A large scale, general purpose finite element computer program, ANSYS, developed and marketed by Swanson Analysis Systems, Inc. is discussed. ANSYS was perhaps the first commercially available program to offer truly interactive finite element model generation. ANSYS's purpose is for solid modeling. This application is briefly discussed and illustrated

Kelley, F. S.

English

NASA Technical Reports Server

N88-19115
Finite Element Meshing of ANSYS ® Solid Models
F. S. Ketley, Supervisor, General Development
Swanson Analysis Systems, Inc.
P. O. Box 65, Johnson Road
Houston, Pennsylvania 15342
Telephone: (412) 746-3304
Presentation at the Workshop on the Integration of
Finite Element Modeling with Geometric Modeling
Rennselaer Polytechnic Institute
May 1987
/_._.¢7Y'o
/ ,7/,,#
ORIGINAIJ PAGE IS
OF POOR QUALIT'Ej
(All images are from ANSYS Revision 4.3)
1. INTRODUCTION - ANSYS AND SASI HISTORY
Swanson Analysis Systems, Inc. (SASI) was founded in 1970 by Dr. John A. Swanson to develop,
support, and market ANSYS, a large scale, general purpose finite element computer program.
ANSYS and the recently introduced ANSYS-PC products remain the only reasons for SASI's
existence. There is no engineering consulting practice to distract attention away from the software
business. SASI currently employs over 100 people at its office near Pittsburgh, Pennsylvania, and
there are thirty regional support distributors marketing and supporting ANSYS worldwide.
ANSYS was developed solely for the commercial market, with no government or university funding.
It has more than 1000 installations to date, including universities, but not PC's.
1
https://ntrs.nasa.gov/search.jsp?R=19880009731 2020-03-20T08:02:40+00:00Z
2. PURPOSE OF ANSYS SOLID MODELING
ANSYS was perhaps the first commercially available program to offer truly interactive finite element
model generation. (In the late 1970's, there was confusion about what constitutes =interactive"
processing. Some programs would simply prompt users for a fixed sequence of commands.)
ANSYS Revision 3, released in August 1978, contained PREP7. This processor allowed a user to
create, display, and modify a finite element mesh in whatever order desired.
ANSYS Revision 3 also contained a powerful 3-dimensional automatic mesh generator called
PREP5. Based on keypoints, lines, areas, and volumes, this processor created brick models with
relative ease. It was also capable of automatic application of boundary conditions. PREP5 was
never as popular for model creation as PREP7. However, some users were upset when we
removed PREP5 at Revision 4.0, released in 1982.
ANSYS Revision 4.0 (1982) introduced the PREP7 Mesh module, with powerful automatic
Quadrilateral and brick meshing capabilities. The 4.0 MESH module was widely used for model
generation, but it could not handle i[regular regions.
The ANSYS PREP7 MESH module was rewritten as a solid modeler for Revision 4.2 (1985), and
enhanced in Revision 4.3 (to be released in June 1987), This was done solely to aid ANSYS users
in the creation of finite element analysis models. SASI did not have to patch finite element
meshing into the ANSYS solid modeler as an afterthought. It was designed in from the beginning.
From SASI's point of view, any other benefits which may be derived from the creation of a solid
model in ANSYS (such as pretty pictures) are bonuses rather than primary objectives.
3. ANSYS REVISION 4.3 SOLID MODELS
ANSYS solid models are internally stored in several forms. The first of these has been well
documented in textbooks and papers.
Hermite cubic splines as shown below.
figures 1 - 3.
2X - C1 + C2 • r + C3 • r +
2
Y - C5 + C6 • r _ C7 • r +
2
Z = C9 + CIO • r + Cll • r +
Lines, surfaces, and volumetric regions are defined by
The parameters r, s, and t vary from 0.0 to 1.0. See
(line)
3
C4 r
3
C8 r
3
C12 r
2 3
X - C1 + C2 • r + C3 • r + C4 r
