Rigid body motion often occurs in the beginning of an analysis because the initial contact condition is not well established. For example, you may encounter problems such as small gaps between element meshes on both sides of the contact pair or between the integration points of the contact elements and target elements. The new contact-stabilization damping feature provides a means to avoid these problems.

For standard contact or rough contact, you can use real constants FDMN and FDMT to define contact damping scaling factors along contact normal and tangential directions. KEYOPT(15) of the contact elements offers further controls on the effect of stabilization damping.

The new contact-stabilization technique damps relative motions between the contact and target surfaces for open contact. It provides a certain amount of resistance to reduce the risk of rigid body motion. For more information, see Applying Contact Stabilization Damping in the Contact Technology Guide.

A brake squeal analysis involves sliding contact at frictional sliding interfaces. In a complex eigenvalue extraction analysis using the QR damped (QRDAMP) or damped (DAMP) mode extraction method, the effects of squeal damping contribute to the damping matrix.

Squeal damping is identified in two parts: destabilizing and stabilizing damping. Two new real constants on the contact elements, FDMD and FDMS, allow you to control how squeal damping is applied. You can use these real constants to apply a scaling factor to the internally calculated destabilizing and stabilizing damping or to input the destabilizing and stabilizing squeal damping coefficients directly. KEYOPT(16) of the contact elements allows further control of how FDMD and FDMS are interpreted during the analysis.

For more information, see Forced Frictional Sliding Using Velocity Input in the Contact Technology Guide.

Surface-projection-based contact, previously available for 3-D surface-to-surface contact only, has been extended to the 2-D contact elements CONTA171 and CONTA172.

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, significantly improving the accuracy of contact results and providing smoother stress distributions in underlying elements for the case of dissimilar meshes at the contact interface. The surface-projection-based contact method is implemented by setting KEYOPT(4) = 3 on the contact element.

For more information, see Using the Surface Projection Based Contact Method (KEYOPT(4) = 3) in the Contact Technology Guide.

Surface-projection-based contact (KEYOPT(4) = 3) has been extended to support the multipoint constraint (MPC) approach (KEYOPT(2) = 2) for all surface-to-surface contact elements (CONTA171, CONTA172, CONTA173, and CONTA174).

In general, the new method provides significantly more accurate and smoother stress distributions near the contact interface of dissimilar meshes compared to the other existing contact options (KEYOPT(4) = 1 and 2), especially for higher-order elements involved in contact.

The surface-projection-based method usually increases computational costs; therefore, it is best used for contact regions where the accuracy of local stresses is critical.

For more information, see Modeling Solid-Solid and Shell-Shell Assemblies in the Contact Technology Guide.

The geometry-correction feature, previously available for 3-D surface-to-surface contact only, has been extended to the 2-D contact elements TARGE169, CONTA171, and CONTA172. Applying a geometry correction to circular (or nearly circular) contact surfaces (via the SECTYPE and SECDATA section commands) reduces the discretization error associated with linear contact elements and can greatly improve the accuracy of contact stresses for certain types of curved 2-D contact/target surfaces.

For more information, see Geometry Correction for Contact and Target Surfaces in the Contact Technology Guide.

In most welding processes, after materials around contacting surfaces exceed a critical temperature, the surfaces begin to melt and bond with each other. The new TBND real constant on the contact elements (CONTA171 to CONTA177) allows you to specify this critical temperature in order to model such behavior. When the temperature at the contact surface exceeds the specified melting temperature, the contact changes to “bonded” and remains bonded for the remainder of the analysis.

For more information, see Using TBND in the Contact Technology Guide.

The following additional contact enhancements are available:

Rezoning for 3-D analyses now supports tabular loading. For more information about loads and boundary conditions, see Rezoning Requirements in the Advanced Analysis Techniques Guide.

Nearly all structural materials are now supported. (The exceptions are CAST (cast iron), CONCR (concrete), MPLANE (microplane), SMA (shape memory alloy), and SWELL (swelling)). Material models can be combined, as described in Material Model Combinations in the Material Reference.

