ANSYS, Inc. Release Notes
ANSYS, Inc. Release Notes
This release of the Mechanical application contains all of the capabilities from previous releases plus many new features and enhancements. Areas where you will find changes and new capabilities include the following:
Release 14.0 includes several new features and enhancements that result in product behaviors that differ from previous releases. These behavior changes are presented below.
By default, a model's node and element numbering will not be condensing when actions such as body suppression occurs. Thus gaps in numbering can occur in the solver input file. This change was done in order to preserve the integrity of nodal based named selections. The ability to compress the numbers can be achieved by a setting in the Details view of the Mesh Numbering folder.
The default values used for contact Formulation, Update Stiffness, and Behavior have changed. The new defaults were chosen to give best solution to a wide range of contact situations. See Connection Enhancements below for further information.
The Auto Detection Value for a contact pinball region is only available for contacts that are generated automatically.
The Bending option for the Shell Entry will not be available in the Stress/Strains details view, however you can calculate this result using User defined results. For a more meaningful result, see the new Bending and Membrane Stress Results.
An Imported Body Temperature object in a 3D analysis no longer supports scoping surface bodies with other geometry types. You will now be required to create a separate Imported Body Temperature object for surface bodies. This change was made to support applying temperatures to the Top, Bottom, or Both face selections of surface bodies.
When using an Imported Body Temperature or an Imported Heat Generation object to transfer and apply loads from an upstream Mechanical analysis, the following changes have been made to the Data View worksheet to allow for more efficient data transfers:
The addition or removal of rows in the worksheet is no longer controlled by the program. You can add rows in the worksheet to specify additional data for a different analysis time.
When resuming legacy databases, rows in the worksheet will be removed if the Source Time value of the row matches that of the previous row. This has been done to prevent importing redundant data.
The Active column will no longer be available for activating or deactivating the load at different steps. Activation or deactivation of these loads can now be done from the Graph or Tabular Data window of the object. Legacy databases will be migrated to handle this change.
The Auto Detect Contact On Attach option, which used to be available in the Options dialog box within the Mechanical application, has been moved. See Miscellaneous Changes and Behaviors in the Meshing Application Release Notes for details.
In an effort to reduce disk space usage, by default, Nodal Forces are not written to the result file. However, this output is required to perform post-processing tasks on the results for most contact force reactions. This default setting can be changed under the Output Controls category of the Mechanical Application Options dialog box (Tools>Options).
By default, changes to solution level command objects will not invalidate an up-to-date solution.
Following the import of a Load History, the Magnitude field displays the label "Tabular Data". If this Load History data is duplicated, the newly created data is independent of the original load.
The Import Load History feature has undergone a behavior change. In prior releases, the name of the imported Load History was displayed in the Details view Magnitude field, reflecting an object in memory. If this load was duplicated, the new duplicate showed the same name because it was the same object in memory. Any change to either object’s tabular data changed the underlying objects data and therefore each Load History was changed – they used the same data. Now, this field displays the label/name “Tabular Data” and duplications are unique and independent of one another.
Harmonic Analysis: thermally induced harmonic loading is now ignored by all Harmonic Analysis.
Random Vibration Analysis and Response Spectrum Analysis: In prior releases, an effective material damping ratio can be defined via Damping Factor (β) in Engineering Data. In release 14.0, the Damping Factor (β) has changed to provide a material-dependent stiffness coefficient based damping, which is not supported, and is ignored in solution. As a result, differences in the solution are therefore observed between the prior releases and the release 14.0 when the analysis is cleared and re-solved. Currently, there is no equivalent damping behavior supported in the release 14.0. To have an equivalent damping behavior in a Modal Analysis using release 14.0, issue the Command Snippet mp,dmpr.
The following general enhancements have been made at release 14.0:
Support for Cyclic Symmetry on Surface Bodies. Analyses that include cyclic symmetry can now be performed on surface bodies as well as solid bodies.
Expanded Criterion Based Named Selections. More options have been to added for creating named selections by criteria (Worksheet Scoping). Additional options include:
Criterion based on radius
Ability to build up selections from other Named Selections.
Tolerance used for numerical evaluation.
