2-D 8-Node Coupled Pore-Pressure-Thermal Mechanical
Solid
CPT213 Element Description
CPT213 is a higher-order 2-D eight-node coupled pore-pressure-thermal mechanical solid element. The element has quadratic displacement behavior and is well suited to modeling curved boundaries.
The element is defined by eight nodes having three (or optionally four) degrees of freedom at each corner node:
Translations in the nodal x and y directions
One pore-pressure degree of freedom
One temperature degree of freedom (optional)
and two degrees of freedom at midside nodes:
Translations in the nodal x and y directions
CPT213 can be used as a plane strain or axisymmetric element. The element has stress stiffening, large deflection, and large strain capabilities. Various printout options are also available. See CPT213 for more details about this element.
A higher-order version of this element is CPT217.
CPT213 Input Data
The geometry, node locations, and the coordinate system for this element are shown in Figure 213.1: CPT213 Geometry.
A degenerated triangular-shaped element can be formed by defining the same node number for nodes K, L and O. In addition to the nodes, the element input data includes the orthotropic material properties. Orthotropic material directions correspond to the element coordinate directions. (The element coordinate system orientation is described in Coordinate Systems.)
Element loads are described in Nodal Loading. Pressures can be input as surface loads on the element faces as shown by the circled numbers in Figure 213.1: CPT213 Geometry. Positive pressures act into the element.
For problems that do not consider the optional temperature degrees of freedom, temperatures can be input as element body loads at the 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.
The nodal forces, if any, should be input per unit of depth for a plane analysis and on a full 360° basis for an axisymmetric analysis.
As described in Coordinate Systems, you can use the ESYS command to orient the material properties and strain/stress output. Use ESYS to choose output that follows the material coordinate system or the global coordinate system.
The effects of pressure load stiffness are automatically included for this element, and the element generally produces an unsymmetric matrix. To avoid convergence difficulty, issue the NROPT,UNSYM command to use the unsymmetric solver.
The following table summarizes the element input. Element Input gives a general description of element input.
CPT213 Input Summary
- Nodes
I, J, K, L, M, N, O, P
- Degrees of Freedom
UX, UY, PRES, TEMP
- Real Constants
None - Material Properties
TB command: See Element Support for Material Models for this element. MP command: EX, EY, EZ, PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), DENS, GXY, GYZ, GXZ, ALPD, BETD, DMPR - Surface Loads
- Pressures --
face 1 (J-I), face 2 (K-J), face 3 (I-K), face 4 (I-L)
- Body Loads
- Temperatures --
T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P)
- Special Features
Initial state Large deflection Large strain Stress stiffening - KEYOPT(3)
Element behavior:
- 1 --
Axisymmetric
- 2 --
Plane strain (Z strain = 0.0) (default)
- KEYOPT(11)
Temperature degree of freedom:
- 0 --
Disabled (default)
- 1 --
Enabled
CPT213 Output Data
The solution output associated with the element is in two forms:
Nodal displacements and pore pressure included in the overall nodal solution
Additional element output as shown in Table 213.1: CPT213 Element Output Definitions.
As illustrated in Figure 213.2: CPT213 Stress Output, the element stress directions are parallel to the element coordinate system. 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 213.1: CPT213 Element Output Definitions
| Name | Definition | O | R |
|---|---|---|---|
| EL | Element number | - | Y |
| NODES | Nodes - I, J, K, L | - | Y |
| MAT | Material number | - | Y |
| THICK | Thickness | - | Y |
| VOLU | Volume | - | Y |
| XC, YC | Location where results are reported | Y | 1 |
| TEMP |
Temperatures T(I), T(J), T(K), T(L) | - | Y |
| S:X, Y, Z, XY | Stresses | Y | Y |
| S:1, 2, 3 | Principal stresses | - | Y |
| S: INT | Stress intensity | - | Y |
| S:EQV | Equivalent stress | - | Y |
| EPEL:X, Y, Z, XY | Elastic strains | Y | Y |
| EPEL:1, 2, 3 | Principal elastic strains | Y | - |
| EPEL:EQV | Equivalent elastic strain [2] | - | Y |
| EPTH:X, Y, Z, XY | Thermal strains | 3 | 3 |
| EPTH:EQV | Equivalent thermal strain [2] | - | 3 |
| ESIG:X, Y, Z, XY | Effective stresses | - | Y |
| PMSV:VRAT,PPRE,DSAT,RPER | Void volume ratio, pore pressure, degree of saturation, and relative permeability | - | Y |
For axisymmetric solutions, the X, Y, XY, and Z stress and strain outputs correspond to the radial, axial, in-plane shear, and hoop stresses and strains.
Table 213.2: CPT213 Item and Sequence Numbers lists output available via 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 document for more information. The following notation is used in Table 213.2: CPT213 Item and Sequence Numbers:
- Name
output quantity as defined in Table 213.1: CPT213 Element Output Definitions
- Item
predetermined Item label for ETABLE
- E
sequence number for single-valued or constant element data
- I,J,...,P
sequence number for data at nodes I, J, ..., P
CPT213 Assumptions and Restrictions
The area of the element must be positive.
The element must lie in a global X-Y plane as shown in Figure 213.1: CPT213 Geometry and the Y-axis must be the axis of symmetry for axisymmetric analyses. An axisymmetric structure should be modeled in the +X quadrants.
An edge with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that face. See Quadratic Elements (Midside Nodes) in the Mechanical APDL Modeling and Meshing Guide in the Modeling and Meshing Guide for more information about the use of midside nodes.
A triangular element can be formed by defining duplicate K-L-O node numbers. (See Degenerated Shape Elements.) For these degenerated elements, the triangular shape function is used and the solution is the same as for the regular triangular 6-node elements.
Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). It is ignored in geometrically linear analyses (NLGEOM,OFF). Prestress effects can be activated via the PSTRES command.