3-D 10-Node Coupled Pore-Pressure-Thermal Mechanical
Solid
CPT217 Element Description
CPT217 is a higher-order 3-D 10-node coupled pore-pressure-thermal mechanical solid element. The element has a quadratic displacement, and linear pore-pressure and temperature behavior.
The element is defined by 10 nodes having four (or optionally five) 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 three degrees of freedom at midside nodes:
Translations in the nodal x and y directions
CPT217 has elasticity, stress stiffening, large deflection, and large strain capabilities. See CPT217 for more details about this element.
CPT217 Input Data
The geometry, node locations, and the coordinate system for this element are shown in Figure 217.1: CPT217 Geometry.
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 as described in the Material Reference.
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 217.1: CPT217 Geometry. Positive pressures act into the element.
For problems that do not consider the optional temperature degrees of freedom, temperatures may 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.
As described in Coordinate Systems, you can use the ESYS command to orient the material properties and strain/stress output. Issue 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. Element Input gives a general input description.
CPT217 Input Summary
- Nodes
I, J, K, L, M, N, O, P, Q, R
- Degrees of Freedom
UX, UY, UZ, PRES, TEMP
- Real Constants
None
- Material Properties
TB command: See Element Support for Material Models for this element. MP command: EX, EY, EZ, ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ), DENS, GXY, GYZ, GXZ, ALPD, BETD, DMPR - Surface Loads
- Pressures --
face 1 (J-I-K), face 2 (I-J-L), face 3 (J-K-L), face 4 (K-I-L)
- Body Loads
- Temperatures --
T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P), T(Q), T(R)
- Special Features
Initial state Large deflection Large strain Stress stiffening - KEYOPT(11)
Temperature degree of freedom:
- 0 --
Disabled (default)
- 1 --
Enabled
CPT217 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 217.1: CPT217 Element Output Definitions
The element stress directions are parallel to the element coordinate system, as shown in Figure 217.2: CPT217 Stress Output. A general description of solution output is given in The Item and Sequence Number Table. 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 217.1: CPT217 Element Output Definitions
| Name | Definition | O | R |
|---|---|---|---|
| EL | Element number | - | Y |
| NODES | Nodes - I, J, K, L | - | Y |
| MAT | Material number | - | Y |
| VOLU: | Volume | - | Y |
| XC, YC, ZC | Location where results are reported | Y | 2 |
| TEMP | Temperatures T(I), T(J), T(K), T(L) | - | Y |
| S:X, Y, Z, XY, YZ, XZ | 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, YZ, XZ | Elastic strains | Y | Y |
| EPEL:1, 2, 3 | Principal elastic strains | Y | - |
| EPEL:EQV | Equivalent elastic strains [3] | - | Y |
| EPTH:X, Y, Z, XY, YZ, XZ | Thermal strains | 1 | 1 |
| EPTH: EQV | Equivalent thermal strains [3] | 1 | 1 |
| EPTO:X, Y, Z, XY, YZ, XZ | Total mechanical strains (EPEL + EPPL + EPCR) | Y | - |
| EPTO:EQV | Total equivalent mechanical strains (EPEL + EPPL + EPCR) | Y | - |
| ESIG:X, Y, Z, XY, XZ, YZ | Effective stresses | - | Y |
| PMSV:VRAT,PPRE,DSAT,RPER | Void volume ratio, pore pressure, degree of saturation, and relative permeability | - | Y |
Table 217.2: CPT217 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 the table:
- Name
Output quantity as defined in Table 217.1: CPT217 Element Output Definitions
- Item
Predetermined Item label for ETABLE command
- I,J,...,R
Sequence number for data at nodes I, J, ..., R
CPT217 Assumptions and Restrictions
The element must not have a zero volume.
Elements may be numbered either as shown in Figure 217.1: CPT217 Geometry or may have node L below the I, J, K plane.
An edge with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that edge. For information about using midside nodes, see Quadratic Elements (Midside Nodes).
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.