+ (C5 + C6 • r + C7 • r 2 + C8 r 3 ) (s)
+ (C9 + ClO • r + Oil • r 2 + C12 r 3 ) (s 2 )
÷ (C13 + C14 • r + C15 • r 2 + C16 r 3 ) (s 3 )
2 3
Y - C17 + C18 • r + C19 • r + C20 r
+ (C21 ÷ C22 • r + C23 • r 2 ÷ C24 r 3 ) (s)
÷ (C25 ÷ C26 • r + C27 • r 2 + C28 r 3 ) (s 2 )
+ (C29 + C30 • r + C31 • r 2 + C32 r 3 ) (s 3 )
2 3
Z - C33 + C34 • r + C35 • r + C36 r
+ (C37 + C38 • r + C39 • r 2 + C40 r 3 ) (s)
+ (C41 + C42 • r ÷ C43 • r 2 + C44 r 3 ) (s 2 )
+ (C45 + C46 • r + C47 • r 2 + 048 r 3 ) (s 3 )
2 3
X = C1 + C2 • r + C3 • r + C4 r
. (C5 + C6 • r + C7 • r 2 + C8 r 3 ) (s)
+ (C9 + CIO • r + Cll • r 2 + C12 r 3 ) (s 2
(surface)
(volumetric reEion)
÷ (C13 + C14 • r + C15 • r 2 + C16 r 3 ) (s 3 )
+ [C17 + C18 • I" + C19 • r 2 + C20 r3
+ (C21 + C22 • r + C23 • i-2 + C24 r 3 ) (3)
+ (C25 + C26 • r + C27 • r 2 + C28 r 3 ) (3 2 )
+ (C29 + C30 • I" ÷ C31 • z` 2 + C32 1` 3 ) (s 3 ) ] It]
+ [C33 + C34 • r + C35 • r 2 + C36 z"3
+ (C37 + C38 • r + C39 • r 2 + C40 z'3 ) (3)
+ (C41 + C42 • r + C43 • r 2 + C44 z.3 ) (3 2 )
+ (C45 ÷ C46 • 1" ÷ C47 • !-2 + C48 z"3 ) (3 3 ) ] It 2 ]
+ [C49 + C50 • r + C51 • r2 + C52 z"3
+ (C53 + C54 • r + C55 • r 2 + C56 1.3 ) (s)
÷ (C57 + C58 • r + C59 • r 2 + C60 r 3 ) (s 2 )
+ (C61 + C62 • r ÷ C63 • r 2 + C64 r 3 ) (s 3 ) ] [t 3 ]
(The equations for Y and Z are similar, using C65 through C192.)
Figure 1 Hermite Spline Defining a Line
Figure 2 Bicubic Hermit• Spline Defining a Surface Region
Figure3 TricubicHermiteSplineDefininga VolumetricRegion
ANSYSalsoallowsthedefinitionof degenerateHermiteregions(figures4 and5). Thisis very
impo_ant. There is no assurance that an arbitrary surface can be mapped by quadrilateral
regions, and even less assurance that an arbitrary 3-dimensional object can be mapped by
hexahedral regions. The degenerate forms give ANSYS a far more general modeling capability
than would be provided by the standard regions,
Figure 4 Degenerate Surface Region
r
Figure 5 Degenerate Volumetric Region
4
New to ANSYS Revision 4.3 is the ability to define surface regions by a list of up to 200 cubic line
segments, and volumetric regions by a list of up to 200 bicubic surface regions (figures 6 and 7).
These alternate region types allow great flexibility in the modeling of complex structures. They also
make it difficult to classify the ANSYS solid modeler into one category, such as "B-rep" or
"CSG". Perhaps "hybrid CSG" is the best term to apply.
I i
IL6
I J
",L7
IL9
I
I
I
I
L_ m
=L4
i_ 33-
I
IL2
I
I
Figure 6 Surface Region Defined by a List of Lines
Hermite
surface
f patches
Figure 7 Volumetric Region Defined by a List of Surface Patches
Oefinition of solid models in ANSYS begins with the input of several "keypoints". "Line segments",
"areas", and "volumes" may be defined by connecting keypoints. Lower order entities are
generated automatically as needed. Lines and areas follow the curvature of the "currently active
coordinate system" (figure 8). Translation, rotation, and symmetry reflection operations are
available, Line segments may be rotated about an axis or dragged along a path to produce areas
(figure 9). Areas may be rotated about an axis or dragged along a path to produce volumes
(figure 10). ANSYS is command driven, with complete documentation available on-line via a menu
system. Cross hair and digitizing tablet input is also possible.
Figure 8
egments
Keypoints
ANSYS Keypoints, Line Segments, Areas, and Volumes
Rotation Axis
Drag Pa_.,,_
Line Segments Line Segments
Figure 9 Rotation and Dragging of Line Segments to Create Areas
DragPath
Area
Figure 10 Dragging of an Area to Create Volumes
4. SURFACE ACCURACY OF ANSYS SOLID MODELS
Accuracy of curved surfaces in cubic spline based solid modelers can be of concern. Circular
arcs and intersection lines cannot be represented exactly by Hermite splines. A circular arc of 90
