MESH200

Meshing Facet

MESH200 Element Description

MESH200 is a "mesh-only" element, contributing nothing to the solution. This element can be used for the following types of operations:

Multistep meshing operations, such as extrusion, that require a lower dimensionality mesh be used for the creation of a higher dimensionality mesh
Line-meshing in 2-D or 3-D space with or without midside nodes,
Area-meshing or volume-meshing in 3-D space with triangles, quadrilaterals, tetrahedra, or bricks, with or without midside nodes.
Temporary storage of elements when the analysis physics has not yet been specified.
Temporary representation of discrete reinforcing fibers and smeared reinforcing layers, including their geometry, material, and orientation. The following element options are available for reinforcing modeling:
- 2-D lines with two or three nodes for smeared reinforcing in 2-D
- 3-D Lines with two or three nodes for discrete reinforcing in 3-D
- 3-D triangle with three nodes, or quadrilateral with four nodes, for smeared reinforcing in 3-D
For more information about modeling reinforcing structural members with MESH200 elements, see Reinforcing in the Mechanical APDL Structural Analysis Guide.

MESH200 may be used in conjunction with any other ANSYS element types. After it is no longer needed, it can be deleted (cleared), or can be left in place. Its presence will not affect solution results.

MESH200 elements can be changed into other element types using EMODIF.

Figure 200.1: MESH200 Geometry

MESH200 Input Data

The permissible geometry and node locations for this element are shown in Figure 200.1: MESH200 Geometry. The element is defined by two to twenty nodes. It has no degrees of freedom, material properties, real constants, or loadings.

"MESH200 Input Summary" summarizes the element input. See Element Input in the Element Reference for a general description of element input.

MESH200 Input Summary

Nodes

I, J if KEYOPT (1) = 0, 2-D line with 2 nodes

I, J, K if KEYOPT (1) = 1, 2-D line with 3 nodes

I, J if KEYOPT (1) = 2, 3-D line with 2 nodes

I, J, K if KEYOPT (1) = 3, 3-D line with 3 nodes

I, J, K if KEYOPT (1) = 4, 3-D triangle with 3 nodes

I, J, K, L, M, N if KEYOPT (1) = 5, 3-D triangle with 6 nodes

I, J, K, L if KEYOPT (1) = 6, 3-D quadrilateral with 4 nodes

I, J, K, L, M, N, O, P if KEYOPT (1) = 7, 3-D quadrilateral with 8 nodes

I, J, K, L if KEYOPT (1) = 8, tetrahedron with 4 nodes

I, J, K, L, M, N, O, P, Q, R if KEYOPT (1) = 9, tetrahedron with 10 nodes

I, J, K, L, M, N, O, P if KEYOPT (1) = 10, brick with 8 nodes

I, J, K, L, M, N, O, P, Q, R, S, T, U, V, W, X, Y, Z, A, B if KEYOPT (1) = 11, brick with 20 nodes

Degrees of Freedom

None

Real Constants

None

Section

When used for reinforcing modeling:

Reinforcing section to define the material ID, fiber cross-section area, fiber spacing (smeared), and fiber orientation (smeared). See SECTYPE and SECDATA.

When used for other applications:

None

Material Properties

When used for reinforcing modeling:

All materials supported by reinforcing elements (REINF263, REINF264, and REINF265). The element material ID is recognized only when the material ID value (MAT) on the SECDATA command is blank.

When used for other applications:

None

Element Coordinate System

When used for reinforcing modeling:

You can define an element coordinate system (ESYS). The x axis indicates the fiber orientation. The element coordinate system applies to 3-D smeared reinforcing only, and is recognized only when the KCN value on the SECDATA command is blank.

When used for other applications:

None

Surface Loads

None

Body Loads

None

Special Features

Linear perturbation

KEYOPT(1)

Element shape and number of nodes:

0 --: 2-D line with 2 nodes
1 --: 2-D line with 3 nodes
2 --: 3-D line with 2 nodes
3 --: 3-D line with 3 nodes
4 --: 3-D triangle with 3 nodes
5 --: 3-D triangle with 6 nodes
6 --: 3-D quadrilateral with 4 nodes
7 --: 3-D quadrilateral with 8 nodes
8 --: tetrahedron with 4 nodes
9 --: tetrahedron with 10 nodes
10 --: brick with 8 nodes
11 --: brick with 20 nodes

KEYOPT(2)

Element shape testing:

0 --: Shape testing is done (default)
1 --: No shape testing is done for this element

MESH200 Output Data

This element has no output data.

MESH200 Assumptions and Restrictions

When this element is a triangle or quadrilateral, it is shape-tested in the same manner as an equivalent "non-structural shell". When it is a tetrahedron or brick, it is shape-tested like a SOLID185. This is so that meshing will work to create well-shaped elements. If KEYOPT(2) = 1, no shape testing is done for this element type.
MESH200 elements may not be active during result contour plotting (/POST1, PLNSOL, or PLESOL). The elements are automatically unselected during either operation.

MESH200 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS Mechanical Pro

Linear perturbation is not available.