General Axisymmetric Surface
Use SURF159 to model axisymmetric solid surface loads acting on general axisymmetric solid elements (SOLID272 or SOLID273). The element has linear or quadratic displacement behavior on the master plane and is well suited to modeling irregular meshes on the master plane. It is defined by two or three nodes on the master plane, and nodes created automatically in the circumferential direction based on the master plane nodes. The total number of nodes depends on the number of nodal planes (KEYOPT(2)). The element area between nodal planes is called a facet. Each node has three degrees of freedom: translations in the nodal x, y and z directions. Various loads and surface effects can exist simultaneously.
In addition to the SURF159 element information provided here, the following topics are available in the Mechanical APDL Theory Reference:
For related information (concerning the elements used with SURF159), see General Axisymmetric Elements in this document.
The geometry and node locations for this element (when KEYOPT(2) = 3) are shown in Figure 159.1: SURF159 Geometry (KEYOPT(2) = 3). The element input data includes nodes, real constants, and the material properties. The total number of nodes is the two or three base nodes times the number of nodal planes. (For information about how Fourier nodes are generated, see the NAXIS command documentation.) SURF159 elements can be generated via the ESURF command before generating nodes for general axisymmetric element sections (NAXIS).
The element has the x-axis as normal to the element surface, the y-axis in the meridional direction, and the z-axis in the circumferential direction.
The mass and volume calculations use the element thicknesses (real constants TKI, and TKJ). Thickness TKJ defaults 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) and the elastic foundation stiffness (input as real constant EFS); the 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.
Pressures must be input as element surface loads (as force-per-length squared) on the element faces as shown by the circled numbers in Figure 159.2: SURF159 Pressures. For SURF159, applying surface loads to the element (SFE) or nodes (SF) is very different in comparison to the SOLID272 and SOLID273 elements. An SF command, if issued, applies loads to faces 1 through K only (where K = KEYOPT(2), the number of nodal planes).
SURF159 allows complex loads.
Faces 1 through 3K [KEYOPT(3) = 0] Positive values of pressure on these faces act in the positive element coordinate directions, as follows: faces 1 through K in the element x (normal) direction, faces K+1 through 2K in the element y (tangent, meridional) direction, and faces 2K+1 through 3K in the element z (tangent, circumferential) direction. For faces 1 through K, positive or negative values may be removed as requested via KEYOPT(6) to simulate the discontinuity at the free surface of a contained fluid. For faces K+1 through 3K, the direction of the load is controlled by the element coordinate system; therefore, the ESYS command may be needed.
Faces 1 through 3K [KEYOPT(3) = 1] Pressure loads are applied to the element faces according to the local coordinate system, as follows: faces 1 through K in the local x direction, faces K+1 through 2K in the local y direction, and faces 2K+1 through 3K 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. KEYOPT(6) does not apply.
Face 3K+1 The direction is normal to the element
and the magnitude of the pressure at each integration point is PI + XPJ + YPK + ZPL, where PI through
PL are input as
VAL4 on the SFE command, and X, Y, Z are the global Cartesian coordinates at the
current location of the integration point. No input values can be
blank. 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 3K+1.
Face 3K+2 The magnitude of the pressure is PI, 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.
Temperatures may be input as element body loads at the nodes. For the nodes on the master plane, the node I1 temperature T(I1) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I1). If both corner node temperatures are specified, the midside node temperature defaults to the average temperature of the adjacent corner nodes. For any other input pattern, unspecified temperatures default to TUNIF. For the nodes generated in the circumferential direction based on the master node, if all other temperatures are unspecified, they default to the value of their base nodes (T(I1), T(J1), and T(K1), depending on their location). For any other input pattern, unspecified temperatures default to TUNIF.
The effects of pressure load stiffness are automatically included for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, issue a NROPT,UNSYM command. For a geometric nonlinear analysis when convergence is an issue, use an unsymmetric matrix.
