SURF154 Element Description

SURF154 is used for various load and surface effect applications in 3D structural analyses. It can be overlaid onto an area face of any 3D element. Various loads and surface effects may exist simultaneously. See SURF154 in the Mechanical APDL Theory Reference for more details about this element.

Figure 154.1: SURF154 Geometry

SURF154 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 154.1: SURF154 Geometry. The element is defined by four to eight nodes and the material properties. A triangular element may be formed by defining duplicate K and L node numbers as described in Degenerated Shape Elements. The default element x-axis is parallel to the I-J side of the element.

The mass and volume calculations use the element thicknesses at nodes I, J, K, and L (real constants TKI, TKJ, TKK, and TKL, respectively). Thickness TKI defaults to 0.0, and thicknesses TKJ, TKK, and TKL default to TKI. The mass calculation uses the density (material property DENS, mass per unit volume) and the real constant ADMSUA, the added mass per unit area.

The stress stiffness matrix and load vector calculations use the in-plane force-per-unit length (input as real constant SURT). The elastic foundation stiffness (input as real constant EFS) uses pressure-per-length (or force-per-length-cubed) 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.

See Element 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 154.2: Pressures. SURF154 allows complex pressure loads.

Faces 1, 2, and 3 [KEYOPT(2) = 0]  —  Positive values of pressure on the first three faces act in the positive element coordinate directions (except for the normal pressure which acts in the negative z direction). For face 1, positive or negative values may be removed as requested with KEYOPT(6) to simulate the discontinuity at the free surface of a contained fluid. For faces 2 and 3, the direction of the load is controlled by the element coordinate system; therefore, ESYS is normally needed. The loads specified in the element coordinate system follow the large displacements and/or rotations of the element.

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 local 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; however, the loads specified in that local coordinate system do not follow the large displacements and/or rotations of the element. KEYOPT(6) does not apply.

Figure 154.2: Pressures

Face 4  —  The direction is normal to the element and the magnitude of the pressure at each integration point is P_I + XP_J + YP_K + ZP_L, where P_I through P_L are input as VAL1 through VAL4 on the SFE command, and X, Y, Z are the global Cartesian coordinates at the current location of the point. No input values can be blank. Face 4 can be used to apply hydrostatic ocean loading, with P_L = -(vertical acceleration) * (water density). Positive or negative values may be removed as requested with KEYOPT(6) to simulate the discontinuity at the free surface of a contained fluid. The SFFUN and SFGRAD commands do not work with face 4. The load follows the large displacements and/or rotations of the element.

Face 5  —  The magnitude of the pressure is P_I, and the direction is where i, j, and k are unit vectors in the global Cartesian directions. The load magnitude may be adjusted with KEYOPT(11) and KEYOPT(12). No input values can be blank. When using the SFFUN or SFGRAD commands, the load direction is not altered but the load magnitude is the average of the computed corner node magnitudes. SFCUM,ADD should be used with caution, as this command also causes the load direction components to be added. The load does not follow the large displacements and/or rotations of the element.

The effects of pressure load stiffness are automatically included for this element for real pressure on face 1 if KEYOPT(2) = 0 or on face 4. If an unsymmetric matrix is needed for pressure load stiffness effects, issue a NROPT,UNSYM command.

Temperatures may be input as element body loads at the nodes. Element body load temperatures are not applied to other elements connected at the same nodes. The node I temperature T(I) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I). If all corner node temperatures are specified, each midside node temperature defaults to the average temperature of its adjacent corner nodes. For any other input temperature pattern, unspecified temperatures default to TUNIF. Temperatures are used for material property evaluation only.

When KEYOPT(4) = 0, an edge with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that edge. See Quadratic Elements (Midside Nodes) in the Modeling and Meshing Guide for more information about the use of midside nodes.

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 an area; however, if the area changes due to large deflections, the force also changes. When KEYOPT(7) = 1, the force remains unchanged even if the area changes.

KEYOPT(8) > 0 applies ocean loading on the element.

A summary of the element input is given in "SURF154 Input Summary". A general description of element input is given in Element Input.

SURF154 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 154.3: SURF154 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 154.3: SURF154 Item and Sequence Numbers:

SURF154 Assumptions and Restrictions

SURF154 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  —  

Ansys Mechanical Premium  —