The new MAPVAR command defines tensors and vectors in user-defined state variables for rezoning.

A new solid circular cross section for pipes is now available. Using PIPE288 and PIPE289 elements and the solid pipe section, you can easily simulate beam structures with special materials, such as rubber and shape memory alloy, which must be represented with 3-D constitutive models and are not available for standard beam elements.

A new aeroelastic-structural analysis capability allows you to design the structures upon which wind turbines are positioned. In the sequential aeroelastic coupling method, the aeroelastic analysis is performed by the aeroelastic code with the effects of the supporting structure incorporated as a superelement to the solution. The program provides the supporting structure-substructure matrices and loading data that are required as input to the aeroelastic code (via the OUTAERO macro). Following the aeroelastic analysis, the results can be read back in to recover the element forces inside the supporting structure.

For more information, see Coupling to External Aeroelastic Analysis of Wind Turbines in the Advanced Analysis Techniques Guide.

Support has been added for discrete-thickness shells. When specifying shell section thickness as a tabular function (SECFUNCTION), the prior NODE option (still available in this release) uses a 1-D array where the thicknesses are associated to the nodes via array index; this pattern works well but requires large array dimensions when gaps in node numbering exist.

The new NOD2 option allows you to vary shell thicknesses versus node number in the form of a 2-D array, relating thickness to node number directly. The size of the array is proportional (2X) to the number of nodes with thicknesses and is independent of node numbering. This capability is particularly useful for tapered shells, where a single part may have large node IDs, but a relatively small number of nodes relative to the entire model.

You can now define element body force loads for pipe and elbow elements, allowing you to specify radial and axial temperature variations on those elements. You can also specify a table name for beam and pipe elements that allow multiple temperature inputs per node; you need only define the tabular load for the first node (Node I), as loads on the remaining nodes are applied automatically. For more information, see the documentation for the BFE command.

It is now possible to analysis the interaction of a structure supported on one or more piles with an elastic or inelastic soil. You can input data to describe the lateral force-displacement, and the end-bearing and skin-friction responses of the soil layers occurring at the pile location. It is not necessary for all piles in the analysis to be situated in identical geological strata. For more information, see Soil-Pile-Structure Analysis in the Advanced Analysis Techniques Guide, and the documentation for the PILExxxx family of commands.

Material-dependent damping proportional to the mass is now available in full harmonic and transient analyses (Lab = ALPD on the MP command). In these analyses, the damping proportional to the stiffness is now specified via Lab = BETD on the MP command (replacing the obsolete DAMP label). For mode-superposition methods, the material-dependent damping ratio is now input via Lab = DMPR on the MP command (replacing the obsolete DAMP label). For more information, see Damping in the Structural Analysis Guide.

The procedure for a linear non-prestressed modal analysis for a brake squeal system has been simplified and streamlined so that it follows the conventional linear modal procedure in conjunction with the CMROTATE command. The solution accuracy of the QRDAMP eigensolver for brake squeal analysis has been greatly improved. In addition, the new squeal damping feature also works with the linear non-prestressed modal analysis. For more information, see Linear Non-prestressed Modal Analysis in the Structural Analysis Guide.

For multiple load steps applied to mode-superposition harmonic and transient analysis, surface elements (SURF153, SURF154, and SURF156), FOLLW201, and remote-load (RBE3) contact elements can now be specified within multiple load steps.

Eigenvalues and mode shapes from a linear perturbation modal analysis can be used in downstream analyses of mode-superposition harmonic and transient analysis, as well as in power spectral density (PSD) and response-spectrum analyses. The prestressed effects from the linear perturbation modal analyses are retained and passed into the downstream analyses.

In mode-superposition harmonic analyses that use the modal stresses in the expansion pass of the modal analysis (MXPAND,,,,YES,,YES), the nodal and reaction forces now contain the damping and inertial components.

