A new frictional contact model is now available using TB, FRIC, TBOPT=ATAN. This option models frictional stress as a continuous function of sliding velocity using an arctangent relation. Because the frictional stress is continuously differentiable with this option, it should help in non-linear problems that are having difficulty converging.

In prior releases, the double-sided target surface option (KEYOPT(8) = 1 of the TARGE170 element) was valid only for the 3D surface-to-surface contact element CONTA174. In release 2025 R2, the double-sided target surface option is now valid for the 3D node-to-surface contact element CONTA175.

Contact detection for the double-sided target surfaces is also refined to prevent missing constraint equations or bad crossing constraint equations for the MPC contact definition. This greatly improves contact solution accuracy and robustness.

For more information, see Double-Sided Target Surfaces in the Contact Technology Guide.

Selecting a constraint type for assemblies is problem-dependent and can have a significant impact on solution accuracy. In release 2025 R2, the mixed constraint type option (KEYOPT(5) = 2 of target element) has been extended to the 3D node-to surface contact element CONTAC175 and the 3D line-to-surface contact element CONTA177 (in addition to the previously-supported 3D surface-to-surface contact element CONTA177). This change enables larger percentages of assembly models to be solved with improved robustness and accuracy, particularly for mixed constraint types (solid-to-solid, shell-solid, shell-to-shell) defined within a contact pair.

For more information, see the discussion of input data for TARGE170.

Performance improvements for multipoint constraint (MPC) bonded contacts (CONTA element KEYOP(2)=2, KEYOP(12)=5,6) include the following:

In most applications (especially larger assemblies), generating contact pairs and surface-based multi-point constraints (MPC) requires many lines of MAPDL script and multiple, repeated EBLOCK commands. This increases the size of input files and reduces their efficiency and readability.

To address this problem, release 2025 R2 includes two new commands:

By using these commands, you can create a contact pair or MPC surface based constraint with one MAPDL command and more efficiently define them in bigger assemblies. This also reduces the size of input files by eliminating the need to use multiple EBLOCK commands.

You can now optionally create a new component from the rigid target elements generated by the RBGEN command. Use the ECOMP option to specify the name of a new component that includes the newly-generated elements. This makes it easier to list, plot, and debug rigid target elements.

You can now optionally specify an acronym name instead of a serial number when you are using the RMODIF command to modify a real constant item for contact elements.

A new joint element is available. MPC184-Genc is a two-node joint element in which the relative rotations are characterized by a rotation axis. It is used to connect two bodies to transmit motion from one body to another. Stiffness and damping behavior can be specified for this joint.

You can now activate joint damping behavior in a static analysis by setting KEYOPT(6) = 1 for the relevant joint element. The relative velocities are computed based on incremental displacements and the time increment in the given substep. For more information, see Stiffness and Damping Behavior of Joint Elements in the Multibody Analysis Guide and the individual joint element descriptions.

To consider only the initial slope of a nonlinear stiffness or damping curve in a linear analysis, you can now use the option, KEYOPT(8) = 1, for the relevant joint element. See the individual joint element descriptions for more details.

The SHELL181/SHELL281 structural shell elements are now supported in the direct-embedding workflow. For more information, see Direct-Embedding Workflow.

The general axisymmetric solid elements, SOLID272 and SOLID273, now support the MODE command (using KEYOPT(2) = 1) and all nodal results can be saved to the .rst file (using KEYOPT(3) = 1). SOLID272 with KEYOPT(1) = 1 now supports the enhanced strain formulation.

SOLID186 and SOLID187 are now enabled to activate nonlocal damage models such as generalized damage (implicit gradient regularization). Nonlocal damage formulation capabilities can better capture the distributed nature of damage in real materials by averaging variables over a finite neighborhood and introducing a characteristic length scale. This leads to more objective and reliable results, improved convergence stability and mesh insensitivity in the presence of strain localization or softening.

In the NLAD framework, the Generalized Remeshing for Adaptive Nonlinear Damage (GRAND) capability enables material removal by generating voids in an implicit analysis. The nonlinear adaptive criterion REMMAT is now used to initiate voids when high strains are reached during the solution process. See Material-Removal-Based Criterion.

The REMESH REASON list in the remesh monitor file .rmsh now includes more remesh reasons and their combinations. Each remesh reason has one identifier number and when there is more than one reason, each identifier is listed in a row.

You can now adjust automatic time incrementation to strictly adhere to the time increment specified by the DELTIM command. By default, automatic time incrementation adjusts the initial time increment to generate a whole number as the total number of substeps. To bypass this default, specify ForceKey as an option for the DELTIM command, The program then adheres to the initial time increment that you specified.

You can now apply a generalized gradient damage model to simulate a brittle failure problem (TB,CDM,,,,MXPS). A maximum principal stress driven damage model is used to effectively capture a brittle rupture. It does not usually converge when simulating an unstable damage growth problem. Therefore, an appropriate small viscous effect can be considered to enhance the stability of the brittle damage simulation using the command TB,CDM,,,,VREG. For details and an example, see Regularized Generalized Damage.

