SURF153 Element Description

SURF153 may be used for various load and surface effect applications. It may be overlaid onto a face of any 2D structural solid element (except axisymmetric harmonic elements PLANE25 and PLANE83). The element is applicable to structural analyses, but for 3D structural analyses, it must be laid on any global Cartesian Z = constant plane. See SURF153 in the Mechanical APDL Theory Reference for more details about this element.

Figure 153.1: SURF153 Geometry

SURF153 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 153.1: SURF153 Geometry. The element is defined by two or three node points and the material properties. The nodes for this element must share the nodes of the underlying solid element. The element x-axis is along to the I-J line of the element.

The mass and volume calculations use the in-plane element thicknesses at nodes I and J (real constants TKI and TKJ, respectively). Thickness TKI defaults to 0.0, and thickness TKJ defaults to TKI. If KEYOPT(3) = 3, the out-of-plane thickness is input as the real constant TKPS (defaults to 1.0). 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 as force-per-length-squared on the element faces as shown by the circled numbers on Figure 153.2: Pressures. SURF153 allows complex pressure loads.

Figure 153.2: Pressures

Faces 1 and 2 [KEYOPT(2) = 0]  —  Positive values of pressure on the first two faces act in the positive element coordinate directions (except for the normal pressure which acts in the negative y 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.

Faces 1 and 2 [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 and face 2 in the local y 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.

Face 3  —  The magnitude of the pressure at each integration point is P_I + XP_J + YP_K, where P_I through P_K are input as VAL1 through VAL3 on the SFE command, and X and Y are the global Cartesian coordinates at the current location of the point. No input values can be blank. The SFFUN and SFGRAD commands do not work with face 3.

Face 4  —  The magnitude of the pressure is P_I, and the direction is where i and j are unit vectors in the global Cartesian directions. The load magnitude can be adjusted with KEYOPTs(11) and (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 effects of pressure load stiffness are automatically included for this element for real pressure on face 1 if KEYOPT(2) = 0 or on face 3. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

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. The node J temperature defaults to T(I). Temperatures are used for material property evaluation only.

KEYOPT(3) = 3 enables you to define constant or varying out-of-plane thickness (TKPS) via the real constant input. To define varying out-of-plane thickness, input a table name (specified as %tablename% and created via *DIM). Tabular out-of-plane thickness can vary in terms of coordinates (X and Y) or node numbers. Supported primary variables for tabular thickness (TKPS) are X, Y, and NODES. (The Function Tool is a convenient way to define your thickness tables; you can use it to define thickness as a function of global/local coordinates.)

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

If a single PLANE element lies beneath SURF153, you can automatically set the element behavior (plane stress, axisymmetric, or plane stress with thickness [including TKPS if applicable]) to that of the underlying solid element using KEYOPT(3) =10. This option is valid only when a single PLANE element lies beneath the SURF element. For example, if you apply a SURF153 element over a PLANE77 (thermal) element whose nodes are also used in the definition of a PLANE183 (structural) element, a warning appears and the load is not applied to the element.

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.

A summary of the element input is given in "SURF153 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

SURF153 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 153.3: SURF153 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 153.3: SURF153 Item and Sequence Numbers:

SURF153 Assumptions and Restrictions

SURF153 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  —