SOLID187 ## SOLID187 Element Description

## SOLID187 Input Data

### SOLID187 Input Summary

## SOLID187 Output Data

## SOLID187 Assumptions and Restrictions

## SOLID187 Product Restrictions

**3-D 10-Node
Tetrahedral Structural Solid**

Compatible Products: DesSpc | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

SOLID187 element is a higher order 3-D, 10-node element. SOLID187 has a quadratic displacement behavior and is well suited to modeling irregular meshes (such as those produced from various CAD/CAM systems).

The element is defined by 10 nodes having three degrees of freedom
at each node: translations in the nodal x, y, and z directions.
The element has plasticity, hyperelasticity, creep, stress stiffening,
large deflection, and large strain capabilities. It also has mixed
formulation capability for simulating deformations of nearly incompressible
elastoplastic materials, and fully incompressible hyperelastic materials.
See SOLID187 in the *Mechanical APDL Theory Reference* for more details
about this element.

The geometry, node locations, and the coordinate system for
this element are shown in *Figure 187.1: SOLID187 Geometry*.

In addition to the nodes, the element input data includes the
orthotropic or anisotropic material properties. Orthotropic and anisotropic
material directions correspond to the element coordinate directions.
The element coordinate system orientation is as described in *Linear Material Properties* in the *Material Reference*.

Element loads are described in *Nodal Loading*.
Pressures may be input as surface loads on the element faces as shown
by the circled numbers on *Figure 187.1: SOLID187 Geometry*. Positive pressures act into the element. 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 **ESYS** to orient the material properties and strain/stress
output. Use **RSYS** to choose output that follows
the material coordinate system or the global coordinate system. For
the case of hyperelastic materials, the output of stress and strain
is always with respect to the global Cartesian coordinate system rather
than following the material/element coordinate system.

KEYOPT(6) = 1 or 2 sets the element for using mixed formulation.
For details on the use of mixed formulation, see *Applications of Mixed u-P Formulations* in the *Element Reference*.

KEYOPT(15) = 1 sets the element for perfectly
matched layers (PML). For more information, see *Perfectly Matched Layers (PML) in Elastic Media* in the *Mechanical APDL Theory Reference*.

KEYOPT(16) = 1 activates steady state analysis
(defined via the **SSTATE** command). For more information,
see *Steady State Rolling* in
the *Mechanical APDL Theory Reference*.

You can apply an initial stress state to this element via the **INISTATE** command. For more information, see the **INISTATE** command, and also Initial Stress Loading in the *Basic Analysis Guide*.

The effects of pressure load stiffness are automatically included
for this element. If an unsymmetric matrix is needed for pressure
load stiffness effects, use **NROPT**,UNSYM.

The next table summarizes the element input. *Element Input* gives a general description of element input.

**Nodes**I, J, K, L, M, N, O, P, Q, R

**Degrees of Freedom**UX, UY, UZ

**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)

**Equivalent source surface flag --**MXWF (input on the

**SF**command)

**Body Loads****Temperatures --**T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P), T(Q), T(R)

**Body force densities --**The element values in the global X, Y, and Z directions.

**Special Features****KEYOPT(6)**Element formulation:

**0 --**Use pure displacement formulation (default)

**1 --**Use mixed formulation, hydrostatic pressure is constant in an element (recommended for hyperelastic materials)

**2 --**Use mixed formulation, hydrostatic pressure is interpolated linearly in an element (recommended for nearly incompressible elastoplastic materials)

**KEYOPT(15)**PML absorbing condition:

**0 --**Do not include PML absorbing condition (default)

**1 --**Include PML absorbing condition

**KEYOPT(16)**Steady state analysis flag:

**0 --**Steady state analysis disabled (default)

**1 --**Enable steady state analysis

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 187.1: SOLID187 Element Output Definitions*

Several items are illustrated in *Figure 187.2: SOLID187 Stress Output*. The element stress directions
are parallel to the element coordinate system. 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 187.1: SOLID187 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 | 3 |