The AML Python Module is the Python extension for Ansys Materials Lab (AML). It allows you to access Ansys structural materials to evaluate material tangent and stress for supported material models and perform parameter fitting for supported material models.

A new method, auto_initialize, is now available to perform AI-based initialization needed for the fitting process. The AML Python Module now supports several Extended Drucker-Prager and Geomechechanics material models.

For more information, see Using AML Python Module.

Automatic coefficient initialization now supports the visco-hyperelasticity model by using a combination of hyperelasticity and Prony series. Temperature-dependent visco-hyperelasticity is supported for the combination of hyperelasticity, Prony series, and the shift function.

For more information, see Visco-Hyperelasticity.

Hyperelasticity is now supported with small-deflection formulation. Static, transient, modal, and harmonic analyses are all supported by small-deflection hyperelasticity. Small-deflection analysis uses the hyperelastic tangent modulus at zero deformation as an approximation to the more general finite strain hyperelasticity when the deflection is small.

Threshold stress-intensity factor range (ΔKth) specified for a SMART fatigue crack-growth analysis is stored as a result at all the susbteps. It can be retrieved using PRCINT, *GET or PLCINT commands. The availability of the threshold range as a result is particularly useful for verification, when it is specified using a table or defined using a functional relation as in the NASGRO equations.

SMART crack-growth can be analyzed with cyclic symmetry boundary conditions in a single stage model. A crack can be initiated in the stage during solution, or a pre-existing crack can be used for the analysis. The cyclic symmetry constraint equations are established (using the CECYCMS command) for the matching node pairs on the low and high sector boundaries. If the crack growth remeshing affects the cyclic symmetry boundaries, the program automatically maintains a matching mesh on these boundaries and updates the constraint equations for the new mesh.

The Ramberg-Osgood model and kinematic hardening elastic-plastic material models are now supported in the calculation of J-integral for explicit cracks.

A new procedure for the Campbell analysis of a prestressed structure using linear perturbation is now supported (Alternative procedure for rotational velocity independent prestress in the Rotordynamic Analysis Guide). It is recommended if the prestress is independent from the rotational velocity.

Spring-damper (COMBIN14) and bushing (COMBI250) elements with tabular real constants (frequency is the primary variable) are now fully supported in a linear perturbation harmonic analysis.

Bearing element (COMBI214) with tabular real constants (rotational velocity is the primary variable) is now fully supported in a linear perturbation modal and a linear perturbation synchronous harmonic analysis (SYNCHRO command).

Static multiframe restarts are now supported for Cyclic Symmetry and Multistage Cyclic Symmetry Analyses. This feature enables you to save information for multiple loadsteps and substeps and restart from a specific loadstep and substep, making analysis corrections as needed.

To reduce the .mode file size and improve efficiency in a mode-superposition analysis where displacement solution is of primary interest, writing to the .mode file can be scoped based on a subset of nodes (see Node-based Mode File Scoping for Mode-Superposition Analysis in the Structural Analysis Guide).

Selecting the proper harmonic indices participating in the response is of paramount importance to efficiently solve a multistage cyclic symmetry analysis. A Python script has been developed to facilitate the selection process. Use it to calculate relevant harmonic indices to include for an accurate response in a specified nodal diameter range in a multiharmonic multistage cyclic symmetry analysis. For details, see Python Script for Selection of Multistage Harmonic Indices in the Multistage Cyclic Symmetry Analysis Guide.

An automatic inertia relief option is available to calculate the residual vectors in a modal analysis, which improves the accuracy for mode superposition analysis (transient and harmonic). For more information, see Including Inertia Relief Calculations in the Basic Analysis Guide.

There is now a convenient way to terminate an HBM analysis and write the last converged substep to the results (.rst) file. You can then restart the analysis with a new input file, using the last converged result as a solution guess for the next frequency/substep. For more details, see Aborting an HBM analysis in the Harmonic Balance Method Analysis Guide.

Large Mass Method (LMM) enforced motion analysis is now implemented natively. This makes performing LMM analyses easier.

To perform a LMM analysis, first define a large mass by using the MASS21 element. Then, use the FVAL command to specify displacement, velocity, or acceleration as input. For more information, see the discussion of this command under New Commands.

You can now use adaptive mass proportional damping to solve complex, non-linear problems. Specify the AUTO field in the ALPHAD command. Automatically adjusting the mass matrix multiplier for damping improves convergence in non-linear problems that use the quasi-static method (TINTP,QUASI) or the static-to-transient method (SOLOPTION,STOT).

The following types of problems are expected to benefit from adaptive mass proportional damping:

To ensure an accurate solution, the damping is set high enough to provide some stability but low enough that damping energy is a small fraction of the potential energy of the system.