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
9.1 What Is Direct Generation?
Direct generation is the approach in which you define the nodes and elements of
a model directly. Despite the many convenience commands that allow you to
copy, reflect, scale, etc. a given pattern of nodes or elements, direct generation
can commonly require about ten times as many data entries to define a model as
compared to solid modeling.
This manual's earlier discussions of pre-planning (Chapter 2), coordinate
systems (Chapter 3), and working planes (Chapter 4) apply to
direct generation as well as to solid modeling.
A model that is assembled by direct generation is defined strictly in terms of nodes
and elements. Even though node and element generation operations can be
interspersed, no one element can be defined until after all of its nodes have been
created.
This section describes various tasks related to the direct generation of nodes.
Topics include:
- Defining nodes
- Generating additional nodes from existing nodes
- Viewing and deleting nodes
- Moving nodes
- Rotating a node's coordinate system
- Reading and writing text files that contain nodal data
9.2.1 Defining Nodes
Use any of the following methods to define nodes:
- To define individual nodes in the active coordinate system, use one of
these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>In Active CS
Main Menu>Preprocessor>Create>Nodes>On Working Plane
If using ANSYS interactively, you can define a working plane snap
increment and use picking [N, P] to
generate nodes graphically. (For more information on the working plane,
see Chapter 4.)
- To define a node at an existing keypoint, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>On Keypoint
- To move a node to an intersection of coordinate system surfaces, use one
of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Move / Modify>To Intersect
9.2.2 Generating Additional Nodes From Existing Nodes
Once you have created an initial pattern of nodes, you can generate additional
nodes using any of the following methods:
- To generate a line of nodes between two existing nodes, use one of these
methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling->Create>Nodes>
Fill between Nds
- To generate additional nodes from a pattern of nodes, use one of these
methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling->Copy>-Nodes->Copy
- To generate a scaled set of nodes from a pattern of nodes, use one of
these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Copy>Scale & Copy
Main Menu>Preprocessor>Move / Modify>Scale & Move
Main Menu>Preprocessor>Operate>Scale>Scale & Copy
Main Menu>Preprocessor>Operate>Scale>Scale & Move
- To generate a quadratic line of nodes from three nodes, use one of these
methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling->Create>Nodes>Quadratic Fill
- To generate a reflected set of nodes, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling->Reflect>Nodes
- To transfer a pattern of nodes to another coordinate system, use one of
these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Move / Modify>Transfer Coord>Nodes
- To define a node at the center of curvature of an arc of nodes, use one of
these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>At Curvature Ctr
If a local cylindrical coordinate system is defined [CS] at the center of curvature, you can use
the FILL command (Main
Menu>Preprocessor> Create>Nodes>Fill between Nds) to generate
additional nodes on the arc. If a radius of curvature is given, the center of
curvature is automatically calculated to be along the perpendicular bisector
of the NODE1-NODE2 line in the plane of NODE1, NODE2, and NODE3.
9.2.3 Viewing and Deleting Nodes
Use the following methods to view and delete nodes:
- To list nodes, use one of these methods:
Command(s):
GUI:
Utility Menu>List>Nodes
Utility Menu>List>Picked Entities>Nodes
- To display nodes, use one of these methods:
Command(s):
GUI:
Utility Menu>Plot>Nodes
Node numbers will also be displayed in EPLOT displays (Utility Menu>
Plot>Elements) for nodes attached to elements, if you have issued the
proper /PNUM command (Utility
Menu>PlotCtrls>Numbering).
- To delete nodes, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Delete>Nodes
Note-Deleting a node also deletes any boundary conditions (such as
displacements, forces, etc.) as well as any coupling or constraint equations
containing the deleted node.
9.2.4 Moving Nodes
Use any of the following methods to move nodes:
- Simply redefine a node by overwriting it with an N command (or with any other
node-generating command).