Whether a row is included as a part of the criterion.
Implementation of Materials as Criterion.
Implementation of Smallest and Largest as available Operators.
Mesh Based Named Selections. Mesh based Named Selections are available as an alternative to geometric based selections and include the following features:
Scope Named Selections based upon things such as interactive picking, node Ids, location, midside nodes, and corner nodes.
Convert geometric Named Selection to mesh based Named Selection using the Convert To option.
Apply the mesh based Named Selections to certain boundary conditions and results.
View properties of the selection in the Selection Information Window or Export to a file.
Release 14.0 has given special attention to the performance of Mechanical in various areas in order to provide a better responding product for both small and large models:
Improved application start time. Mechanical is now preloaded when a Mechanical system is detected in the schematic. This can result in a significant reduction of fixed cost overhead when opening Mechanical through the "Edit" command. For example, an "Edit" of a simple model can be as more than 10 times faster.
Better system performance when postprocessing large result files. Prior to release 14.0, if the result file was much larger than the amount of physical memory on the computer, severe performance degradation could happen when evaluating results, especially when multiple result sets were present. Mechanical has changed how it reads result files from disk which has addressed this degradation.
Creation of objects that scope to a large number of entities (on the order of thousands) has been improved. Additionally the database resume time for an "Edit" operation with large numbers of entities in the tree or scoping has been improved.
Improvements for Imported Loads.
Faster graphics response. The time to display contours for an Imported Load has been improved. Speedups of a factor of 2-3 can be seen on larger models.
Faster save/resume times. The time required to save and resume Imported Loads has been made significantly faster. For example, an Imported Load that took 20 seconds to save and 10 seconds to resume in release 13.0 now saves in 3 seconds and resumes in less than 1 second. For larger models, speedups of a factor of 8-10 are now achievable for save and a factor of 15 and greater for resume.
Improved memory usage for save/resume. Memory usage when Imported Loads are saved or resumed has been greatly reduced. Improvements of a factor of 15 or more can been seen.
Improved Automatic Contact Detection. Automatic contact detection speeds have increased. For models where a large number of contacts are created, improvements of a factor of two or more can be seen.
Faster weight-calculation time for Triangulation and Distance Based Average mapping. Triangulation and Distance Based Average weighting calculation times have improved by utilizing multiple cores. For larger meshes utilizing 8 cores, a 3 to 4 times speedup can be seen.
The following analysis enhancements have been made at release 14.0:
Damped Modal Analysis Results. Results for damped modal analyses are now available directly in Mechanical, including, for a damped analysis, the option to allow or ignore the time decay animation for complex modes.
Transient Response Analysis Using Linked Modal Analysis System. A transient structural analysis using the Mode Superposition method can now be accomplished by linking a Transient Structural analysis system to an existing Modal analysis system on the Project Schematic. This new solution methodology can result in much faster solution times for a linear transient structural analysis.
Rotordynamics. A type of modal analysis to analyze dynamic characteristics of rotating systems with the effects of damping, Coriolis, and different rotational velocities. The analysis helps you produce Campbell plots to identify critical speeds. It is supported for all body types; solid, shell and line bodies, but limited to single spool systems.
MSUP Harmonic Analysis. You can now perform the Mode Superposition harmonic analysis linked to a pre-stressed modal analysis.
Double precision is now the default for Explicit Dynamics analyses.
Composites. Mechanical now has support for modeling layered shells (composites) for both Mechanical APDL and Explicit solvers. Features include:
Engineering Data Support for orthotropic strength material properties
A Layered Section Object to define and setup simple layered shells
Support for Imported Layered Sections from external sources such as ANSYS Composite PrepPost (ACP)
Post processing on a per layer basis
The following features are now supported for Explicit Dynamics 2D Plane Strain Analyses:
Coordinate Systems
Initial Condition - Velocity and Angular Velocity
Inertial Loads - Acceleration and Gravity
Supports (Constraints) - Fixed Support, Displacement, Velocity
Loads- Pressure, Force, Hydrostatic Pressure
Connections - Frictional/Frictionless for Manual Contacts and Body Interactions
Geometry
Symmetry
Results/Probes
Analysis Settings
Axisymmetric Analysis
The following geometry enhancements have been made at release 14.0:
Compare Parts on Update. Can now be set to Associative or Non-Associative.
