
- You can apply your surface loads with the assumed correct sign, and then
verify their direction by turning on the surface load symbol [/PSF, Item,Comp,2] before executing EPLOT.
8.4.1 Controlling Area, Line, and Element Normals
Inconsistent normal directions can lead to problems in your model. For example,
if adjacent shell elements have inconsistent normal directions, you could
encounter difficulties in postprocessing of stress and strain results. Clearly, if a
surface of your model contains both top and bottom shell element faces, averaged
nodal stresses and strains could be incorrect. However, PowerGraphics [/GRAPH,POWER] accounts for the
mismatched normal directions and can produce proper nodal stress plots.
(PowerGraphics is the default when the GUI is on.)
ANSYS provides various tools that you can use to control area, line, and element
normals:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Move / Modify>-Elements-
Shell Normals
Main Menu>Preprocessor>-Modeling-Move / Modify>-Areas-Area
Normals
Main Menu>Preprocessor>-Modeling-Move / Modify>Reverse
Normals>of Shell Elems
Main Menu>Preprocessor>-Modeling-Move / Modify>Reverse
Normals>of Lines
Main Menu>Preprocessor>-Modeling-Move / Modify>Reverse
Normals>of Areas
The sections that follow describe how you can use these tools to:
- Reorient shell element normals so that they are consistent with that of a
specified element [ENORM]
- Reorient area normals so that they are consistent with that of a specified
area [ANORM]
- Reverse the normals of existing shell elements [ENSYM]
- Reverse the normal of a line [LREVERSE]
- Reverse the normal of an area [AREVERSE]
Note-You cannot use the tools described in this section to change the normal
direction of any element that has a body or surface load. We recommend that you
apply all of your loads only after ensuring that the element normal directions are
acceptable.
Caution: Real constants (such as non-uniform shell thickness and tapered beam
constants) may be invalidated by an element reversal.
8.4.1.1 Reorienting Shell Element Normals
If you find that your elements have inconsistent positive normal directions, you
can reorient them uniformly to match a specified element. (Element coordinate
systems, if defined by the I,J,K nodes, might also be reoriented by this operation.)
To use the command method to reorient shell element normals, issue the
command ENORM,ENUM:
- Use the ENUM argument to identify the number of the element having the
normal direction that the reoriented elements are to match.
For example, the command ENORM,3
reorients the normals of all selected shell elements so that they are consistent
with the normal direction of element number 3. See the description of the ENORM command in the ANSYS Commands Reference for details.
In the GUI, you can reorient shell element normals by choosing menu path Main
Menu>Preprocessor>-Modeling-Move / Modify>-Elements-Shell Normals.
When the Reorient Shell Normals picker appears, pick the element having the
normal direction that the reoriented elements are to match and click on OK.
8.4.1.2 Reorienting Area Normals
If a group of areas has inconsistent normal directions, you can reorient them
uniformly to match the normal direction of a specified area.
To use the command method to reorient area normals, issue the command ANORM,ANUM,NOEFLIP:
- Use the ANUM argument to identify the number of the area having the
normal direction that the reoriented areas are to match.
- Use the NOEFLIP argument to indicate whether you want to change the
normal direction of any existing elements on the reoriented area(s) so that
they are consistent with the new normal direction. Specify 0 if you want to
make the normals consistent; specify 1 if you do not.
For example, the command ANORM,5,0
reorients the normals of all selected areas so that they are consistent with the
normal direction of area number 5, and also makes any area elements on the
areas consistent with that normal direction. See the description of the ANORM command in the ANSYS Commands Reference for details.
In the GUI, you can reorient area normals by choosing menu path Main
Menu>Preprocessor>-Modeling-Move / Modify>-Areas-Area Normals.
When the Reorient Area Normals picker appears, pick the area having the normal
direction that the reoriented areas are to match and click on OK in the picker.
Then, in the Make area normals consistent dialog box, indicate whether you want
any existing area elements to be consistent with the new normal direction and
click on OK in the dialog box.
8.4.1.3 Reversing the Normals of Existing Shell Elements
To use the command method to reverse the normals of existing shell elements,
issue the command ENSYM,,,,IEL1,IEL2,IEINC:
- Use the IEL1, IEL2, and IEINC arguments to reverse the normals of
elements from IEL1 to IEL2 (defaults to IEL1) in steps of IEINC
(defaults to 1).
For example, the command ENSYM,,,,1,50
reverses the normals of shell elements numbered 1 through 50.
In the GUI, you can reverse the normals of existing shell elements by choosing
menu path Main Menu>Preprocessor>-Modeling-Move / Modify>Reverse
Normals>of Shell Elems. When the Reverse Shell Normals picker appears, pick
the shell elements whose normals are to be reversed and click on OK.