- To modify one (or all) of the coordinates defining a node (that is, move a
node to a new location), use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>By Angles
Main Menu>Preprocessor>Move / Modify>By Angles
Main Menu>Preprocessor>Move / Modify>Set of Nodes
Main Menu>Preprocessor>Move / Modify>Single Node
9.2.5 Calculating the Distance Between Nodes
To calculate the distance between two nodes:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Check Geom>ND distances
9.2.6 Rotating a Node's Coordinate System
Use any of these methods to rotate a node's coordinate system (which, by default,
is parallel to the global Cartesian coordinate system):
- To rotate nodal coordinate systems into the active coordinate system, use
one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>-Rotate Node CS->
To Active CS
Main Menu>Preprocessor>Move / Modify>-Rotate Node CS->
To Active CS
- To rotate a nodal coordinate system by direction cosines, use one of these
methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>By Vectors
Main Menu>Preprocessor>Move / Modify>By Vectors
- To rotate a nodal coordinate system by angles, use the N or NMODIF command (described earlier
in this chapter).
See Chapter 3 for more information on nodal coordinate systems.
9.2.7 Reading and Writing Text Files That Contain Nodal Data
You can read a text file containing nodal data. This ability could be useful if you
are importing ASCII nodal data from another mesh generator, a CAD/CAM
program, or another ANSYS session. You can also write such an ASCII file for
export to another program (which must be able to read this ANSYS file) or to
another ANSYS session. You will not normally need to read or write nodal data in
a standard ANSYS model generation session.
- To specify a range of nodes to be read from a node file, use one of these
methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>Read Node File
- To read nodes from a file, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>Read Node File
- To write nodes to a file, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Nodes>Write Node File
9.3 Elements
This section describes various tasks related to the direct generation of elements.
Topics include:
- Prerequisites for defining elements
- Assembling element tables
- Pointing to entries in element tables
- Reviewing the contents of element tables
- Defining elements
- Viewing and deleting elements
- Generating additional elements from existing elements
- Using special methods for generating elements
- Reading and writing text files that contain element data
- Modifying elements by changing nodes
- Modifying elements by changing element attributes
9.3.1 Prerequisites for Defining Element Attributes
Two things are required before you can define an element:
1. You must have already defined the minimum number of nodes required for
that element.
2. You must have specified the proper element attributes.
9.3.1.1 Assembling Element Tables
You assemble tables of element attributes using the methods described below
and various coordinate system commands. See Chapter 7 for more
information on creating element attribute tables.
- To define an element type from the element library, use one of these
methods:
Command(s):
GUI:
Main Menu>Preprocessor>Element Type>Add/Edit/Delete
- To define the element real constants, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Real Constants
- To define a linear material property, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Material Props>option
- To activate a data table (for nonlinear material properties), use one of these
methods:
Command(s):
GUI:
Main Menu>Preprocessor>Material Props>Data Tables>option
Main Menu>Preprocessor>Material Props>Mooney-Rivlin>option
9.3.1.2 Pointing to Entries in Element Tables
Once the element attribute tables are in place, you can "point" to various entries in
the element tables. The values of these pointers that are in effect at the time that
you create your elements are used by the program to assign attributes from the
tables to the elements.
To set the element type attribute pointer [TYPE], element real constant set attribute
pointer [REAL], element material attribute
pointer [MAT], or element coordinate system
attribute pointer [ESYS], use one of these
methods (the GUI paths are the same for all four commands):
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>Elem Attributes
See Figure 7-2 in Chapter 7 for schematic illustrations of attribute
tables.
9.3.1.3 Reviewing the Contents of Element Tables
You can review the contents of element tables by the following methods:
- To list currently defined element types, use one of these methods:
Command(s):
GUI:
Utility Menu>List>Properties>Element Types
- To list the real constant sets, use one of these methods:
Command(s):
GUI:
Utility Menu>List>Properties>All Real Constants
Utility Menu>List>Properties>Specified Real Constants
- To list linear material properties, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Material Props>List
Utility Menu>List>Properties>All Materials
Utility Menu>List>Properties>All Matls, All Temps
Utility Menu>List>Properties>All Matls, Specified Temp
Utility Menu>List>Properties>Specified Matl, All Temps
- To list data tables, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Material Props>Data Tables>List
Utility Menu>List>Properties>Data Tables
- To list coordinate systems, use one of these methods:
Command(s):
GUI:
Utility Menu>List>Other>Local Coord Sys
9.3.2 Defining Elements
Once you have defined the necessary nodes and set the element attributes, you
can proceed to define your elements. Using one of the methods described below,
you can define an element by identifying its nodes. The number of nodes
required for each element and the order in which they must be input are
determined by the element type. BEAM3, the 2-D
beam element, for example, requires two nodes (I,J), and SOLID45, the 3-D brick element, requires eight nodes
(I,J,K,L for one face and M,N,O,P for the opposite face). The order in which
nodes are defined determines the element normal direction. See "Keeping Track
of Element Faces and Orientations" in Chapter 8 for more information.
