Surface-projection-based contact is available for the 3-D surface-to-surface contact elements, CONTA173 and CONTA174. Surface projection based contact enforces contact constraints on an overlapping region of contact and target surfaces rather than on individual contact nodes or Gauss points. The advantages of using this technique are:

This contact method is implemented by setting KEYOPT(4) = 3 on the CONTA173 and CONTA174 elements. For more information, see Using the Surface Projection Based Contact Method (KEYOPT(4) = 3) in the Contact Technology Guide.

In some contact applications, using a faceted surface in place of the true curved geometry can significantly affect the accuracy of contact stresses. An optional geometric correction feature has been introduced for nearly spherical and revolute (cylindrical) contact surfaces. Geometry correction, which is defined via SECTYPE and SECDATA section commands, is available for 3-D surface-to-surface contact elements: TARGE170, CONTA173, and CONTA174. Applying geometry correction reduces the discretization error associated with faceted surfaces and can greatly improve the accuracy of contact stresses for certain types of curved contact/target surfaces. For more information, see Geometry Correction for Contact and Target Surfaces in the Contact Technology Guide.

Previously, the ramping option for initial contact penetration (KEYOPT(9) = 2 or 4) was active only within the first load step. A new contact element real constant, STRM, allows you to define the load step number in which the ramping option will take place for a given contact pair. This real constant is useful for modeling multiple interference fits that occur sequentially (that is, the interference present in each contact pair can be resolved in different load steps). STRM is available for contact elements CONTA171 through CONTA177.

Contact offset CNOF can now be defined as a function of time and/or x, y, z location (in global or local coordinates) by using tabular input, allowing more flexibility for accurately modeling contact behavior. Consider the case of a CAD geometry based on nominal values. The geometry may lack a slight curvature variation that is important for analysis purposes. Moving nodes to the actual positions can be a tedious process, yet using the original geometry and neglecting the slight variation in curvature will result in a different contacting area. Consequently, inputting CNOF as a function of location allows you to easily include curvature that varies with location without having to modify the original CAD geometry. For more information, see Adjusting Initial Contact Conditions in the Contact Technology Guide.

When using impact constraints to model impact between rigid bodies, a coefficient of restitution can now be input via the real constant COR to model loss of energy during impact. The coefficient of restitution defines the ratio of relative velocity of rigid bodies after impact to relative velocity of rigid bodies before impact; its value varies between 0 and 1. A value of 0 indicates that the rigid bodies stick to each other after impact, while a value of 1 indicates that the rigid bodies rebound after impact with the magnitude of relative velocity after impact being the same as before impact. The new COR real constant is available for contact elements CONTA171 through CONTA178.

The following new output quantities are available (via the ETABLE command) for contact elements CONTA171 through CONTA177: slip rate (VREL); fluid penetration starting time (FSTART ); and true geometric gap/penetration at current converged substep (GGAP). In addition, a pair-based contacting area (summation of areas where contact is closed) can be reported through the NLHIST and NLDIAG commands.

Use the new REINF263 element with a standard 2-D solid or shell element (referred to as the base element) to provide extra reinforcing to that element. REINF263 uses a smeared approach and is suitable for modeling evenly spaced reinforcing fibers that appear in layered form. Each reinforcing layer contains a cluster of fibers with unique orientation, material, and cross-section area, and is simplified as a homogenous membrane having unidirectional stiffness. You can specify multiple layers of reinforcing in one REINF263 element. The nodal locations, degrees of freedom, and connectivity of the element are identical to those of the base element.

Use the new SURF159 element to model axisymmetric solid surface loads acting on general axisymmetric solid (SOLID272 or SOLID273) elements. The element has linear or quadratic displacement behavior on the master plane and is well suited to modeling irregular meshes on the master plane. It is defined by two or three nodes on the master plane, and nodes created automatically in the circumferential direction based on the master plane nodes. The total number of nodes depends on the number of nodal planes. Each node has three degrees of freedom: translations in the nodal x, y, and z directions. Various loads and surface effects can exist simultaneously.

The new hydrostatic fluid elements, HSFLD241 and HSFLD242, allow you to model fluids that are fully enclosed by 2-D/axisymmetric solids, 3-D solids, or 3-D shells. The elements are well suited for calculating fluid volume and pressure for coupled problems involving fluid-solid interaction. The pressure in the fluid volume is assumed to be uniform (no pressure gradients), so sloshing effects cannot be included. Temperature effects and compressibility may be included, but fluid viscosity cannot be included. The elements have linear and quadratic displacement behavior for nodes shared with the enclosing solid. A single pressure node with a hydrostatic pressure degree of freedom is shared by all the hydrostatic fluid elements defining a fluid volume. The elements can be used in static and transient dynamic analyses with various loads and boundary conditions.

