9.2. Elements

This section describes various tasks related to the direct generation of elements. Topics include:

9.2.1. Prerequisites for Defining Element Attributes

Before you directly generate elements, you must have already defined the minimum number of nodes required for that element and must have specified the proper element attributes.

You assemble tables of element attributes using the methods described in the following table and various coordinate system commands. See Generating the Mesh in the Modeling and Meshing Guide for more information on creating element attribute tables.

Table 9.7:  Assembling Element Tables

DefineCommandGUI
an element type from the element library ET Main Menu> Preprocessor> Element Type> Add/Edit/Delete
the element real constants R Main Menu> Preprocessor> Real Constants
a linear material propertyMP, MPDATA, MPTEMP Main Menu> Preprocessor> Material Props> Material Models> analysis type

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. Use one of the methods shown in the following table to set attribute pointers.

Table 9.8:  Pointing to Entries in Element Tables

SetCommandGUI
element type attribute pointer TYPE Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes
element real constant set attribute pointer REAL Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes
element material attribute pointer MAT Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes
element coordinate system attribute pointer ESYS Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes

You can review the contents of element table using one of the methods described in the following table.

Table 9.9:  Reviewing the Contents of Element Tables

ListCommandGUI
currently defined element types ETLIST Utility Menu> List> Properties> Element Types
real constant sets RLIST Utility Menu> List> Properties> All Real Constants or > Specified Real Constants
linear material properties MPLIST Utility Menu> List> Properties> All Materials or > All Matls, All Temps or > All Matls, Specified Temp or > Specified Matl, All Temps
data tables TBLIST

Main Menu> Preprocessor> Material Props> Material Models

Utility Menu> List> Properties> Data Tables

coordinate systems CSLIST Utility Menu> List> Other> Local Coord Sys

9.2.2. Defining Elements

After you have defined the necessary nodes and set the element attributes, you can proceed to define your elements. You can define an element by identifying its nodes using the E command (Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes or Main Menu> Preprocessor> Modeling> Create> Elements> User Numbered> Thru Nodes). The number of nodes required for each element and the order in which they must be input are determined by the element type. The order in which nodes are defined determines the element normal direction. See Keeping Track of Element Faces and Orientations in the Modeling and Meshing Guide for more information.

If you are working interactively, you can use graphical picking (that is, pick nodes) to generate the elements by choosing one of the GUI paths associated with the E command.

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, SOLID186, a 3-D 20-node structural solid 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.)


Caution:  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.


Once you have created your elements, use the methods described in the following table to maintain elements.

Table 9.10:  Maintaining Elements

MaintenanceCommandGUI
list elements ELIST

Utility Menu> List> Elements

Utility Menu> List> Picked Entities> Elements

display elements (1) EPLOT Utility Menu> Plot> Elements
delete elements (2) EDELE

Main Menu> Preprocessor> Modeling> Delete> Elements


  1. 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.)

  2. 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 Number Control and Element Reordering in the Modeling and Meshing Guide), or through the EN command Main Menu> Preprocessor> Modeling> Create> Elements> User Numbered> Thru Nodes), which allows you to define an element's number directly.

Once you have created an initial pattern of elements, you can generate additional elements using the methods described in the following table. Please note these commands do not generate nodes; you must generate the necessary nodes before you generate additional elements. 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.

Table 9.11:  Generating Additional Elements From Existing Elements

Generate ElementsCommandGUI
from an existing pattern EGEN Main Menu> Preprocessor> Modeling> Copy> Elements> Auto Numbered
from an existing pattern with explicitly incremented element numbers ENGEN Main Menu> Preprocessor> Modeling> Copy> Elements> User Numbered
from a pattern by symmetry reflection ESYM Main Menu> Preprocessor> Modeling> Reflect> Elements> Auto Numbered
by symmetry reflection with explicitly assigned element numbers ENSYM

Main Menu> Preprocessor> Modeling> Reflect> Elements> User Numbered

Main Menu> Preprocessor> Modeling> Move/Modify> Reverse Normals> of Shell Elements


Some elements can be generated using the special methods described in the following table.

Table 9.12:  Using Special Methods for Generating Elements

GenerateCommandGUI
“surface” elements over the exterior faces of existing elementsESURF (1) Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> option
“surface” elements overlaid on the edges of existing plane elements and assign the extra node as the closest fluid element nodeLFSURF (2) Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surface Effect> Attach to Fluid> Line to Fluid
"surface" elements overlaid on the surface of existing solid elements and assign the extra node as the closest fluid element nodeAFSURF (3) Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf Effect> Attach to Fluid> Area to Fluid
"surface" elements overlaid on the surface of the existing elements and assign the extra node as the closest fluid element nodeNDSURF (4) Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf Effect> Attach to Fluid> Node to Fluid
two-node elements between coincident or offset nodes EINTF Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> At Coincid Nd

  1. Use ESURF,XNODE to generate SURF151or SURF152, elements with the "optional" node used in some thermal analyses.

  2. Use LFSURF to generate SURF151 elements with the "optional" node used in some thermal analyses.

  3. Use AFSURF to generate SURF152 elements with the "optional" node used in some thermal analyses.

  4. Use NDSURF to generate SURF151 or SURF152 elements with the "optional" node used in some thermal analyses.

9.2.3. 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 Mechanical APDL session). You will not normally need to use these capabilities in a standard Mechanical APDL model generating session. If you do need to read or write element data you can use any of the methods described in the following table.

 CommandGUI
specify a range of elements to be read from an element file ERRANG Main Menu> Preprocessor> Modeling> Create> Elements> Read Elem File
read elements from a file EREAD Main Menu> Preprocessor> Modeling> Create> Elements> Read Elem File
write elements to a file EWRITE Main Menu> Preprocessor> Modeling> Create> Elements> Write Elem File

9.2.4. A Note About Overlapping Elements

Be advised that if you create overlapping elements (that is, elements attached to the same nodes and occupying the same space), various Mechanical APDL 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.

9.2.5. Modifying Elements By Changing Nodes

You can redefine an element in terms of different nodes, 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 the EMODIF command (Main Menu> Preprocessor> Modeling> Move/Modify> Elements> Modify Nodes).

To redefine an element by its number and node connectivity, use the EN command (Main Menu> Preprocessor> Modeling> Create> Elements> User Numbered> 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.

9.2.6. Modifying Elements By Changing Element Attributes

There are several ways of changing the attributes of an element after it has been created.

To change the material number of a specified element within either PREP7 or SOLUTION, use the MPCHG command. (See the MPCHG command description in the Command Reference for a list of menu paths associated with this command.)

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 following program listing illustrates the use of the EGEN, EMODIF, and *REPEAT commands. See their individual command descriptions in the Command Reference for more information.

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 (Main Menu> Preprocessor> Modeling> Delete> Elements), redefining your pointers, and recreating your elements using the EN command (Main Menu> Preprocessor> Modeling> Create> Elements> User Numbered> Thru Nodes).

9.2.7. 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 (Main Menu> Preprocessor> Modeling> Move/Modify> Elements> Add Mid Nodes or > Remove Mid Nd) 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 de-node elements for non-midside-node elements, you will also need to use EMID,-1.

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 midpoint (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 Mechanical APDL meshing controls.


Release 18.2 - © ANSYS, Inc. All rights reserved.