8.4.1.4 Reversing the Normal of a Line
To use the command method to reverse the normal of a line, issue the command
LREVERSE,LNUM,NOEFLIP:
- Use the LNUM argument to identify the number of the line whose normal is
to be reversed.
- Use the NOEFLIP argument to indicate whether you want to change the
normal direction of the existing elements on the line so that they are
consistent with the reversed line's new normal direction. Specify 0 if you
want to make the normals consistent; specify 1 if you do not.
For example, the command LREVERSE,1,1 reverses the direction of
line 1, but does not make any line elements on the line consistent with the new
direction. See the description of the LREVERSE command in the ANSYS Commands Reference for details.
In the GUI, you can reverse the normal of a line by choosing menu path Main
Menu>Preprocessor>-Modeling-Move / Modify>Reverse Normals>of Lines.
When the Reverse Line Normals picker appears, pick the line whose normal is to
be reversed and click on OK in the picker. Then, in the Make line normals
consistent dialog box, indicate whether you want any existing line elements to be
consistent with the new normal direction and click on OK in the dialog box.
8.4.1.5 Reversing the Normal of an Area
To use the command method to reverse the normal of an area, issue the
command AREVERSE,ANUM,NOEFLIP:
- Use the ANUM argument to identify the number of the area whose normal
is to be reversed.
- Use the NOEFLIP argument to indicate whether you want to change the
normal direction of the existing elements on the area so that they are
consistent with the reversed area's new normal direction. Specify 0 if you
want to make the normals consistent; specify 1 if you do not.
For example, the command AREVERSE,7,0 reverses the normal
direction of area 7 and makes any existing area elements on it consistent with the
new normal direction. See the description of the AREVERSE command in the ANSYS Commands Reference for details.
In the GUI, you can reverse the normal of an area by choosing menu path Main
Menu>Preprocessor>-Modeling-Move / Modify>Reverse Normals>of Areas.
When the Reverse Area Normals picker appears, pick the area whose normal is to
be reversed and click on OK in the picker. Then, in the Reverse area normals
dialog box, indicate whether you want any existing area elements to be consistent
with the new normal direction and click on OK in the dialog box.
8.5 Revising a Meshed Model: Clearing and
Deleting
Because of the solid modeling cross-reference checking that the ANSYS program
performs, you cannot delete meshed solid model entities, nor can you use EDELE or NDELE to delete elements and nodes that are
associated with solid model entities. In order to revise your model, you generally
need to clear solid model entities of their meshes by using the mesh clearing
commands. These clearing commands can be thought of as the inverse of the
meshing commands. After clearing your model, you can proceed to modify your
solid model as desired.
8.5.1 Clearing a Mesh
The mesh clearing commands delete the nodes and elements associated with the
corresponding solid model entity. When you clear a higher level entity, all lower
level entities will be automatically cleared, unless those lower entities are
themselves meshed with elements. Nodes on the boundary of an entity shared by
an adjoining meshed entity are not deleted as a result of clearing.
- To delete nodes and point elements associated with selected keypoints,
use one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Clear>Keypoints
- To delete nodes and line elements associated with selected lines, use one
of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Clear>Lines
- To delete nodes and area elements associated with selected areas, use
one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Clear>Areas
- To delete nodes and volume elements associated with selected volumes,
use one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Meshing-Clear>Volumes
The program will report how many of each kind of entity have been cleared after a
mesh clearing operation. An entity is considered to have been "cleared" if either
its elements or its nodes have been cleared.
Figure 8-9 Nodes at boundary of two areas
If the elements/nodes being cleared are at the end of the element/node lists, then
the next available element/node ID is reset accordingly. (You can suppress this
resetting with a MOPT,CLEAR,OFF
command.)
As was discussed earlier, element attributes that were assigned to the solid model
by TYPE, REAL, MAT, and ESYS commands followed by a meshing
command [AMESH, VMESH, etc.] will be cleared by a mesh
clearing command. These "clearable" attributes are designated by negative
attribute numbers in the output from listing commands [ALIST, VLIST, etc.]. The mesh clearing commands do
not affect attributes that were assigned by an attribute association command [AATT, VATT, etc.]. In either case, issuing new attribute
association commands will overwrite whatever element attributes were previously
associated with the cleared solid model.