Use one of these methods to define elements:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>-Auto Numbered
-Thru Nodes
Main Menu>Preprocessor>Create>Elements>-User Numbered
-Thru Nodes
If you are working interactively, you can use graphical picking (that is, pick nodes)
to generate the elements by choosing one of the above GUI paths.
If you are using command input, only eight nodes can be input on the E command. For element types that require more
than eight nodes, use the EMORE
command to define the additional nodes. For example, SOLID95, the 3-D 20-node brick element, will require
two EMORE commands in addition to the
E command. (The EMORE command is not necessary if
graphical picking is used to create the elements.)
9.3.3 Viewing and Deleting Elements
Use the following methods to maintain elements:
- To list elements, use one of these methods:
Command(s):
GUI:
Utility Menu>List>Elements
Utility Menu>List>Picked Entities>Elements
- To display elements, use one of these methods:
Command(s):
GUI:
Utility Menu>Plot>Elements
Element numbers will be shown in your EPLOT display if you turn them on with
the /PNUM command (menu path
Utility Menu>PlotCtrls>Numbering). In most instances, the program will
automatically assign element numbers, using the next available unused
number. (The first E command defines
element number 1, the second E
command defines element number 2, and so on.)
- To delete elements, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Delete>Elements
Deleting elements creates "blanks" in your element-numbering sequence.
The automatic numbering procedure will not reuse these blank numbers,
even if they are at the end of your sequence. (If you define 10 elements,
then delete them all, the next E command
will define element number 11. Numbers 1-10 will remain blank.) You can
control element numbering through the number control commands (see
Chapter 11), or through the EN
command Main Menu>Preprocessor>Create>Elements>Thru Nodes),
which allows you to define an element's number directly.
9.3.4 Generating Additional Elements From Existing
Elements
Once you have created an initial pattern of elements, you can generate additional
elements using any of the following methods:
- To generate elements from an existing pattern, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Copy>Auto Numbered
- To generate elements from a pattern by symmetry reflection, use one of
these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Reflect>Auto Numbered
- To generate elements from an existing pattern (with hands-on numbering
control), use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Copy>User Numbered
- To generate elements by symmetry reflection (with hands-on numbering
control), use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Reflect>User Numbered
Main Menu>Preprocessor>Move/Modify>Reverse Normals>of Shell
Elements
These commands do not generate nodes; you must have generated the
necessary nodes beforehand. Also, the element attributes (MAT, TYPE, REAL,
and ESYS) for the generated elements are based upon the elements in the
original pattern and not upon the current specification settings.
9.3.5 Using Special Methods for Generating Elements
Some particular kinds of elements can be generated using the special methods
described below:
- To generate "surface" elements over the exterior faces of existing
elements, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Create>Elements>-On Contct
Surf-option
- To generate "surface" elements overlaid on the edge of existing plane
elements and to assign the extra node as the closest fluid element node,
use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Create>Elements>-On Contct
Surf-Surface Effect>-On Meshed Model-Line to Fluid
Use LFSURF to generate SURF151 elements with the "optional" node
used in some thermal analyses.
- To generate "surface" elements overlaid on the surface of existing solid
elements and to assign the extra node as the closest fluid element node,
use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>-Modeling-Create>Elements>-On Contct
Surf-Surface Effect>-On Meshed Model-Area to Fluid
Use AFSURF to generate SURF152 elements with the "optional" node
used in some thermal analyses.
- To "hook" together coincident nodes with 2-D line elements (such as gap
elements), use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>At Coincid Nd
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>At ContactSrf
9.3.6 Reading and Writing Text Files That Contain Element
Data
You can read or write a text file that contains element data. These capabilities
can be useful for transferring data to and from another program (or another
ANSYS session). You will not normally need to use these capabilities in a
standard ANSYS model generating session.
