3-D 20-Node Coupled Pore-Pressure-Thermal Mechanical Solid
CPT216 Element Description
CPT216 is a higher-order 3-D 20-node coupled pore-pressure-thermal mechanical solid element. The element exhibits quadratic displacement behavior and is well suited to modeling irregular meshes.
The element is defined by 20 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, y, and z directions
CPT216 has elasticity, stress stiffening, large deflection, and large strain capabilities. The element can have any spatial orientation. Various printout options are available.
See CPT216 for more details about this element.
A lower-order version of this element is CPT215.
CPT216 Input Data
The geometry, node locations, and the element coordinate system for this element are shown in Figure 216.1: CPT216 Geometry. A prism-shaped element may be formed by defining the same node numbers for nodes K, L, and S; nodes A and B; and nodes O, P, and W. A tetrahedral-shaped element and a pyramid-shaped element may also be formed as shown in Figure 186.1: SOLID186 Homogeneous Structural Solid Geometry. (CPT217 is similar, but is a 10-node tetrahedral element.)
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 Coordinate Systems.
Element loads are described in Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 216.1: CPT216 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. 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. Element Input provides a general description of element input.
CPT216 Input Summary
- Nodes
I, J, K, L, M, N, O, P, Q, R, S, T, U, V, W, X, Y, Z, A, B
- 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
face 1 (J-I-L-K), face 2 (I-J-N-M), face 3 (J-K-O-N), face 4 (K-L-P-O), face 5 (L-I-M-P), face 6 (M-N-O-P) - Body Loads
- Temperatures --
T(I), T(J),T(K), T(L), T(M), T(N), T(O), T(P), T(Q), T(R), T(S), T(T), T(U), T(V), T(W), T(X), T(Y), T(Z), T(A), T(B)
- Special Features
Initial state Large deflection Large strain Stress stiffening - KEYOPT(2)
Element technology:
- 0 --
Uniform reduced integration (default)
- 1 --
Full integration
- KEYOPT(11)
Temperature degree of freedom:
- 0 --
Disabled (default)
- 1 --
Enabled
CPT216 Element Technology
CPT216 uses the uniform reduced integration method or the full integration method, as follows:
Uniform reduced integration method
Helps to prevent volumetric mesh locking in nearly incompressible cases. However, hourglass mode might propagate in the model if there are not at least two layers of elements in each direction.
Full integration
The full integration method does not cause hourglass mode, but can cause volumetric locking in nearly incompressible cases. This method is used primarily for purely linear analyses, or when the model has only one layer of elements in each direction.
CPT216 Output Data
The solution output associated with the element is in two forms:
Nodal displacements and pore pressures included in the overall nodal solution
Additional element output as shown in Table 216.1: CPT216 Output Definitions
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 216.1: CPT216 Output Definitions
| Name | Definition | O | R |
|---|---|---|---|
| EL | Element number and name | - | Y |
| NODES | Nodes - I, J, K, L, M, N, O, P | - | 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), T(M), T(N), T(O), T(P) | - | 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 | Y | Y |
| EPTH:X, Y, Z, XY, YZ, XZ | Thermal strains | 1 | 1 |
| EPTH:EQV | Equivalent thermal strains | 1 | 1 |
| 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 |
Available only at centroid as a *GET item.
Table 216.2: CPT216 Item and Sequence Numbers lists output available via the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 216.2: CPT216 Item and Sequence Numbers:
- Name
output quantity as defined in Table 216.1: CPT216 Output Definitions
- Item
predetermined Item label for ETABLE
- I,J,...,B
sequence number for data at nodes I, J, ..., B
CPT216 Assumptions and Restrictions
The element must not have a zero volume. Also, the element may not be twisted such that the element has two separate volumes (which occurs most frequently when the element is numbered improperly). Elements may be numbered either as shown in Figure 216.1: CPT216 Geometry or may have the planes IJKL and MNOP interchanged.
An edge with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that edge. See Quadratic Elements (Midside Nodes) for more information on the use of midside nodes.
Use at least two elements in each direction to avoid the hourglass effect when using reduced integration (KEYOPT(2) = 0).
When degenerated into a tetrahedron, wedge, or pyramid element shape (described in Degenerated Shape Elements), the corresponding degenerated shape functions are used. Degeneration to a pyramidal form should be used with caution. The element sizes, when degenerated, should be small to minimize the stress gradients. Pyramid elements are best used as filler elements or in meshing transition zones.
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.