PRES | Pressures P1 at nodes J, I, K; P2 at I, J, L; P3 at J, K, L; P4 at K, I, L | - | Y |

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:EQV | Equivalent elastic strains [6] | - | Y |

EPTH:X, Y, Z, XY, YZ, XZ | Thermal strains | 1 | 1 |

EPTH: EQV | Equivalent thermal strains [6] | 1 | 1 |

EPPL:X, Y, Z, XY, YZ, XZ | Plastic strains
[7] | 1 | 1 |

EPPL:EQV | Equivalent plastic strains
[6] | 1 | 1 |

EPCR:X, Y, Z, XY, YZ, XZ | Creep strains | 1 | 1 |

EPCR:EQV | Equivalent creep strains [6] | 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 | - |

NL:SEPL | Plastic yield stress | 1 | 1 |

NL:EPEQ | Accumulated equivalent plastic strain | 1 | 1 |

NL:CREQ | Accumulated equivalent creep strain | 1 | 1 |

NL:SRAT | Plastic yielding (1 = actively yielding, 0 = not yielding) | 1 | 1 |

NL:HPRES | Hydrostatic pressure | 1 | 1 |

SEND: ELASTIC, PLASTIC, CREEP, ENTO | Strain energy density | - | 1 |

LOCI:X, Y, Z | Integration point locations | - | 4 |

SVAR:1, 2, ... , N | State variables | - | 5 |

YSIDX:TENS,SHEA | Yield surface activity status for Mohr-Coloumb, soil, concrete, and joint rock material models: 1 for yielded and 0 for not yielded. | - | Y |

FPIDX: TF01,SF01, TF02,SF02, TF03,SF03, TF04,SF04 | Failure plane surface activity status for concrete and joint rock material models: 1 for yielded and 0 for not yielded. Tension and shear failure status are available for all four sets of failure planes. | - | Y |

Nonlinear solution, output only if the element has a nonlinear material, or if large-deflection effects are enabled (

**NLGEOM**,ON) for SEND.Available only at centroid as a

***GET**item.Available only if

**OUTRES**,LOCI is used.Available only if the

`UserMat`

subroutine and**TB**,STATE command are used.The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (

**MP**,PRXY); for plastic and creep this value is set at 0.5.For the shape memory alloy material model, transformation strains are reported as plasticity strain EPPL.

*Table 187.2: SOLID187 Item and Sequence Numbers* lists output available
through **ETABLE** using the Sequence Number method.
See The General Postprocessor
(POST1) in the *Basic Analysis Guide* and *The Item and Sequence Number Table* in
this reference for more information. The following notation is used
in *Table 187.2: SOLID187 Item and Sequence Numbers*:

**Name**output quantity as defined in

*Table 187.1: SOLID187 Element Output Definitions***Item**predetermined Item label for

**ETABLE**command**I,J,...,R**sequence number for data at nodes I, J, ..., R

The element must not have a zero volume.

Elements may be numbered either as shown in

*Figure 187.1: SOLID187 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. See Quadratic Elements (Midside Nodes) in the

*Modeling and Meshing Guide*for information about using midside nodes.When mixed formulation is used (KEYOPT(6) = 1 or 2), no midside nodes can be missed.

If you use the mixed formulation (KEYOPT(6) = 1 or 2), the damped eigensolver is not supported. You must use the sparse solver (default).

Stress stiffening is always included in geometrically nonlinear analyses (

**NLGEOM**,ON). Prestress effects can be activated by the**PSTRES**command.

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

**ANSYS Mechanical Pro **

Birth and death is not available.

Fracture parameter calculation is not available.

Initial state is not available.

Linear perturbation is not available.

Material force evaluation is not available.

Steady state is not available.

**ANSYS Mechanical Premium **

Birth and death is not available.

Fracture parameter calculation is not available.

Material force evaluation is not available.