3-D 8-Node Structural Solid Shell

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

SOLSH190 Element Description

SOLSH190 is used for simulating shell structures with a wide range of thickness (from thin to moderately thick). The element possesses the continuum solid element topology and features eight-node connectivity with three degrees of freedom at each node: translations in the nodal x, y, and z directions. Thus, connecting SOLSH190 with other continuum elements requires no extra efforts. A degenerate prism option is available, but should only be used as filler elements in mesh generation. The element has plasticity, hyperelasticity, stress stiffening, creep, large deflection, and large strain capabilities. It also has mixed u-P formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. The element formulation is based on logarithmic strain and true stress measures.

You can use SOLSH190 for layered applications such as modeling laminated shells or sandwich construction. The layered section definition is given by section (SECxxx) commands. Accuracy in modeling composite shells is governed by the first-order shear-deformation theory (also known as Mindlin-Reissner shell theory).

See SOLSH190 for more details about this element.

Figure 190.1:  SOLSH190 Geometry

SOLSH190 Geometry

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

x = Element x-axis if ESYS is supplied.

SOLSH190 Input Data

The geometry, node locations, and the element coordinate system for this element are shown in Figure 190.1: SOLSH190 Geometry. The element is defined by eight nodes. The element coordinate system follows the shell convention where the z axis is normal to the surface of the shell. The node ordering must follow the convention that the 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 as 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 SOLSH190 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 SOLSH190 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.

SOLSH190 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 190.1: SOLSH190 Geometry. The axis can be defined as shown:


{x}I, {x}J, . . . , {x}P = global nodal coordinates

If edges IJ and KL are parallel (rectangular or trapezoidal elements), the default orientation is the same as described in Coordinate Systems (the first surface direction is aligned with the IJ side). For elements with nonparallel edges IJ and JK, the default orientation represents the stress state better because the element uses a single point of quadrature (by default) in the element domain.

You can reorient the default first surface direction S1 in the element reference plane 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 Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 190.1: SOLSH190 Geometry. Positive pressures act into the element.

If you specify no element body load for defining temperatures--that is, you define temperatures with commands other than BFE--SOLSH190 adopts an element-wise temperature pattern and requires only eight temperatures for the eight element nodes. Unspecified nodal temperatures default to the assigned uniform temperature (TUNIF). ANSYS computes all layer interface temperatures by interpolating nodal temperatures T1 ~ T8.

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 NL. If you input exactly NL + 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.

You can use the MP command to define the isotropic or orthotropic elastic material properties and the TB,ANEL command to define anisotropic elastic material properties. Other material properties include density, damping ratios, and coefficients of thermal expansion. You may also use the TB command to define nonlinear material behavior such as plasticity, hyperelasticity, viscoelasticity, creep, and viscoplasticity.

KEYOPT(2) = 1 activates the internal strain enhancements to the element transverse-shear strains. With this option, the element is capable of quadratic transverse-shear strain distributions through the entire thickness of the element. At least three integration points through the thickness are required for this option. Use a shell section to define more integration points through the thickness.

KEYOPT(6) = 1 sets the element for using u-P 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 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 Initial State in the Mechanical APDL Advanced 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.

"SOLSH190 Input Summary" contains a summary of element input. For a general description of element input, see Element Input.

SOLSH190 Input Summary


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

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-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 -- 
Element-wise pattern (no element body load command issued):   T1, T2, T3, T4, T5, T6, T7, T8 for 8 element nodes. Temperatures at layer interface corners are computed by interpolating nodal temperatures.
Layer-wise pattern (element body load command issued):   T1, T2, T3, T4 (at bottom of layer 1), T5, T6, T7, T8 (between layers 1-2); similarly for temperatures between subsequent layers, ending with temperatures at top of layer NL (4 * (NL + 1) maximum). For a one-layer element, therefore, 8 temperatures are used.
Body force densities -- 

The element values in the global X, Y, and Z directions.

Special Features
Birth and death
Coriolis effect
Element technology autoselect
Generalized cross-section
Initial state
Large deflection
Large strain
Linear perturbation
Nonlinear stabilization
Steady state (except for the degenerated shape [prism] option)
Stress stiffening

Enhanced transverse-shear strains:

0 -- 

No enhanced transverse-shear strains (default).

1 -- 

Include enhanced transverse-shear strains.


Element formulation:

0 -- 

Use pure displacement formulation (default).

1 -- 

Use mixed u-P formulation.


Storage of layer data:

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 -- 

For multilayer elements, store data for top and bottom for all layers. (Before using this option, be aware that the amount of data involved can be very large.)


Steady state analysis flag:

0 -- 

Steady state analysis disabled (default)

1 -- 

Enable steady state analysis

SOLSH190 Element Technology

SOLSH190 employs incompatible modes to enhance the accuracy in in-plane bending situations. The satisfaction of the in-plane patch test is ensured. A separate set of incompatible modes is adopted to overcome the thickness locking in bending dominant problems. The incompatible modes introduce seven internal DOFs that are inaccessible to users and condensed out at the element level.

