SOLID185


3D 8-Node Structural Solid

Valid Products: Pro | Premium | Enterprise | PrepPost | Solver | AS add-on

SOLID185 Element Description

SOLID185 is used for 3D modeling of solid structures. It is defined by eight nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions. The element has plasticity, hyperelasticity, stress stiffening, creep, 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.

SOLID185 is available in two forms:

See SOLID185 for more details about this element.

A higher-order version of the SOLID185 element is SOLID186.

SOLID185 Homogeneous Structural Solid Element Description

SOLID185 Structural Solid is suitable for modeling general 3D solid structures. It allows for prism, tetrahedral, and pyramid degenerations when used in irregular regions. Various element technologies such as B-bar, uniformly reduced integration, and enhanced strains are supported.

Figure 185.1: SOLID185 Homogeneous Structural Solid Geometry

SOLID185 Homogeneous Structural Solid Geometry

SOLID185 Homogeneous Structural Solid Input Data

The geometry and node locations for this element are shown in Figure 185.1: SOLID185 Homogeneous Structural Solid Geometry. The element is defined by eight nodes and the orthotropic material properties. The default element coordinate system is along global directions. You may define an element coordinate system using ESYS, which forms the basis for orthotropic material directions.

Element loads are described in Element Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 185.1: SOLID185 Homogeneous Structural Solid 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). For any other input temperature pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is used instead of TUNIF.

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

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

KEYOPT(16) = 1 activates steady-state analysis (defined via SSTATE). For more information, see Steady-State Rolling in the Theory Reference. For a steady-state analysis, elements must be numbered as shown in Figure 185.1: SOLID185 Homogeneous Structural Solid Geometry.

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

You can apply an initial stress state to this element (INISTATE). For more information, see Initial State in the Advanced Analysis Guide.

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.

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

"SOLID185 Homogeneous Structural Solid Input Summary" contains a summary of element input. For a general description of element input, see Element Input.

SOLID185 Homogeneous Structural Solid Input Summary

Nodes

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

Degrees of Freedom

UX, UY, UZ

Real Constants
None, if KEYOPT(2) = 0,
HGSTF - Hourglass stiffness scaling factor if KEYOPT(2) = 1. Any positive number is valid. Default = 1.0. If set to 0.0, the value resets to default.
Material Properties
TB command: See Element Support for Material Models for this element.
MP command: EX, EY, EZ, PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ), GXY, GYZ, GXZ, ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), DENS, ALPD, BETD, DMPR, DMPS
Surface Loads
Pressures -- 
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)
To define general surface loads (or surface tractions) on the faces, issue SFCONTROL.
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)

Body force densities -- 

The element values in the global X, Y, and Z directions. For analyses supporting complex loading, imaginary X, Y, and Z values are supported (see the BFE command for details).

Special Features
KEYOPT(2)

Element technology:

0 -- 

Full integration with method (default)

1 -- 

Uniform reduced integration with hourglass control

2 -- 

Enhanced strain formulation

3 -- 

Simplified enhanced strain formulation

KEYOPT(3)

Layer construction:

0 -- 

Structural Solid (default) -- nonlayered

1 -- 

Layered Solid (not applicable to SOLID185 Structural Solid)

KEYOPT(6)

Element formulation:

0 -- 

Use pure displacement formulation (default)

1 -- 

Use mixed u-P formulation

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

KEYOPT(17)

Extra surface output:

0 -- 

Basic element solution (default)

4 -- 

Surface solution for faces with nonzero pressure

SOLID185 Homogeneous Structural Solid Element Technology

SOLID185 Homogeneous Structural Solid uses the full-integration method (also known as the selective reduced integration method), enhanced strain formulation, simplified enhanced strain formulation, or uniform reduced integration.

When enhanced strain formulation (KEYOPT(2) = 2) is selected, the element introduces nine internal (user-inaccessible) degrees of freedom to handle shear locking, and four internal degrees of freedom to handle volumetric locking.

For more information, see Element Technologies.