Searching Faces With Multiple Thicknesses. Faces with multiple thicknesses can now be easily identified.
Line Body Definition Extended to Pipes. Line bodies can now optionally modeled as pipes or beams. Modeling as pipes allows for specialized pipe loading as well as options to account for cross section distortion.
External Thickness Import. This feature enables you to import and map X, Y, Z thickness data for a 3D surface body or a 2D plane stress body.
The following contact and connection enhancements have been made at release 14.0:
Expanded Contact to Line Bodies. Edges and vertices of line bodies can now be scoped to the contact side of a Contact Region.
Expanded Support for Normal Lagrange Formulation. The Normal Lagrange contact formulation is now available for all contact regions regardless of scoping type or underlying geometry.
Stabilization Damping Factor. The Damping Stabilization Factor is now available to damp relative motion and provides a certain amount of resistance to reduce the risk of rigid body motion because of open contacts.
Program Controlled Defaults Added To Behavior Contact Property. The Behavior contact property now includes a Program Controlled default setting that automatically adjusts depending on the presence of rigid body faces (3-D) or edges (2-D).
Program Controlled Defaults Added To Formulation and Update Stiffness Contact Properties. Formulation and Update Stiffness properties now each include Program Controlled default settings that automatically adjust depending on the presence of rigid body contacts.
Contact Detection. Nodal detection is now supported for 3D face-face contacts and 2D edge-edge contacts.
Joint Availability. Joints are now available for use in harmonic, random vibration, and response spectrum analyses.
Mesh Connections Common to Selected bodies. This new option highlights the mesh connections that are common to the bodies selected in the Graphics viewer.
Mesh Connection Across Parts. The Mesh Connection feature leverages the Post Pinch technology to automatically generate Post Pinch controls internally at meshing time. This technology allows Mesh Connections to work across parts so that a multi-body part is no longer required.
The following graphical enhancements have been made at release 14.0:
Selection Information Window. A new window can now be displayed that provides an efficient way to obtain geometric information on selected items in the model.
Viewing Line Body Cross Sections as 3-D Geometry. A feature has been added to the View menu that displays a line body with defined cross sections in 3-D geometry.
Show Mesh. Displays the model’s mesh regardless of the selected tree object.
Graphical Based Node Selection. Nodes can now be selected in the graphics view. Additionally, there are several selection modes available to choose the desired nodes.
Show Coordinate Systems. Displays all of the Coordinate Systems that are associated with the model.
Viewing and Exporting Finite Element Connections. The new FE Connections Visibility option, Draw Connections Attached To All, allows you to display All Nodes associated with Solution Information or to view nodes scoped to a Named Selection. Connections can also be viewed as Lines or as Points.
Display Edge Direction. You can now display model edge directions.
Create Section Plane. You can now create a section plane on your model that is based on a predefined Coordinate System.
The following loads/supports/conditions enhancements have been made at release 14.0:
Pipe Pressure for Line Bodies. Pressure can now be applied to line bodies defined as pipes. The Pipe Pressure load can be applied as a constant, tabular, or function load.
Pipe Temperature for Line Bodies. Temperature can now be applied to line bodies defined as pipes. The Pipe Temperature load can be applied as a constant, tabular, or function load.
Direct FE is a new Menu of options in the Mechanical Application that contains specific Finite Element (FE) boundary conditions in the form of forces, supports, and conditions, and includes:
Nodal Orientation. A nodal coordinate system can be created for later use in applying nodal rotations to displacements. This is represented by a Orientation object and is available in the Direct FE menu.
Nodal Force - A force can now be applied to individual nodes or a group of nodes by scoping Nodal Force to a node-based Named Selection.
Nodal Pressure - A pressure can now be applied to individual nodes or a group of nodes by scoping Nodal Pressure to a node-based Named Selection.
FE Displacement - A node-based displacement can now be applied.
FE Rotation - A fixed rotation can now be applied to the nodes of a body.
