3-D 10-Node Tetrahedral Structural Solid

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

SOLID187 Element Description

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.

Figure 187.1:  SOLID187 Geometry

SOLID187 Geometry

SOLID187 Input Data

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 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.

KEYOPT(6) = 1 or 2 sets the element for using mixed formulation. For details on the use of mixed formulation, see .

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.

For extra surface output, KEYOPT(17) = 4 activates surface solution for faces with nonzero pressure. For more information, see Surface Solution in the Mechanical APDL Element 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.

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.

SOLID187 Input Summary


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

Degrees of Freedom


Real Constants


Material Properties
TB command: See Element Support for Material Models for this element.
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
Birth and death
Coriolis effect
Element technology autoselect
Fracture parameter calculation
Initial stress import
Large deflection
Large strain
Linear perturbation
Material force evaluation
Nonlinear adaptivity
Nonlinear stabilization
Steady state
Stress stiffening

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)


PML absorbing condition:

0 -- 

Do not include PML absorbing condition (default)

1 -- 

Include PML absorbing condition


Steady state analysis flag:

0 -- 

Steady state analysis disabled (default)

1 -- 

Enable steady state analysis


Extra surface output:

0 -- 

Basic element solution (default)

4 -- 

Surface solution for faces with nonzero pressure

SOLID187 Output Data

The solution output associated with the element is in two forms:

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.

Figure 187.2:  SOLID187 Stress Output

SOLID187 Stress Output

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

ELElement Number-Y
NODESNodes - I, J, K, L-Y
MATMaterial number-Y
XC, YC, ZCLocation where results are reportedY3
PRESPressures P1 at nodes J, I, K; P2 at I, J, L; P3 at J, K, L; P4 at K, I, L-Y
TEMPTemperatures T(I), T(J), T(K), T(L)-Y
S:X, Y, Z, XY, YZ, XZStressesYY
S:1, 2, 3Principal stresses-Y
S:INTStress intensity-Y
S:EQVEquivalent stress-Y
EPEL:X, Y, Z, XY, YZ, XZElastic strainsYY
EPEL:EQVEquivalent elastic strains [6]-Y
EPTH:X, Y, Z, XY, YZ, XZThermal strains11
EPTH: EQVEquivalent thermal strains [6]11
EPPL:X, Y, Z, XY, YZ, XZPlastic strains [7]11
EPPL:EQVEquivalent plastic strains [6]11
EPCR:X, Y, Z, XY, YZ, XZCreep strains11
EPCR:EQVEquivalent creep strains [6]11
EPTO:X, Y, Z, XY, YZ, XZTotal mechanical strains (EPEL + EPPL + EPCR)Y-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)Y-
NL:SEPLPlastic yield stress11
NL:EPEQAccumulated equivalent plastic strain11
NL:CREQAccumulated equivalent creep strain11
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding)11
NL:HPRESHydrostatic pressure11
SEND: ELASTIC, PLASTIC, CREEP, ENTOStrain energy density-1
LOCI:X, Y, ZIntegration point locations-4
SVAR:1, 2, ... , NState variables-5
YSIDX:TENS,SHEAYield 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,SF04Failure 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

  1. Nonlinear solution, output only if the element has a nonlinear material, or if large-deflection effects are enabled (NLGEOM,ON) for SEND.

  2. Output only if element has a thermal load

  3. Available only at centroid as a *GET item.

  4. Available only if OUTRES,LOCI is used.

  5. Available only if the UserMat subroutine and TB,STATE command are used.

  6. 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.

  7. 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:


output quantity as defined in Table 187.1: SOLID187 Element Output Definitions


predetermined Item label for ETABLE command


sequence number for data at nodes I, J, ..., R

Table 187.2:  SOLID187 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input

See Surface Solution for the item and sequence numbers for surface output (KEYOPT(17) = 4) for the ETABLE command

SOLID187 Assumptions and Restrictions

  • 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.

SOLID187 Product Restrictions

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.

Release 18.2 - © ANSYS, Inc. All rights reserved.