SOLID185 Homogeneous Structural Solid Output Data

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

Several items are illustrated in Figure 185.2: SOLID185 Homogeneous Structural Solid Stress Output. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this document for more information.

Figure 185.2: SOLID185 Homogeneous Structural Solid Stress Output

SOLID185 Homogeneous Structural Solid Stress Output

Stress directions shown are for global directions.


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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 185.1: SOLID185 Homogeneous Structural Solid Element Output Definitions

Name Definition O R
ELElement Number-Y
NODESNodes - I, J, K, L, M, N, O, P-Y
MATMaterial number-Y
VOLU:Volume-Y
XC, YC, ZCLocation where results are reportedY 3
PRESPressures P1 at nodes J, I, L, K; P2 at I, J, N, M; P3 at J, K, O, N; P4 at K, L, P, O; P5 at L, I, M, P; P6 at M, N, O, P-Y
TEMPTemperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P)-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 strains 2 2
EPTH:EQVEquivalent thermal strains [6] 2 2
EPPL:X, Y, Z, XY, YZ, XZPlastic strains [7] 1 1
EPPL:EQVEquivalent plastic strains [6] 1 1
EPCR:X, Y, Z, XY, YZ, XZCreep strains 1 1
EPCR:EQVEquivalent creep strains [6] 1 1
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 stress 1 1
NL:EPEQAccumulated equivalent plastic strain 1 1
NL:CREQAccumulated equivalent creep strain 1 1
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding) 1 1
NL:PLWKPlastic work/volume 1 1
NL:HPRESHydrostatic pressure 1 1
SEND:ELASTIC, PLASTIC, CREEP, ENTOStrain energy densities- 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 185.2: SOLID185 Homogeneous Structural Solid Item and Sequence Numbers lists output available via ETABLE using the Sequence Number method. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 185.2: SOLID185 Homogeneous Structural Solid Item and Sequence Numbers:

Name

output quantity as defined in the Table 185.1: SOLID185 Homogeneous Structural Solid Element Output Definitions

Item

predetermined Item label for ETABLE command

I,J,...,P

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

Table 185.2: SOLID185 Homogeneous Structural Solid Item and Sequence Numbers

Output Quantity Name ETABLE and ESOL Command Input
Item I J K L M N O P
P1SMISC2143----
P2SMISC56--87--
P3SMISC-910--1211-
P4SMISC--1314--1615
P5SMISC18--1719--20
P6SMISC----21222324

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

SOLID185 Homogeneous Structural Solid Assumptions and Restrictions

  • Zero-volume elements are not allowed.

  • Elements may be numbered either as shown in Figure 185.1: SOLID185 Homogeneous Structural Solid Geometry, or may have the planes IJKL and MNOP interchanged (except when KEYOPT(16) = 1). The element may not be twisted such that the element has two separate volumes (which occurs most frequently when the elements are not numbered properly).

  • For a steady-state analysis (KEYOPT(16) = 1), elements must be numbered as shown in Figure 185.1: SOLID185 Homogeneous Structural Solid Geometry.

  • All elements must have eight nodes. You can form a prism-shaped element by defining duplicate K and L and duplicate O and P node numbers. (See Degenerated Shape Elements.) Pyramid and tetrahedral shapes are also available.

  • For the degenerated shape elements where the or enhanced strain formulations are specified, degenerated shape functions and a conventional integration scheme are used.

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

  • For modal cyclic symmetry analyses, Ansys, Inc. recommends using enhanced strain formulation.

  • Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). Prestress effects can be activated by the PSTRES command.

This element has a layered option (KEYOPT(3) = 1). See "SOLID185 Layered Structural Solid Assumptions and Restrictions" for additional information.

SOLID185 Layered Structural Solid Element Description

Use SOLID185 Layered Solid to model layered thick shells or solids. The layered section definition is specified via section (SECxxx) commands. A prism degeneration option is also available.

Figure 185.3: SOLID185 Layered Structural Solid Geometry

SOLID185 Layered Structural Solid Geometry

xo = Element x-axis if ESYS is not supplied.

x = Element x-axis if ESYS is supplied.