Lock at Load Step. A joint can now be locked at a specific load step during a multi-step analysis. This feature is available for both a static or a transient analysis.
PSD Loading to Multiple Remote Displacements (and Fixed Supports). For a Modal Analysis, you can now apply a PSD Excitation load to all remote displacements or to all remote displacements and all fixed supports.
Ansoft-Mechanical Data Transfer. Imported Loads from HFSS, Maxwell, or Q3D now support the ability to import data from multiple times/frequencies and apply them at different times using a single Imported Load object.
Mechanical-Maxwell Stress Feedback. Deformation results can now be exported from a structural analysis in Mechanical and used in a Maxwell analysis.
Activation/Deactivation Support for Imported Loads. Imported loads can now be activated or deactivated on a step basis from the Graph or Tabular Data window of the object.
Heat Flux and Heat Generation Import from External Files. Heat Flux and Heat Generation data, specified in the External Data system, can now be imported and applied in a steady-state or transient thermal analysis.
Imported Body Temperature Loads Enhanced for Surface body Selections. Temperatures imported into a structural analysis can now be applied to the Top, Bottom, or Both face selections of surface bodies.
Convection. A convection load (film coefficient and ambient temperature) can be applied as a tabular load or a function of x or y or z and/or time.
The following mapping enhancements have been made at Release 14.0:
Scan For File Changes, a context menu option on an External Data System's Setup cell, checks each Data Source file and validates that inputs are correct.
Named Selection Creation. Automatic named selection creation for unmapped, mapped, and outside nodes.
Mapping Settings. Imported loads settings have been changed:
Triangulation. Weighting setting Radial Basis Functions has been changed to Triangulation to better describe the technique used in calculating source point load contributions.
Distance Based Average. A new weighting option Distance Based Average has replaced Closest Point allowing input from the user to specify how many closest points to use when calculating source point contributions.
Databases from previous releases with Closest Point weighting will be migrated to Distance Based Average with the Advanced setting Number of Points set to 1.
Better control of outside nodes during weight calculation. Nodes found outside the boundaries of the surface/volume elements created during mapping can now be handled using Distance Based Average or Projection techniques.
Kriging Weighting Type. Kriging is a regression-based interpolation technique that assigns weights to surrounding source points according to their spatial covariance values and can provide for smoother mapping compared to other weighting techniques.
Validation. A new Validation object has been added to help in determining the quality of the mapping.
Multiple File Inputs. Importing loads from upstream External Data system containing multiple data files. See External Data in the Workbench User Guide and External Data Import in the ANSYS Mechanical Application User's Guide for details.
New Source Geometry Analytical Transformation Capabilities. Analytical Transformation of source point locations using scale factors or functions. This feature can be useful to help account for differences between the source and target geometry.
Export. Imported data (loads and thicknesses) can be exported to a file.
Shell Thickness Factor. When mapping data from an External Data system onto surface bodies, a new Shell Thickness Factor property allows you to account for the thickness at each target node, and consequently modify the location used for each target node during the mapping process.
The following solution enhancements have been made at release 14.0:
Save Project Before and After Solution. As a safeguard in protecting a Workbench database, a project can now be saved before a solve is requested as well as after it is solved, before postprocessing.
Loads values can be modified. Load values for most boundary conditions can now be modified.
Nodal forces and pressures can be added. Nodal Force and Nodal Pressure objects can be created without loss of restart points.
Improved License Management for RSM Jobs There is a new Workbench preference, Release License for Pending Jobs, which enables you to control when the Mechanical application holds its license during batch mode operations while the Solution cell is in the pending state. Releasing the license may lengthen the time required to perform the batch run. See Mechanical for details.
Expanded Output Controls: The output controls have been expanded and now support controls such as nodal forces, miscellaneous records, and the maximum number of results sets to write.
Distributed Solver For Pre-Stress Modal Analysis. Pre-stress modal analysis can now be performed via the Distributed solver option (DANSYS) when using the MAPDL solver.
License Queuing. You may now instruct the MAPDL solver to wait for an available license by using a configuring settings when solving remotely via RSM.
Post Processing Commands. You can now add or modify solution level command objects for a solved analysis without invalidating your existing solution.