- To specify a range of elements to be read from an element file, use one of
these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>Read Elem File
- To read elements from a file, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>Read Elem File
- To write elements to a file, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>Write Elem File
9.3.7 A Note About Overlapping Elements
Please be advised that if you create overlapping elements (that is, elements
attached to the same nodes and occupying the same space), various ANSYS
features such as graphics, surface loads, selecting logic, etc. might not function as
expected. It is best to avoid the use of overlapping elements altogether; if this is
not possible, use extreme caution whenever you employ overlapping elements.
9.3.8 Modifying Elements By Changing Nodes
To redefine an element in terms of different nodes, you can use the methods
described below, taking care that the element attribute pointers are set to the
appropriate values. (The element attribute settings that are in place when you
execute these commands or GUI paths will control the element type, real
constants, material properties, and for some element types, the element
coordinate system that are assigned to the redefined elements.)
- To modify a previously defined element, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Move / Modify>Modify Nodes
- To redefine an element by its number and node connectivity, use one of
these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Create>Elements>Thru Nodes
You can also use the ENGEN and ENSYM commands and GUI paths, which are
described earlier in this chapter, to overwrite and redefine groups of elements.
9.3.9 Modifying Elements By Changing Element Attributes
There are several ways of changing the attributes of an element after it has been
created, including:
- To change the material number of a specified element within either PREP7
or SOLUTION, use one of these methods:
Command(s):
GUI:
Main Menu>Preprocessor>Loads>Other>Change Mat Props>
Change Mat Num
Main Menu>Preprocessor>Material Props>Change Mat Num
Main Menu>Solution>Other>Change Mat Props>Change Mat Num
- The combination of the EMODIF
and *REPEAT commands provide
another versatile method of redefining the attributes of existing elements
(within PREP7 only). You cannot access the *REPEAT command directly in the
GUI. The use of the EMODIF and
*REPEAT commands is illustrated
in the following example:
E,1,2 ! Element 1
REAL,3 ! REAL set pointer = 3
E,2,3 ! Element 2 (REAL=3)
EGEN,40,1,2 ! Generate 40 elements from el. 2 (all with REAL=3)
EMODIF,5,REAL,4 ! Redefine element 5 with REAL set 4
*REPEAT,18,2 ! Redefine els. 7-39 in steps of 2 (with REAL=4)
Alternatively, you can change the entries in the attribute tables after creating an
element, but before entering SOLUTION. A warning will be issued if the REAL set
or MAT set contain unused entries (such as could happen if a REAL property set
for a beam were assigned to a spar element).
Another way of changing your element attributes is by deleting your elements
(using the EDELE command or menu path
Main Menu>Preprocessor>Delete>
Elements), redefining your pointers, and re-creating your elements (using the EN command or menu path Main
Menu>Preprocessor>Create>Elements>Thru Nodes).
9.3.10 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 the EMID command to add the
extra midside nodes as required. Also, in order to delete midside nodes, you
must first remove them from the midside-node elements by issuing EMID,-1:
Command(s):
GUI:
Main Menu>Preprocessor>Move / Modify>Add Mid Nodes
Main Menu>Preprocessor>Move / Modify>Remove Mid Nd
When defining midside node elements using the direct generation method (that is,
the E, EN, and
similar commands), midside nodes are created and located according to the
following scheme:
- Some higher-order elements permit the removal of midside nodes. For
such elements, if a zero value (or blank) is used for a midside node when a
higher-order element is defined, the corresponding midside node is
removed from the element. This results in some or all of the quadratic
terms (depending on the number of removed midside nodes) in the
element's shape functions being ignored, thus forcing the element edge(s)
to be and remain straight. In the extreme case of an element with all of its
midside nodes removed, the element will use linear shape functions thus
producing results similar to the analogous lower-order (non-midside node)
element type.
- When defining a higher-order element, if a node number is used for a
midside node and that node has not yet been defined (N, NGEN, FILL, NSYM, and similar commands), then the
node will be automatically defined and given a geometric location that is the
calculated mid-point (linearly interpolated in Cartesian coordinates)
between its respective corner nodes. Nodal rotations for such nodes will
also be automatically calculated by linearly interpolating between the nodal
rotation angles of the corner nodes. This allows for the convenience of
creating midside node elements without the need to explicitly define the
geometric locations for midside nodes located midway between the corner
nodes.
Note that this behavior applies only to the direct model generation method.
Controls regarding midside nodes in meshed models are provided in the ANSYS
meshing controls.
Go to the beginning of this chapter