SOLID185 Layered Structural Solid Input Data

The geometry and node locations for this element are shown in Figure 185.3: SOLID185 Layered Structural Solid Geometry. The element is defined by eight nodes. A prism-shaped element may be formed by defining the same node numbers for nodes K and L, and O and P.

In addition to the nodes, the element input data includes the anisotropic material properties. Anisotropic material directions correspond to the layer coordinate directions which are based on the element coordinate system. The element coordinate system follows the shell convention where the z axis is normal to the surface of the shell. The nodal ordering must follow the convention that I-J-K-L and M-N-O-P element faces represent the bottom and top shell surfaces, respectively. You can change the orientation within the plane of the layers via the ESYS command in the same way that you would for shell elements (as described in Coordinate Systems). To achieve the correct nodal ordering for a volume mapped (hexahedron) mesh, you can use the VEORIENT command to specify the desired volume orientation before executing the VMESH command. Alternatively, you can use the EORIENT command after automatic meshing to reorient the elements to be in line with the orientation of another element, or to be as parallel as possible to a defined ESYS axis.

Layered Section Definition Using Section Commands

You can associate SOLID185 Layered Solid with a shell section (SECTYPE). The layered composite specifications (including layer thickness, material, orientation, and number of integration points through the thickness of the layer) are specified via shell section (SECxxx) commands. You can use the shell section commands even with a single-layered element. The program obtains the actual layer thicknesses used for element calculations by scaling the input layer thickness so that they are consistent with the thickness between the nodes.

You can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. Two points are located on the top and bottom surfaces respectively and the remaining points are distributed equal distance between the two points. The element requires at least two points through the entire thickness. When no shell section definition is provided, the element is treated as single-layered and uses two integration points through the thickness.

SOLID185 Layered Solid does not support real constant input for defining layer sections.

Other Input

The default orientation for this element has the S1 (shell surface coordinate) axis aligned with the first parametric direction of the element at the center of the element and is shown as xo in Figure 185.3: SOLID185 Layered Structural Solid Geometry.

The default first surface direction S1 can be reoriented in the element reference plane (as shown in Figure 185.3: SOLID185 Layered Structural Solid Geometry) via the ESYS command. You can further rotate S1 by angle THETA (in degrees) for each layer via the SECDATA command to create layer-wise coordinate systems. See Coordinate Systems for details.

Element loads are described in Element Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 185.3: SOLID185 Layered Structural Solid Geometry. Positive pressures act into the element.

If you specify no element body load for defining temperatures--that is, if you define temperatures with commands other than BFE--SOLID185 Layered Solid adopts an element-wise temperature pattern and requires only eight temperatures for the eight element corner 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 nodal temperatures default to TUNIF. Mechanical APDL calculates all layer interface temperatures by interpolating nodal temperatures.

Alternatively, you can input temperatures as element body loads at the corners of the outside faces of the element and at the corners of the interfaces between layers. In such a case, the element uses a layer-wise pattern. Temperatures T1, T2, T3, T4 are used for the bottom of layer 1, temperatures T5, T6, T7, T8 are used for interface corners between layers 1 and 2, and so on between successive layers, ending with temperatures at the top layer NLayer. If you input exactly NLayer+1 temperatures, one temperature is used for the four bottom corners of each layer, and the last temperature is used for the four top corner temperatures of the top layer. The first corner temperature T1 defaults to TUNIF. If all other corner temperatures are unspecified, they default to T1. For any other input pattern, unspecified temperatures default to TUNIF.

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

KEYOPT(16) = 1 activates steady-state analysis (defined via SSTATE). For more information, see Steady-State Rolling in the Theory Reference. For a steady-state analysis, elements must be numbered as shown in Figure 185.3: SOLID185 Layered Structural Solid Geometry.

You can apply an initial stress state to this element (INISTATE). For more information, see Initial State in the Advanced Analysis Guide.

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

The following table summarizes the element input. Element Input provides a general description of element input.

