2-D 4-Node Coupled Pore-Pressure-Thermal Mechanical Solid
CPT212 is a 2-D four-node coupled pore-pressure-thermal mechanical solid element. The element has bilinear displacement behavior.
The element is defined by four 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)
CPT212 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 CPT212 for more details about this element.
The geometry and node locations for this element are shown in Figure 212.1: CPT212 Geometry.
A degenerated triangular-shaped element can be formed by defining the same node number for nodes K and L. 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 212.1: CPT212 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). For any other input temperature pattern, unspecified temperatures default to TUNIF.
Input the nodal forces, if any, 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 the RSYS command 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. For a general description of element input, see Element Input.
I, J, K, L
UX, UY, PRES, TEMP
|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|
face 1 (J-I), face 2 (K-J), face 3 (I-K), face 4 (I-L)
T(I), T(J), T(K), T(L)
Plane strain (Z strain = 0.0) (default)
Temperature degree of freedom:
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 212.1: CPT212 Element Output Definitions
The element stress directions are parallel to the element coordinate system, as shown in Figure 212.2: CPT212 Stress Output. 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 212.1: CPT212 Element Output Definitions
|NODES||Nodes - I, J, K, L||-||Y|
|XC, YC||Location where results are reported||Y||2|
|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|
|EPEL:X, Y, Z, XY||Elastic strains||Y||Y|
|EPEL:1, 2, 3||Principal elastic strains||-||Y|
|EPEL:EQV||Equivalent elastic strain||Y||Y|
|EPTH:X, Y, Z, XY||Thermal strains||1||1|
|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|
Available only at centroid as a *GET item.
For axisymmetric solutions in a global coordinate system, the X, Y, XY, and Z stress and strain outputs correspond to the radial, axial, in-plane shear, and hoop stresses and strains, respectively.
Table 212.2: CPT212 Item and Sequence Numbers lists output available via the ETABLE command using the Sequence Number method. For more information, see Creating an Element Table and The Item and Sequence Number Table in this document. The table uses the following notation:
Table 212.2: CPT212 Item and Sequence Numbers
The area of the element must be positive.
The element must lie in a global X-Y plane as shown in Figure 212.1: CPT212 Geometry and the Y-axis must be the axis of symmetry for axisymmetric analyses. An axisymmetric structure should be modeled in the +X quadrants.
You can form a triangular element by defining duplicate K and L node numbers. (For more information, see Degenerated Shape 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 by the PSTRES command.