If a thermal load is defined in a modal or harmonic analysis (including the static part of a prestressed harmonic analysis), you can now use the new THEXPAND command to ignore its contribution to the modal and harmonic loads.

You can now import variable bearing characteristics used for bearing element COMBI214 real constants into table parameters from an ASCII file via the importbearing1 macro. The file format is described in Bearing Characteristics File Format in the Rotordynamic Analysis Guide.

The critspeedmap macro is now available to generate the critical speed map of a rotor. For a usage example, see Example: Critical Speed Map Generation in the Rotordynamic Analysis Guide.

The bearing element COMBI214 now supports stiffness and damping characteristics dependent upon the eccentricity. The table parameters definition is given in Using the COMBI214 Element in the Rotordynamic Analysis Guide.

The damping proportional to the mass (ALPHAD) is now supported in spectrum and power spectral density (PSD) analyses.

Enhancements to the RESP command allow you to generate the response spectrum from an acceleration input, and to determine the pseudo-velocity and pseudo-acceleration response spectrum.

In PSD and multi-point response spectrum (MPRS) analyses, the maximum number of input tables is now 200, while the maximum number of participation factor calculations (PFACT command) is 300.

An option is now available on the mode-combination commands (CQC, DSUM, GRP, NRLSUM, PSDCOM, ROSE, SRSS) to combine the summed modal static and inertial forces. The default (and prior release behavior) is to combine the modal static forces (that is, only the stiffness multiplied by mode shape forces, both of which are the stress-causing forces). An option is now available to combine the summed modal static forces and inertia forces (both stiffness and mass forces, which are the forces acting on the supports).

Load case combinations (LCOPER) now add the element nodal forces in the FORCE,TOTAL case before the combination yielding correct total (static, plus damping, plus inertial) forces. Also, SET,,,,,AMPL and SET,,,,PHASE yield the correct force amplitudes and phase angles when FORCE,TOTAL is set.

The modal assurance criterion values obtained via the RSTMAC command can be retrieved as APDL parameters for further processing. See the *GET command.

This release includes a new approach to crack growth simulation. The method is based on the virtual crack closure technique (VCCT) with interface elements to model the crack growth. The method is very suitable for interfacial delamination of laminate composites, and is also applicable to crack growth simulation in homogeneous material. A number of fracture criteria are available, including critical energy-release rate, linear, bilinear, B-K, modified B-K (Reeder), power law, and user-defined. A material data table can be used to define the fracture criterion and associated material properties.

Support for the new crack growth simulation technology is available via the PLANE182 and SOLID185 elements. The new CGROW command defines all necessary parameters for the crack growth simulation.

For more information, see VCCT-Based Crack Growth Simulation in the Structural Analysis Guide.

Material curve fitting allows you to derive coefficients from experimental data that you provide for your material. Curve fitting involves comparing your experimental data to certain preexisting nonlinear material models to determine the best material model to use during solution.

A new material curve-fitting option determines your material constants by relating your experimental data to the Chaboche nonlinear kinematic hardening model. Curve fitting is performed either interactively or via batch commands. You can fit uniaxial plastic strain vs. stress data, along with discrete temperature dependencies for multiple data sets.

For more information, see Chaboche Material Curve Fitting in the Material Reference.

The shape memory alloy (SMA) can undergo large deformation without showing residual strains (pseudoelasticity effect, also often called superelasticity), and can then recover its original shape through thermal cycles (the shape memory effect). As such, the SMA material models (TB,SMA) can now be used to model both the superelastic behavior and the shape memory effect behavior of shape memory alloys.

For more information, see Shape Memory Alloy (SMA) Material Model in the Material Reference.

The new microplane material (TB,MPLANE) models material behavior through uniaxial stress-strain laws on various planes. Directional-dependent stiffness degradation is modeled through uniaxial damage laws on individual potential failure planes, leading to a macroscopic anisotropic damage formulation.

The model is well suited for simulating engineering materials consisting of various aggregate compositions with differing properties (for example, concrete modeling, in which rock and sand are embedded in a weak matrix of cements).