SOLID185 Layered Structural Solid Input Summary

Nodes

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

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, PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ),
ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ),
DENS, GXY, GYZ, GXZ, ALPD, BETD
Surface Loads
Pressures -- 
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)
Equivalent source surface flag -- 

MXWF (input on the SF command)

Body Loads
Temperatures -- 

T1, T2, T3, T4 at bottom of layer 1;  T5, T6, T7, T8 between layers 1-2; similarly for between successive layers, ending with temperatures at top of layer NLayer (4 * (NLayer + 1) maximum)

Body force densities -- 

The element values in the global X, Y, and Z directions. For analyses supporting complex loading, imaginary X, Y, and Z values are supported (see the BFE command for details).

Special Features
KEYOPT(2)

Element technology:

2 -- 

Enhanced strain formulation

3 -- 

Simplified enhanced strain formulation (default)

KEYOPT(3)

Layer construction:

0 -- 

Structural Solid (not applicable to SOLID185 Layered Solid)

1 -- 

Layered Solid

KEYOPT(6)

Element formulation:

0 -- 

Use pure displacement formulation (default)

1 -- 

Use mixed formulation

KEYOPT(8)

Layer data storage:

0 -- 

For multi-layer elements, store data for bottom of bottom layer and top of top layer. For single-layer elements, store data for TOP and BOTTOM. (Default)

1 -- 

Store top and bottom data for all layers. (The volume of data may be considerable.)

KEYOPT(16)

Steady-state analysis flag:

0 -- 

Steady-state analysis disabled (default)

1 -- 

Enable steady-state analysis

SOLID185 Layered Structural Solid Element Technology

SOLID185 Layered Structural Solid uses enhanced strain formulation or simplified enhanced strain formulation.

When enhanced strain formulation (KEYOPT(2) = 2) is selected, the element introduces nine internal (user-inaccessible) degrees of freedom to handle shear locking, and four internal degrees of freedom to handle volumetric locking.

For more information, see Element Technologies.

SOLID185 Layered Structural Solid Output Data

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

Several items are illustrated in Figure 185.4: SOLID185 Layered Structural Solid Stress Output. See Filling the Element Table for Variables Identified By Sequence Number in the Basic Analysis Guide and The Item and Sequence Number Table in this document for more information.

Figure 185.4: SOLID185 Layered Structural Solid Stress Output

SOLID185 Layered Structural Solid Stress Output

The element stress directions are parallel to the layer coordinate system.


KEYOPT(8) controls the amount of data output to the results file for processing with the LAYER command. Interlaminar shear stress is available as SYZ and SXZ evaluated at the layer interfaces. KEYOPT(8) must be set to 1 to output these stresses in POST1. 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 185.3: SOLID185 Layered Structural Solid Element Output Definitions

Name Definition O R
ELElement Number-Y
NODESNodes - I, J, K, L, M, N, O, P-Y
MATMaterial number-Y
VOLU:Volume-Y
XC, YC, ZCLocation where results are reportedY 3
PRESPressures P1 at nodes J, I, L, K; P2 at I, J, N, M; P3 at J, K, O, N;  P4 at K, L, P, O; P5 at L, I, M, P;  P6 at M, N, O, P-Y
TEMPT1, T2, T3, T4 at bottom of layer 1; T5, T6, T7, T8 between layers 1-2; similarly for between successive layers, ending with temperatures at top of layer NL (4 * (NL + 1) maximum)-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 strains 2 2
EPTH:EQVEquivalent thermal strains [6] 2 2
EPPL:X, Y, Z, XY, YZ, XZPlastic strains [7] 1 1
EPPL:EQVEquivalent plastic strains [6] 1 1
EPCR:X, Y, Z, XY, YZ, XZCreep strains 1 1
EPCR:EQVEquivalent creep strains [6] 1 1
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 stress 1 1
NL:EPEQAccumulated equivalent plastic strain 1 1
NL:CREQAccumulated equivalent creep strain 1 1
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding) 1 1
NL:PLWKPlastic work/volume 1 1
NL:HPRESHydrostatic pressure 1 1
SEND:ELASTIC, PLASTIC, CREEP, ENTOStrain energy densities- 1
N11, N22, N12In-plane forces (per unit length)-Y
M11, M22, M12Out-of-plane moments (per unit length)-Y
Q13, Q23Transverse-shear forces (per unit length)-Y
LOCI:X, Y, ZIntegration point locations- 4
SVAR:1, 2, ... , NState variables- 5
ILSXZ SXZ interlaminar shear stress - 9
ILSYZ SYZ interlaminar shear stress - 9
ILSUMMagnitude of the interlaminar shear stress vector - 8, 9
ILANG Angle of interlaminar shear stress vector (measured from the element x-axis toward the element y-axis in degrees) - 9
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.