8.5.1.1 Modifying Element Attributes
There are several reasons why you might want to modify element attributes after
meshing: you might have simply committed an error in assigning attributes, you
might need to change your design, or you might be converting your model from
one analysis discipline to another (such as in a sequential thermal-stress
analysis). The techniques available for modifying element attributes include the
following:
8.5.1.2 The "Brute Force" Method: You can clear your mesh using mesh
clearing commands; set new attributes using either attribute association
commands or commands such as TYPE, REAL, etc.; and then remesh using meshing
commands. Because remeshing can sometimes be expensive, this approach
should probably be avoided if the mesh itself is acceptable. Note what happens
when a mesh clearing command is executed: solid model attributes set by a
meshing command (identified by negative attribute numbers in listings produced
by ALIST, VLIST, etc.) will be deleted; solid model
attributes set by an attribute association command [AATT, VATT, etc.] will not be changed. Thus, because
the attribute association commands override the TYPE, REAL, MAT, and ESYS commands, you will not be able to
reassign solid model attributes with the TYPE, REAL, MAT, and ESYS commands if you initially assigned
attributes by using attribute association commands. (You will need to issue a new
attribute association command.) Upon remeshing, the attributes associated with
the solid model entities will be assigned to the elements generated on those
entities.
Direct Element Modification: Element attributes can also be modified without
the expense of remeshing: you can select the elements to be modified; reset
attributes (using, in this procedure, the TYPE,
REAL, MAT, and ESYS commands); and execute EMODIF,ALL or menu path Main Menu>
Preprocessor>-Modeling-Move / Modify>-Elements-Modify Attrib. This
procedure modifies the element attributes directly, without affecting the
corresponding solid model attributes. This procedure, although convenient, can
be dangerous, because the element attributes in your finite element model will no
longer match the element attributes in your solid model. Also, you could
conceivably change element attributes to inappropriate values, without receiving
any kind of warning. For these reasons, you must proceed cautiously if you
decide to attempt to change element attributes by direct element modification.
Another way of directly modifying the material number of specified elements is by
using the MPCHG command or menu
path Main Menu>Preprocessor>Material Props>Change Mat Num. (Unlike
other element-modification commands, which are valid only within PREP7, MPCHG is valid within both PREP7 and
SOLUTION. Thus, this command can be used to change element properties
between solutions.)
Attribute Table Modification: Another possibility would be to change entries in
the attribute tables after meshing, but before entering SOLUTION. A warning will
be issued if the REAL set or the MAT set contain unused entries (such as could
happen if a REAL property set for a beam were assigned to a spar element). No
remeshing is required with this procedure.
A Note About Adding and Deleting Midside Nodes: For any of these
procedures, if you change the element TYPE attribute to substitute midside-node
elements for non-midside-node elements, you will also need to use one of the
following methods to add the extra midside nodes as required:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Move / Modify>-Elements-Add
Mid Nodes
EMID must be preceded by execution of a
MODMSH,DETACH command or menu
path Main Menu>Preprocessor>Checking Ctrls>Model Checking. Also, in
order to delete midside nodes, you must first remove them from the midside-node
elements by issuing EMID,-1.
8.5.2 Deleting Solid Model Entities
You can delete solid model entities with the entity deletion commands described
below. Lower level entities cannot be independently deleted if they are attached
to a higher level entity. Thus, if you have created a block using a geometric
primitive command, you cannot selectively delete a keypoint that is associated
with that block, unless you first delete, in descending hierarchical order, all the
higher level entities (lines, areas, and volumes) that are attached to that keypoint.
- To delete unmeshed areas, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Delete>Area and Below
Main Menu>Preprocessor>-Modeling-Delete>Areas Only
- To delete unmeshed keypoints, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Delete>Keypoints
- To delete unmeshed lines, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Delete>Line and Below
Main Menu>Preprocessor>-Modeling-Delete>Lines Only
- To delete unmeshed volumes, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Delete>Volume and Below
Main Menu>Preprocessor>-Modeling-Delete>Volumes Only
Conversely, by activating the "sweep" option (that is, setting KSWP = 1) on the LDELE, ADELE, or VDELE commands, you can direct the program
to delete all the associated lower level entities automatically. (Such lower level
entities will not be deleted if they are attached to another higher level entity,
however.) For example, if you decide to delete an unmeshed sphere volume, you
can issue a single VDELE command, with
KSWP set to 1, to delete the volume and all its associated areas, lines, and
keypoints.
8.5.3 Modifying Solid Model Entities
You can modify the geometry of a solid model by changing the position of its
keypoints using one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Move / Modify>-Keypoints-
Set of KPs
Main Menu>Preprocessor>-Modeling-Move / Modify>-Keypoints-
Single KP
Any meshed regions attached to modified keypoints will be automatically cleared
of nodes and elements. All lines, areas, and volumes attached to the modified
keypoint will then be automatically redefined using the active coordinate system.