A preintegrated composite beam section is an abstract cross-section type that allows you to define a fully populated but symmetrical cross-section stiffness and mass matrix directly. You can use preintegrated composite beam sections when using BEAM188 or BEAM189 elements, provided that linear elastic material behavior is acceptable. Four new commands (CBMX, CBMD, CBTMP, and CBTE) are available for specifying the individual component quantities necessary for defining a preintegrated composite beam section. For more information, see Using Preintegrated Composite Beam Sections in the Structural Analysis Guide.

Support has been added for Puck and Hashin fiber and matrix failure criteria. The new FCTYP command specifies which failure criteria are active for postprocessing and includes support for Puck and Hashin failure criteria. Output commands (PxxSOL), along with the ETABLE postprocessing command, have also been enhanced to support the new failure criteria.

A new data table (TB,FCLI) is available for defining material strength limits used to calculate failure criteria. For more information, see Material Strength Limits (TB,FCLI) in the Element Reference.

When layers are defined via cross sections, the number layers for current-technology shell, solid and elbow elements is no longer restricted to 250. Likewise, the number of temperatures that can be used with those elements is no longer limited to 1024. The changes apply to the following elements: SHELL181, SHELL281, SHELL208, SHELL209, ELBOW290, SOLID185, SOLID186, SOLSH190.

An enhanced transverse-shear strain formulation has been implemented in solid-shell element SOLSH190. Previously, SOLSH190 could predict only constant transverse-shear strains through the thickness. With the new formulation, SOLSH190 is capable of parabolic transverse-shear distribution in the thickness direction, leading to significant improvement in particularly thick shell models.

Manual rezoning is now available for 3-D analyses. The remeshing method uses a generic new mesh (.cdb file) imported via a separate meshing step (REMESH,READ). Rezoning also supports additional solid and contact elements. For more information, see Manual Rezoning in the Advanced Analysis Techniques Guide.

Force density is now supported as a vector (BFE,Element,FORCE). The vector is interpreted in the global Cartesian coordinate system. Only constant values are valid (and not tabular loads).

The force density is distributed to elements nodes via the shape functions. Density values and directions remain unchanged as the element deforms; therefore, the total force varies as the element volume changes.

Force-density support is available in the following elements: PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, SOLSH190, PLANE223, SOLID226, SOLID227, and SOLID285.

Three new wave types (specified via KWAVE on the OCDATA command) are available for ocean loading: irregular wave, Shell new wave, and constrained new wave.

The irregular wave is created by adding the parameters (wave height, velocity, and acceleration) of a number of regular airy waves (wave components) with random phases and amplitudes corresponding to the required spectrum. The spectrum is divided into a number of equal energy strips based on the number of wave components specified, and each of the strips is a wave component. The frequency of the wave component is the frequency at the centroid of the strip. The amplitude of a wave component is given by the square root of twice the area of the strip.

The Shell new wave model is similar to irregular wave. It uses a statistically based linear superposition of linear wave components to define the wave profile and associated kinematics representing the most likely maximum condition of a real sea.

A constrained new wave embeds a Shell new wave into an irregular wave so that the maximum crest amplitude as given by the new wave occurs at a specific time and position while the statistical nature of the random sea is preserved.

For more information, see Hydrodynamic Loads on Line Elements in the Theory Reference for the Mechanical APDL and Mechanical Applications.

Most computational resources in a modal analysis are dedicated to mode extraction. By reusing these results, fewer resources are required. All downstream analysis involving eigenmodes can now reuse the modes from the Jobname.MODE file in a subsequent spectrum analysis, modal transient or harmonic analysis, or QR damped complex-mode-extraction modal-based methods.

For more information, see Reusing Eigenmodes in the Structural Analysis Guide.

The summation of the element nodal forces in a spectrum analysis now takes into account the forces signs. Applicable postprocessing commands are: NFORCE, FSUM, PRRFOR, and PRNLD.

To define the input spectrum in a multipoint response spectrum (MPRS) analysis, use the following new commands: SPDAMP, SPFREQ, SPUNIT, and SPVAL. The SPDAMP command allows you to input a damping ratio for each spectrum curve.

To display the input spectrum, issue the new SPGRAPH command.

In MPRS and power spectral density (PSD) analyses, you can now define the excitation direction in a global coordinate system via the SED command.

Spectrum analysis enhancements have also been made to other commands.