  8. The components are combined as and the largest value of σil is output as the maximum interlaminar shear stress.

  9. Available only if a valid shell section (SECTYPE,,SHELL) is defined for the element.

Table 185.4: SOLID185 Layered Structural Solid Item and Sequence Numbers lists output available via ETABLE using the Sequence Number method. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 185.4: SOLID185 Layered Structural Solid Item and Sequence Numbers:

Name

output quantity as defined in Table 185.3: SOLID185 Layered Structural Solid Element Output Definitions

Item

predetermined Item label for ETABLE command

I,J,...,P

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

Table 185.4: SOLID185 Layered Structural Solid Item and Sequence Numbers

Output Quantity Name ETABLE and ESOL Command Input
Item E I J K L M N O P
P1SMISC-2143----
P2SMISC-56--87--
P3SMISC--910--1211-
P4SMISC---1314--1615
P5SMISC-18--1719--20
P6SMISC-----21222324
THICKSMISC27--------
N11SMISC28--------
N22SMISC29--------
N12SMISC30--------
M11SMISC31--------
M22SMISC32--------
M12SMISC33--------
Q13SMISC34--------
Q23SMISC35--------
Output Quantity Name ETABLE and ESOL Command Input
Item Bottom of Layer i Top of Layer NL
ILSXZ SMISC 8 * (i - 1) + 418 * (NL - 1) + 42
ILSYZ SMISC 8 * (i - 1) + 43 8 * (NL - 1) + 44
ILSUM SMISC 8 * (i - 1) + 45 8 * (NL - 1) + 46
ILANG SMISC 8 * (i - 1) + 47 8 * (NL - 1) + 48

SOLID185 Layered Structural Solid Assumptions and Restrictions

  • Zero-volume elements are not allowed.

  • Elements can be numbered either as shown in Figure 185.3: SOLID185 Layered Structural Solid Geometry, or may have the planes IJKL and MNOP interchanged (except when KEYOPT(16) = 1). The element may not be twisted such that the element has two separate volumes (which occurs most frequently when the elements are not numbered properly).

  • For a steady-state analysis (KEYOPT(16) = 1), elements must be numbered as shown in Figure 185.3: SOLID185 Layered Structural Solid Geometry.

  • All elements must have eight nodes. You can form a prism-shaped element by defining duplicate K and L and duplicate O and P node numbers. (See Degenerated Shape Elements.)

  • This element is primarily intended for conveniently modeling the in-plane effects in layered thick shells or solids. The in-plane stiffness is the average of the individual layer stiffnesses. For complicated through-thickness behaviors, consider using multiple layers of homogeneous (non-layered) SOLID185 elements.

  • If you use the mixed formulation (KEYOPT(6) = 1), the damped eigensolver is not supported. Use the default sparse solver.

  • 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.

  • If the material of a layer is hyperelastic, the layer orientation angle has no effect.

  • To obtain more accurate transverse shear results, use multiple elements through the thickness.

SOLID185 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  —  

  • Layered solid (KEYOPT(3) = 1) is not available.

  • Birth and death is not available.

  • Fracture parameter calculation is not available.

  • Initial state is not available.

  • Material force evaluation is not available.

  • Rezoning is not available.

  • Steady state is not available.

Ansys Mechanical Premium  —  

  • Fracture parameter calculation is not available.

  • Material force evaluation is not available.

  • Rezoning is not available.