SOLSH190 utilizes a suite of special kinematic formulations to avoid locking when the shell thickness becomes extremely small. However, due to its shell-like behavior, SOLSH190 fails to pass the patch test if the element is distorted in the thickness direction.

SOLSH190 is fully compatible with 3-D constitutive relations. Compared to classical shell elements that are based on plane stress assumptions, SOLSH190 usually gives more accurate predictions when the shell is thick.

SOLSH190 Output Data

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

Several items are illustrated in Figure 190.2: SOLSH190 Stress Output. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this reference for more information.

Figure 190.2:  SOLSH190 Stress Output

SOLSH190 Stress Output
xo = Element x-axis if ESYS is not supplied.
x = Element x-axis if ESYS is supplied.

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

Table 190.1:  SOLSH190 Element Output Definitions

ELElement Number-Y
NODESNodes - I, J, K, L, M, N, O, P-Y
MATMaterial number-Y
XC, YC, ZCLocation where results are reportedY 2
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 [5]-Y
EPTH:X, Y, Z, XY, YZ, XZThermal strainsYY
EPTH:EQVEquivalent thermal strains [5]-Y
EPPL:X, Y, Z, XY, YZ, XZPlastic strains [6] 1 1
EPPL:EQVEquivalent plastic strains [5]- 1
EPCR:X, Y, Z, XY, YZ, XZCreep strains 1 1
EPCR:EQVEquivalent creep strains [5]- 1
EPTO:X, Y, Z, XY, YZ, XZTotal mechanical strains (EPEL + EPPL + EPCR)Y-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)--
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: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- 3
SVAR:1, 2, ... , NState variables- 4
ILSXZ SXZ interlaminar shear stress - 7
ILSYZ SYZ interlaminar shear stress - 7
ILSUM Magnitude of the interlaminar shear stress vector - 7
ILANG Angle of interlaminar shear stress vector (measured from the element x-axis toward the element y-axis in degrees) - 7
Sm: 11, 22, 12Membrane stresses-Y
Sb: 11, 22, 12Bending stresses-Y
Sp: 11, 22, 12Peak stresses-Y
St: 13, 23Averaged transverse-shear stresses-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. Available only at centroid as a *GET item.

  3. Available only if OUTRES,LOCI is used.

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

  5. The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (MP,NUXY); for plastic and creep this value is set at 0.5.

  6. For the shape memory alloy material model, transformation strains are reported as plasticity strain EPPL.

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

Table 190.2: SOLSH190 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 190.2: SOLSH190 Item and Sequence Numbers:


output quantity as defined in the Table 190.1: SOLSH190 Element Output Definitions


predetermined Item label for ETABLE command


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

Table 190.2:  SOLSH190 Item and Sequence Numbers

Output Quantity Name ETABLE and ESOL Command Input
Item E I J K L M N O P
Sm: 11SMISC36--------
Sm: 22SMISC37--------
Sm: 12SMISC38--------
Sb: 11SMISC39--------
Sb: 22SMISC40--------
Sb: 12SMISC41--------
Sp: 11 (at bottom face)SMISC42--------
Sp: 22 (at bottom face)SMISC43--------
Sp: 12 (at bottom face)SMISC44--------
Sp: 11 (at top face)SMISC45--------
Sp: 22 (at top face)SMISC46--------
Sp: 12 (at top face)SMISC47--------
St: 13SMISC48--------
St: 23SMISC49--------

Output Quantity Name ETABLE and ESOL Command Input
Item Bottom of Layer i Top of Layer NL
ILSXZSMISC8 * (i - 1) + 518 * (NL - 1) + 52
ILSYZSMISC8 * (i - 1) + 538 * (NL - 1) + 54
ILSUMSMISC8 * (i - 1) + 558 * (NL - 1) + 56
ILANGSMISC8 * (i - 1) + 578 * (NL - 1) + 58

SOLSH190 Assumptions and Restrictions

  • Zero-volume elements are not allowed.

  • Elements may be numbered either as shown in Figure 190.1: SOLSH190 Geometry or may have the planes IJKL and MNOP interchanged. 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).

  • 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.)

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

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

  • Using both hyperelastic and elastoplastic layers in the same element can produce unpredictable results and is not recommended.

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

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

  • For sandwich plates or shells, analyze the face and core of the sandwich using stacked layers of SOLSH190 elements. Doing so accounts for the large variation in face and core material properties, and the distortion through-the-thickness. (Sandwich modeling can yield excessively stiff results if SOLSH190 is used as a single element through-the-thickness.) Generally, it is good practice to use additional elements through-the-thickness when the material properties between layers vary significantly.

SOLSH190 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.

  • Initial state is not available.

  • Linear perturbation is not available.

ANSYS Mechanical Premium 

  • Birth and death is not available.

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