degrees has a radius error of 0.03 % (figure 11). For an arbitrary region extending 90 degrees on
the surface of a cylinder, the radius error can be as much as 0.2 % (figure 12). Lines resulting
from the intersection of arbitrary 90 degree regions can have a radius error of 0.4 % (figure 13).
Figure 14 shows the effect of a +/- 0.5 % local perturbation of radius on the results of the analysis
of a flat plate with a hole. The maximum corner stress decreased by 0.8 % as a result of the
perturbation. For solid elements, the stress error appears to be of the same order of magnitude
as the geometric error. Figure 15 shows the effect of a +/- 0.5 % local perturbation of radius on
the results of the analysis of a pressurized spherical shell. The stress error introduced was
approximately 8 %. For shell elements, the stress error appears to be an order of magnitude
higher than the geometric error, The radius error in the ANSYS solid modeler is drastically
reduced if the line segments and areas are limited to spans of 45 degrees or less. Typical radius
errors are then 0.0005 % for line segments. 0,005 % for areas, and 0.03 % for intersection lines.
Radius error = 0.03%
Radius error = 0
Figure 11 Radius Error for a 90 Degree Line Segment
Figure12 RadiusErrorfor Arbitrary90DegreeArea
i
J_
i_1 II
/11111
# IIl|l
/ lllJl
I I1111
L
3 Y×
Intersection of cylinders -
/ Maximum radius error = 0.4%
Figure 13 Radius Error for Intersection of 2 Arbitrary 90 Degree Areas i
Radius = Constant
7?777X',..7
_-.", /il __
Radius varies +/- 0.5%
Figure 14 Effect of Radius Error on Plane Stress Solution
Membrane Stress
/ ---.. -_ __ varies +/- 0.5%
/ _/_ / _ _ Membrane Stress
._- i _ I ",<
/ I"'l_l\l\
I I"'_1\1\1\ i,"" ./ i\l\lk/\
'_/../ _.\ ,,_,, \,,\_ _.
- _6"/\ # \ / \,_"\
+/"{,',-.,0.)0
Radaus Varies
varies +/- 8%
R,-.--/"
+/- 0.5% __
Figure 15 Effect of Radius Error on Shell Stress Solution
5. FINITE ELEMENT MESHING OF AN ANSYS SOLID MODEL
The first step in meshing of an ANSYS solid model is to establish the mesh density. This is
accomplished by assigning a number of element divisions and a spacing ratio to every line
segment attached to the areas or volumes (figure 16). Commands are available for making the
assignments line segment by line segment or to a group of line segments at once. Divisions can
be computed based on line segment length and a desired element size and assigned
automatically. Spacing ratios can also be computed automatically for smooth mesh transitioning
(figure 17).
DivisionsAllLineEStablished _ ____for Segments _ _ °
Figure16 EstablishingFiniteElementMeshDensity
/
/
/
/
I.. /
%
/
/
/
/
/
m
/I
I
I
I
I
I
I
I
Figure 17 Automatically Adjusted Line Divisions and Spacing Ratios
Meshing of areas with quadrilateral elements and volumes with brick elements is available in certain
cases. The most limiting restriction is that only the standard region shapes (four keypoints on
areas, eight keypoints on volumes) are allowed. Further, the number of element divisions
requested must match on opposing sides of areas (figure 18). The area corner angles must be
reasonable for quadrilateral or brick elements. The mesh is mapped onto the natural coordinates
of the areas and volumes (figures 19 and 20).
10
fMatching Divisions /--_'_ I
Matching Divisions
Figure 18 Matching Divisions on Areas Required for Quadrilateral or Brick Meshing
f
Figure 19 Quadrilateral Element Mesh!ng of an Area
I
'/' _ i
S
Figure 20 Brick Element Meshing of a Volume
11
Meshing with triangles is available for all areas, regular or not. Meshing with tetrahedra is available
for all volumes, regular or not. The elements of choice are the 6-noded triangular solid or shell
(figure 21) and the 10-noded tetrahedral solid (figure 22). ANSYS has these elements available
for stress, thermal, electro-magnetic, or multi-field analysis. For planar, axisymmetric, or shell