Unmeshed solid model entities may also be redefined by reissuing the commands
that originally defined them. For example, consider the following sequence, in
which a second K command is used to modify a
keypoint:
CSYS,0
K,1,5.0,6.0,7.0 ! Create KP 1 at X=5.0, Y=6.0, Z=7.0
CSYS,1
K,1,5.0,6.0,7.0 ! Redefine KP 1 at R=5.0, 
=6.0, Z=7.0
Keypoint 1 could only be redefined in this way if it was not attached to any higher
level entities. Lines, areas, and volumes can be similarly redefined, but only if
they are not attached to any higher level entities.
You can modify unmeshed lines using the operations described below. These
operations will also update attached unmeshed areas, even if these areas are
attached to volumes.
- To divide a single line into two or more lines, use one of the following
methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Operate>-Booleans-Divide>
Line into 2 Ln's
Main Menu>Preprocessor>-Modeling-Operate>-Booleans-Divide>
Line into N Ln's
Main Menu>Preprocessor>-Modeling-Operate>-Booleans-Divide>
Lines w/ Options
- To combine adjacent lines into one line, use one of the following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Operate>-Booleans
-Add>Lines
- To generate a fillet line between two intersecting lines, use one of the
following methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Create>-Lines-Line Fillet
8.6 Understanding Solid Model
Cross-Reference Checking
The previous sections alluded to several conditions that restrict you as you modify
your meshed solid model. These restrictions arise due to the cross-reference
checking that has been incorporated into the ANSYS program to prevent
contamination of the solid model and finite element model data. They may be
summarized as follows:
- Meshed keypoints, lines, areas, or volumes may not be deleted or moved.
- Nodes or elements associated with keypoints, lines, areas, or volumes may
not be moved. They can be deleted only with the mesh clearing
commands.
- Areas contained in volumes may not be deleted or changed.
- Lines contained in areas may not be deleted or changed (except by LDIV, LCOMB, or LFILLT, as discussed previously).
- Keypoints contained in lines may not be deleted. They can be moved only
with the KMODIF command, which
revises and clears (if meshed) attached lines, areas, and volumes.
The basic reasoning behind these rules might be visualized from the following
sketch. Schematically, your completed model can be thought of as a stack of
blocks, in which the bottommost block represents your keypoints, the next block
represents lines, and so forth. If you were to change a lower entity (a line, for
instance), you would disturb the entities that are stacked on top of it. (Admittedly,
this illustration somewhat oversimplifies the dependence of higher level entities on
lower entities.)
Figure 8-10 Why we have solid model cross-reference checking
These rules are not as restrictive as they might appear. Furthermore, for those
few instances when they absolutely prevent you from performing an operation that
you need, you can deactivate them, as is discussed in the next few paragraphs.
Be aware, however, that in deactivating these rules, you lose the protections that
they provide, and thereby increase the chances of irrevocably damaging your
model's database.
8.6.1 Circumventing Cross-Reference Checking (A Risky
Activity)
Cross-reference checking of the solid model usually serves only to help you avoid
corrupting your model's database. There are occasions, however, when you
might have good reason to attempt a "forbidden" operation. The MODMSH command (Main
Menu>Preprocessor>Checking Ctrls>Model Checking) exists for this purpose.
MODMSH has three options: DETACH,
NOCHECK, and CHECK.
MODMSH,DETACH detaches the finite
element model from the solid model, which will allow the finite element model to
be modified by node and element commands. This detachment keeps the
database "clean," in that there will be no recognized database conflicts. Consider,
for instance, a single keypoint and its associated node. Following a MODMSH,DETACH, the program will no
longer recognize the associativity between these two entities, so that you can now
move the node to a new location without creating a conflict in the database. Once
you have detached your model, you cannot perform such operations as selecting
or defining the finite element model in terms of the solid model, clearing the mesh,
or transferring solid model boundary conditions to the finite element model.
MODMSH,NOCHECK is very
dangerous. It deactivates all cross-reference checking, and makes it startlingly
easy to get the database so fouled up that hardly any solid modeling operations
are possible. Its utility is that it allows you to use commands such as EMODIF, NMODIF, EDELE, NDELE, etc. to modify elements and nodes
that were generated with the mesh commands. Activating this option will cause
the program to warn you that cross-reference checking is bypassed whenever
you initiate a solution or issue a PFACT or
SOLVE command. Use this option only if
you are completely sure of what you are doing, for the havoc you can inflict on
your database with the NOCHECK option on will often make it impossible for the
ANSYS customer support staff to help you recover from any trouble you get
yourself into.
MODMSH,CHECK restores
cross-reference checking after it has been inhibited. However, since the
database integrity could have been compromised while the checking was off, the
program will continue to warn you whenever you initiate a solution or issue a PFACT or SOLVE command. The only way to get rid of
this warning message is to start over with a "clean" database.
Go to the beginning of this chapter