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 for more information on creating element attribute 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. Use one of the methods shown in the following table to set attribute pointers.

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

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. 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 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 3D 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.)

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

Once you have created an initial pattern of elements, you can generate additional elements using the methods described in the following table. Note that 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.

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

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.

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.

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.

To redefine an element by its number and node connectivity, use the EN command.

You can also use the ENGEN and ENSYM commands (described earlier in this chapter) to overwrite and redefine groups of elements.

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.

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.

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, redefining your pointers, and recreating your elements using the EN command.

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 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:

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.