applications, 6-noded triangles are good performers, giving results of equal or superior quality for
equal edge divisions when compared to 4-noded or 8-noded quadrilaterals. For 3-dimensional
solid applications, 10-noded tetrahedra perform well. (This element is a theoretically consistent,
completely conforming element which passes the patch test, Because tetrahedral meshes are
rarely symmetric, however, this element can develop localized spurious deformation modes. For
this reason, some theoreticians have refused to bless this element for general use. This is really
bad news if their fear is justified, since tetrahedral meshing is the only reasonable approach to
automated meshing of arbitrary 3-dimensional shapes. No conclusions can be reached, however,
until the stress analysis community has had ample opportunity to gain experience with tetrahedra.)
ANSYS uses the same algorithm for triangular meshing of areas and tetrahedral meshing of
volumes: an initial mesh is formed without regard to region shape and is then repeatedly
improved by operations which divide or combine elements, until all elements are nicely shaped or
until no operations available will improve the situation. This iterative scheme is computationally
intensive, but is highly reliable and produces well distributed meshes of well shaped elements.
Figure 21 6-Noded Triangle Element
Figure 22 l O-Noded Tetrahedron Element
12
Figure23 TriangularMesh on the Exterior of a Volume
Prior to Tetrahedron Meshing
We at SASl have been asked on several occasions why we do not mesh areas with mixtures of
quadrilaterals and triangles, or mesh volumes with mixtures of bricks, wedges, and tetraheOra.
First, there is little evidence to suggest that such mixed meshes are likely to perform any better
than meshes consisting entirely of triangles or tetrahedra. Second, the algorithms to produce such
meshes appear to be at least as complex and compute intensive as the triangle and tetrahedron
algorithms, if they are to check element shape as thoroughly as they should. Finally, connecting
brick elements to wedges and tetrahedra is not a straightforward process if one wishes to avoid
displacement incompatibilities.
Meshing of adjacent areas or adjacent volumes in ANSYS will always produce compatible and
properly interconnected finite element meshes. This is possible because the triangle and
tetrahedron meshing algorithms used do not have the "authority" to alter the exterior of the mesh
of a region. As shown in figure 23, the tetrahedral meshing of a volume starts with a fixed exterior
triangular mesh, which cannot change.
6. BOUNDARY CONDITIONS
The following boundary conditions may be defined directly on an ANSYS solid model.
imposed displacements at keypoints
imposed temperatures at keypoints
imposed voltage at keypoints
imposed magnetic potential at keypoints
(stress analysis)
(thermal analysis)
(electrical analysis)
(magnetic analysis)
(constraints can be interpolated over attached line segments, areas, and volumes)
temperatures at keypoints (stress analysis)
heat generation rates at keypoints (thermal analysis)
(can be interpolated over attached line segments, areas and volumes)
13
applied forces at keypoints
applied heat input at keypoints
applied current flow at keypoints
applied magnetic flux at keypoints
pressures on line segments
convections on line segments
symmetry / antisymmetry
on line segments
(stress analysis)
(thermal analysis)
(electrical analysis)
(magnetic analysis)
(2-0 stress analysis)
(2-D thermal analysis)
(2-D solid or 3-D shell
stress analysis)
pressures on areas
convections on areas
symmetry / antisymmetry
OR areas
(3-D stress analysis)
(3-D thermal analysis)
(3-D stress analysis)
Boundary conditions may be defined before or after finite element meshing, and can be displayed
on the solid model. They will be transferred to the finite element model automatically when