I1, J1, K1, I2, J2, K2, . . . , In, Jn, Kn (where n = KEYOPT(2), the number of nodal planes)
UX, UY, UZ
|(Blank), (Blank), (Blank), EFS, SURT, ADMSUA,|
MP command: DENS, VISC, ALPD, BETD, DMPR
In the following table, K represents the number of nodal planes (specified via KEYOPT(2)):
|Pressure Face||Nodes||Pressure Load Type|
|KEYOPT(3) = 0||KEYOPT(3) = 1|
|face 1||J1, I1, I2, J2||Normal||x direction per ESYS|
|face 2||J2, I2, I3, J3|
|. . .||. . .|
|face K||JK, IK, I1, J1|
|face K+1||J1, I1, I2, J2||Meridional tangent||y direction per ESYS|
|face K+2||J2, I2, I3, J3|
|. . .||. . .|
|face 2K||JK, IK, I1, J1|
|face 2K+1||J1, I1, I2, J2||Circumferential tangent||z direction per ESYS|
|face 2K+2||J2, I2, I3, J3|
|. . .||. . .|
|face 3K||JK, IK, I1, J1|
|face 3K+1||All||Global taper|
|face 3K+2||All||Oriented vector|
T(I1), T(J1), T(K1), T(I2), T(J2), T(K2), . . . , T(In), T(Jn), T(Kn)
|Birth and death|
Number of Fourier nodes in the circumferential direction (that is, the number of nodal planes):
Axisymmetric deformation (with or without torsion).
General 3-D deformation.
For information about specifying the number Fourier nodes, see General Axisymmetric Elements in this document.
For information about how Fourier nodes are generated, see the NAXIS command documentation.
Pressure applied to faces 1 through 3K (3 x KEYOPT(2)), according to the coordinate system:
Apply face loads in the default element coordinate system (for example, the first K faces act normal to the surface).
Apply face loads in the specified element coordinate system (for example, the first K faces act in the x direction as defined via the ESYS command).
Applicable only to normal direction pressure (faces 1 through K and 3K+1):
Use pressures as calculated (positive and negative).
Use positive pressures only (negative set to zero).
Use negative pressures only (positive set to zero).
To use KEYOPT(6), KEYOPT(3) must be set to 0.
Loaded area during large-deflection analyses:
Use new area.
Use original area.
Pressure applied by vector orientation (face 3K+2):
On projected area and includes tangential component.
On projected area and does not include tangential component.
On full area and includes the tangential component.
Effect of the direction of the element normal (element x-axis) on vector oriented (face 3K+2) pressure:
Pressure load is applied regardless of the element normal orientation.
Pressure load is not used if the element normal is oriented in the same general direction as the pressure vector.
Table 159.1: SURF159 Real Constants
|1 ... 3||(Blank)||--|
|6||ADMSUA||Added mass/unit area|
|7||TKI||In-plane thickness at node I|
|8||TKJ||In-plane thickness at node J (defaults to TKI)|
The solution output associated with the element is in two forms:
Nodal displacements included in the overall nodal solution
Additional element output as shown in Table 159.2: SURF159 Element Output Definitions
To view 3-D mode shapes for a modal or eigenvalue buckling analysis,
expand the modes with element results calculation active (via the MXPAND command's
Elcalc = YES
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 159.2: SURF159 Element Output Definitions
|NODES||Nodes - I, J, . . . , K (nodes in master plane)||Y||Y|
|NNP||Number of nodal planes||Y||Y|
|ADMSUA||Added mass per unit area||Y||Y|
|EFS||Elastic foundation stiffness||Y||Y|
Table 159.3: SURF159 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this document for more information. The following notation is used in the output table:
Table 159.3: SURF159 Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input (K = KEYOPT(2))|
The item and sequence numbers shown are for real pressures. Imaginary pressures are represented in the same way but have 12K+8 added to them.
The length of the base element must be nonzero.
The base element must lie on one side of the axisymmetric axis, and the axisymmetric axis must be on the same plane as the base element (master plane).
A base element or base node must be associated with one axisymmetric axis (defined via SECTYPE and SECDATA commands) before generating nodes for general axisymmetric element sections (NAXIS) or defining an element by node connectivity (E).
An edge with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that edge. For more information about the use of midside nodes, see Quadratic Elements (Midside Nodes) in the Modeling and Meshing Guide.
You cannot apply a pressure load by applying a surface load to selected areas (SFA).
The contribution of the element to the mass moment inertia of the whole model is calculated by element mass multiplied by the square of the coordinates of the elemental centroid. The moment of inertia may therefore be inaccurate.
The element does not support the expansion pass of a superelement with large rotation.
Issuing an /ESHAPE,1 command while PowerGraphics is active causes the program to plot the elements in 3-D and the results on both nodal planes and all integration planes in the circumferential direction; otherwise, the program plots the elements in 2-D and the results on the master plane.
You cannot display surface load symbols (/PSF) for this element.
When listing the surface loads for elements (SFELIST), only information for the first facet is returned.
When plotting contour values via /ESHAPE,1, expanded SURF159 elements are assigned zeroes; you should therefore deselect SURF159 elements when plotting results such as stresses and strains.
In postprocessing, print commands return the nodal plane results only.