SURF156 Element Description

SURF156 can be used to apply line pressure loads on structures. It may be overlaid onto the edge of any 3-D element. The element is applicable to 3-D structural analyses. Various loads and surface effects may exist simultaneously. See SURF156 - 3-D Structural Surface Line Load Effect in the Mechanical APDL Theory Reference for more details about this element.

Figure 156.1:  SURF156 Geometry

SURF156 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 156.1: SURF156 Geometry. The element is defined by two to four nodes (KEYOPT(4) = 0 or 1). The orientation node lies in the element x-z plane and is required for orientation of the element loads. The element x-axis is parallel to the line connecting nodes I and J of the element.

The elastic foundation stiffness (input as real constants EFSY and EFSZ) uses pressure (or force-per-length-squared) units. The foundation stiffness can be damped, either by using the material property BETD as a multiplier on the stiffness or by directly using the material property VISC.

The mass calculation uses the real constant ADDMAS, the (added) mass per unit length.

See Nodal Loading for a description of element loads. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 156.2: Pressures. SURF156 allows complex pressure loads. The input units are force per length.

Faces 1, 2, and 3 [KEYOPT(2) = 0] Positive values of pressure on the first three faces act in the positive element coordinate directions. For faces 2 and 3, the direction of the load is controlled by the element coordinate system which is oriented via the orientation node; therefore, the ESYS command has no effect. When using large deflection (NLGEOM,ON), the orientation of the loads may change based on the new location of the nodes. If the orientation node is on another element that moves, the orientation node will move with it. If the orientation node is not on another element, the node cannot move.

Faces 1, 2, and 3 [KEYOPT(2) = 1] Pressure loads are applied to the element faces according to the local coordinate system, as follows: face 1 in the x direction, face 2 in the local y direction, and face 3 in the local z direction. A local coordinate system must be defined, and the element must be set to that coordinate system via the ESYS command. When using large deflection (NLGEOM,ON), the orientation of the loads does not change.

Figure 156.2:  Pressures

Face 4 The magnitude of the pressure P_I and the direction where i, j, and k are unit vectors in the global Cartesian directions. When specifying a varying surface load (SFFUN) or a gradient (slope) for surface loads (SFGRAD), the load direction is not altered, but the load magnitude is the average of the calculated corner node magnitudes. Use caution if accumulating surface loads by adding subsequent values to the previous values (SFCUM,ADD), as doing so also adds the load-direction components.

Face 5 The magnitude of the pressure is P_I, the load point is node I, and the direction is the element x-axis.

Face 6 The magnitude of the pressure is P_I, the load point is node J, and the direction is the element negative x-axis.

The effects of pressure load stiffness are automatically included for this element for real pressure on faces 2 and 3 if KEYOPT(2) = 0. If an unsymmetric matrix is needed for pressure load stiffness effects, issue a NROPT,UNSYM command.

KEYOPT(7) = 1 is useful when the element is used to represent a force. When KEYOPT(7) = 0, the force is input as a pressure times a unit length; however, if the length changes due to large deflections, the force also changes. When KEYOPT(7) = 1, the force remains unchanged even if the length changes.

A summary of the element input is given in "SURF156 Input Summary". A general description of element input is given in Element Input.

SURF156 Output Data

The solution output associated with the element is in two forms:

A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 156.2: SURF156 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (/POST1) of the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 156.2: SURF156 Item and Sequence Numbers:

SURF156 Assumptions and Restrictions

SURF156 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