In mode superposition harmonic or transient analysis, the enforced motion method can be used when the excitations are caused by imposed motions (such as acceleration or displacement). For more information, see Enforced Motion Method for Mode Superposition Transient and Harmonic Analysis in the Structural Analysis Guide and Enforced Motion in Structural Analysis in the Theory Reference for the Mechanical APDL and Mechanical Applications.

The unsymmetric extraction method (MODOPT,UNSYM) is now applicable to non-damped models when the system matrices are unsymmetric, allowing a larger number of eigenvalues to be extracted in less time using an automated frequency shift strategy.

The unsymmetric and damped (MODOPT,DAMP) extraction methods are now supported using distributed memory parallelism in Distributed ANSYS.

For more information, see Unsymmetric Method, Comparing Mode-Extraction Methods, and the MODOPT command documentation.

The linear perturbation process supports modal solutions for Block Lanczos, UNSYM, DAMP, and QRDAMP eigensolvers (MODOPT). The solution accuracy of QRDAMP for brake squeal analysis has been greatly improved when QRDAMP is used in conjunction with linear perturbation and the CMROTATE command.

The HROPT command now selects the most efficient method to solve an acoustic harmonic analysis by defaulting to AUTO (HROPT,AUTO). Depending on the model, either the full method or the Variational Technology (VT) method is selected. Using the VT method can reduce the time for an analysis by up to a factor of 10, especially if the number of harmonic solutions (specified with NSUBST command) is large.

For more information, see the HROPT command documentation, Harmonic Response Analysis, and Harmonic Sweep Using VT Accelerator.

This capability is also available for harmonic cyclic symmetry analyses. For more information, see the HROPT command documentation and Cyclic Symmetry Analysis.

Spin softening is now activated by default in prestressed modal analyses when any rotational velocities are specified. The KSPIN option on the OMEGA and CMOMEGA commands is no longer documented.

Energy-release rates can now be calculated using VCCT technology for two-dimensional continuum elements, such as PLANE182, and the 3-D continuum element SOLID185. To specify the VCCT calculation type, use the enhanced CINT command. For more information, see Fracture Mechanics Parameters in the Structural Analysis Guide.

The new response function option for hyperelastic material constants (TB,HYPER,,,,RESPONSE) uses experimental data (TB,EXPE) to determine the constitutive response functions. The response functions (first derivatives of the hyperelastic potential) are used to determine the hyperelastic constitutive behavior of the material.

The response function hyperelastic option can include experimental data from uniaxial tension, uniaxial compression, equibiaxial, and/or planar shear tests. Additionally, the volumetric response can be specified via experimental pressure-volume data or a polynomial volumetric potential function.

For more information, see Response Function Hyperelastic Option in the Structural Analysis Guide, Response Function Hyperelastic Material Constants in the Element Reference, and Experimental Response Functions in the Theory Reference for the Mechanical APDL and Mechanical Applications.

The new extended tube model is available as a hyperelastic material option (TB,HYPER,,,,ETUBE). The model simulates filler-reinforced elastomers and other rubber-like materials, supports material curve-fitting, and is available in all current-technology continuum, shell, and pipe elements.

For more information, see the documentation for the TB command, Extended Tube Material Constants in the Element Reference, and Extended Tube Model in the Theory Reference for the Mechanical APDL and Mechanical Applications.

The new Gurson-Chaboche material model option is an extension of the Gurson plasticity model. The option is used for modeling porous metal materials, combining both isotropic and kinematic hardening effects. It accounts for microscopic material behaviors, such as void dilatancy, void nucleation, and void coalescence into macroscopic plasticity models. Compared to the Gurson option with isotropic hardening only, the new option can provide more realistic deformation results for cyclic loading.

The Gurson-Chaboche model first requires the input parameters for Gurson plasticity with isotropic hardening (TB,GURSON), followed by additional input parameters for Chaboche kinematic hardening (TB,CHABOCHE).

For more information, see Gurson-Chaboche Material Model in the Structural Analysis Guide, and Gurson Plasticity with Isotropic/Chaboche Kinematic Hardening in the Theory Reference for the Mechanical APDL and Mechanical Applications.

When specifying Newton-Raphson options in an applicable static creep analysis, you now have the option of using modified Newton-Raphson with a creep-ratio limit in order to reduce the solution time. For more information, see the NROPT command description.

The cap creep model is an extension of the cap (rate-independent plasticity) model. The extension is based on creep theory similar to that of the extended Drucker-Prager (EDP) creep model.

Unlike EDP which requires only one creep test measurement, a cap creep model requires two independent creep test measurements to account for both shear-dominated creep and compaction-dominated creep behaviors. The new TBEO command allows you to define both types of creep data separately.

For more information, see Cap Creep Model in the Theory Reference for the Mechanical APDL and Mechanical Applications.