needed. (The transfer can be forced earlier if the user wishes to display them on the finite
element model.)
Even if boundary conditions are not applied directly to an ANSYS solid model, they can be
conveniently applied to a finite element model created by the solid modeler. Nodes and elements
associated with various mesh entities can be activated or deactivated as desired, making it easy to
specify where constraints or Ioadings belong.
7. ANSYS INTERFACE WITH CAD SYSTEMS
ANSYS accepts keypoint and line segment information from a number of other solid modeling
systems (see Table 1). A user can use this data to create areas and/or volumes and a finite
element model.
Table 1
Translations within
ANSYS
Other Systems Having Some Interface
with ANSYS
IGES ADAMS-DRAM ClS-MEDUSA PATRAN
MEDUSA ADVANTAGE DIAD Solid Modeler PDGS
FEMVlEW ANVIL ENGINEER WORKS PROF. CADAM
FEMGEN APPLICON EUCLID ROMULUS-D
NASTRAN AUTOCAD FEMAS SOLUTION 3000
SUPERTAB AXXYZ GRAFTEK UNIGRAPHICS
CADAM ICAD VERSACAD
CADKEY INTERGRAPH
CATIA ME30
CDS-4000 M.E. Workbench
ClMLINK MOLDFLOW
Even though ANSYS can accept nodes and elements created by other systems, we believe that in
most cases the user will be better off doing the finite element meshing step within ANSYS. First,
we have seen evidence (finite element models from other systems) that not all develol3ers of
meshing software know what constitutes a good analysis model. Badly shaped elements may give
poor quality analysis results. (It is far better to inform the user that meshing is not possible with
14
the data supplied than to produce an unacceptable mesh.) Second, if the user has meshed in
another system, he or she may be reluctant to make any alterations to the model which may be
indicated by initial analysis results. Third, the required mesh may by load dependent. Finally,
nodes and elements brought into ANSYS from another system will not be associated with the solid
model, and boundary condition manipulation will be difficult.
8. FUTURE DEVELOPMENT PLANS
In the short term (Revision 4.4, 1988), we plan improvements in the command structure for
defining ANSYS solid models. We hope to improve the speed and reliability of our meshing
algorithms. We plan to allow definition of contact surfaces. We plan to improve our interfaces
with other software packages.
In the long term (Revision 5, 1990), we want to address some or all of the following.
• mapping analysis results back onto the solid model
• adaptive mesh refinement
• improved curved surface accuracy
• improved user interface
9. EXAMPLES
Figures 24 through 31 show several examples of ANSYS solid models and resulting finite element
meshes. Table 2 shows the various statistics for these models.
Table 2
Example Statistics
Elapsed time* for creation
Number of Number of of solid model & finite
Model Commands Elements element model Computer
Block with two holes 159 3047 tetrahedra 183 minutes VAX 11/780
Helix 62 2856 tetrahedra 160 minutes Prime 9950
Pawn 60 819 triangles 19 minutes MicroVax
Knight 351 2427 tetrahedra 318 minutes MicroVax
Gear 279 1136 tetrahedra 31 minutes Prime 9950
Gear Submodel 186 2684 tetrahedra 138 minutes Prime 9950
Turbine Spacer 403 1224 tetrahedra 75 minutes Prime 9950
"CP times are nearly identical
15
ORIGINAL; PAGE I_
0E POOR QUALrl_
Figure 24 Tetrahedron Model of Block with
Two Holes
Figure 25 Detail of Tetrahedron Model -
Block with Two Holes
Figure 26 Tetrahedron Model of Helix Figure 27 Triangle Model of Pawn
16
OR2GfNA!_ PAGE IS
OE t:'OOR QUALITY
Figure 28 Tetrahedron Model of Knight Figure 29 Stress Contours on Tetrahedron
Model of Gear
/
Figure 30 Stress Contours on Tetrehedron
Submodel of Gear
Figure 31 Stress Contours on Tetrahedron
Model of Turbine Spacer
17


Finite element meshing of ANSYS (trademark) solid models

Abstract

Similar works

Full text

Available Versions

NASA Technical Reports Server