For more information, see Microplane Material Model in the Material Reference.

The initial state capability allows you to define a nontrivial state from which to start an analysis. The initial state capability has been enhanced to include initial creep strain, user-defined state variables, and a node-based option.

Initial state application has always been element-based, but a new node-based option is available for current-technology elements. For layered elements, you can apply an initial state to each layer at every node within the element. For beam elements, you can apply an initial state to each cell number at every node within the element. For all other elements, the initial state is applied at each node within the element.

For more information, see Initial State in the Basic Analysis Guide and the documentation for the INISTATE command.

You can now model the response of materials with viscoelasticity and anisotropic hyperelasticity behavior (combining TB,PRONY and TB,AHYPER).

The viscoelasticity is assumed to be isotropic (that is, independent from the loading direction), and is defined via the Prony series (TB,PRONY) and shift function (TB,SHIFT) to model the strain rate effect. The new capability supports most current-technology elements (the exceptions being beam and link elements).

For more information, see Material Model Combinations in the Material Reference, AHYPER and PRONY (Anisotropic Hyperelasticity and Viscoelasticity (Implicit)) Example in the Structural Analysis Guide, and Large Strain Visco-Anisotropic Hyperelasticity in the Mechanical APDL Theory Reference.

A new viscoelastic constitutive model for the harmonic domain (using the generalized Maxwell model) is now available for modeling the steady-state response of viscoelastic materials in small-deformation models. For more information, see Harmonic Viscoelasticity in the Material Reference and Viscoelasticity in the Structural Analysis Guide.

Coupled pore fluid diffusion and structural analysis now supports hyperelastic materials, allowing for an initial, efficient analysis of porous materials with hyperelasticity models. In this case, the program assumes that all Biot and permeability parameters remain constant during deformation.

The coupled pore-pressure thermal elements used in analyses involving porous media are listed in Coupled Pore-Pressure Element Support in the Coupled-Field Analysis Guide. For more information, see Porous Media Flow in the Mechanical APDL Theory Reference.

In addition to the existing exponential option, a new bilinear option (TB,CZM,,,,BILI) is available for modeling interface delamination using interface elements (INTER202 through INTER205) with a cohesive zone material (CZM) model. The new CZM model option uses bilinear traction-separation laws.

Unlike an exponential model, a bilinear model gives correct results for linearly debonding material interfaces, and makes it possible to simulate Mode I or Mode II dominated (or mixed-mode) debonding.

For more information, see Interface Delamination and Failure Simulation in the Structural Analysis Guide, Cohesive Zone Material in the Material Reference, and Cohesive Zone Material (CZM) Model in the Mechanical APDL Theory Reference.

Swelling is a material enlargement (volume expansion) caused by neutron bombardment or other effects (such as moisture). The swelling strain rate is generally nonlinear and is a function of factors such as temperature, time, neutron flux level, stress, and moisture content. Several options are now available for modeling swelling effects (TB,SWELL), and element support has been greatly expanded. For more information, see Swelling Model in the Material Reference.

For the anisotropic hyperelasticity material model (TB,AHYPER), a new exponential-based strain energy potential function is available for characterizing the isochoric part of strain energy potential. For more information, see Anisotropic Hyperelastic Material in the Material Reference and Anisotropic Hyperelasticity in the Mechanical APDL Theory Reference.

The damage initiation and propagation in fiber-reinforced composites can now be simulated with a nonlinear solution process. Different than the postprocessing failure analysis, the new capability allows you to estimate ultimate composite strength under complex stress states.

The material damage initiation and evolution laws are specified via two new material models (TB, DMGI and TB,DMGE, respectively). Currently, only failure-criteria-based initiation laws and instant-stiffness-reduction evolution laws are supported (TB, FCLI).

The new damage models are compatible with linear elastic orthotropic materials, which are commonly used for representing the homogenized properties of fiber-reinforced composites.

For more information, see Damage Initiation Criteria and Damage Evolution Law in the Material Reference.