The following results enhancements have been made at release 14.0:
Display Finite Element Beams, Weak Springs and Constraint Equations. The Solution Information object now includes properties to control the ability to display internal beams, weak springs and constraint equations that are generated during solution.
Results Scoping Extended to Meshing Entities. Using criteria based named selections, scoping for several results is now available on underlying meshing entities, in addition to geometric entities.
Forces/Moment Reactions . Force Reaction probes and Moment Reaction probes are now available for use in Harmonic and Modal analyses. In Random Vibration and Response Spectrum analyses, they can only be scoped to Remote Displacement boundary condition.
Bending and Membrane Stresses. Two new result objects, Bending Stress and Membrane stress, are added to calculate membrane and bending stresses and strains. These results are available only when you solve using the Mechanical APDL solver for surface bodies and solid bodies that are meshed using the thin-solid option.
Force Reaction Probe Support for Cylindrical Coordinates. Force Reaction probes can now be displayed in either cylindrical or Cartesian coordinate systems.
PSD Probes Scoping Extended to Remote Points. Scoping for Response PSD probes is now available at remote points.
Duplication for User Defined Results. User defined results can now be duplicated, with and without the result, and across analysis systems.
Force Reaction Result Trackers. Force Reaction result trackers that can be scoped to boundary conditions and geometry are available for explicit dynamics analyses. Geometry scoped Force Reaction trackers can show results for the following force components:
Support - specifies that the tracker show results for the forces that will be generated due to supports that are present in the model.
Euler/Lagrange Coupling - specifies that the tracker show results for the forces exerted by any material in bodies assigned with an Eulerian reference frame that interact with the scoped region.
Contact - specifies that the tracker show results for the total force resulting from the contact forces acting on the scoped area.
All - specifies that the tracker show results for the sum of all three components.
Design Assessment. The following enhancements have been made to the Design Assessment system:
The Design Assessment system can now accept upstream connections from the following systems: Static Structural, Modal, Harmonic Response, Random Vibration, Response Spectrum, Explicit Dynamics and Transient Structural. Solution Combination can be performed with Static Structural, Modal, Harmonic Response, Random Vibration, Response Spectrum and Transient Structural systems.
Additional BEAMST results are available in the DA Result object when the BEAMCHECK assessment type is specified.
FATJACK (within Design Assessment) enhanced for additional analysis types: Stress History, Spectral, Deterministic.
Units support for attribute input.
Script locations can be defined relative to various locations.
User defined results are now available.
Upstream results are programmatically accessible, enabling direct access through the API to custom results.
Solve and Evaluate script output is now displayed within Design Assessment.
Design Assessment results are now available at nodes, and nodes on elements. Results can also be assigned units and can be presented in vector or tensor forms. The units systems of upstream results can be obtained and mesh data is now provided in the Design Assessment analysis units rather than geometry units.
Design Assessment can now access shell thickness information, including varying thickness definitions.
Design Assessment is now available for Linux platforms.
Result Suppression. Result objects including result Probes can now be suppressed. These suppressed result objects are excluded from the solution.
Create Contour Result From Result. You can now create a contour result from a Frequency Response result type in a Harmonic Analysis. This feature creates a new result object in the tree with the same type, orientation, frequency, and phase angle as the frequency result type.
Expanded User Defined Result Types. Element attribute numbers such as material or type used for the Mechanical APDL solution can now be accessed using User Defined Result Types.
Generate Path from Edge Result. You can now generate a Path form results scoped to contiguous edges.
Enhanced Chart. The Chart object has been enhanced to provide scaling (such as semi-log) and plot options. Additionally, the charts can now plot harmonic Frequency Response objects in order to easily compare and collate result data.
The following usage enhancements have been made in release 14.0:
For Windows users, the solution file folder can be displayed using the Open Solver Files Directory feature.
Convenience MAPDL Parameter: The Mechanical input file to the MAPDL solver now contains a parameter that points to the user_files directory in the Workbench project structure. This can be used by those familiar with MAPDL commands to perform useful file operations.
There are two distinct techniques for calculating Equivalent Strain.
The calculation for Technique One proceeds as follows:
Average the component (X, Y, Z, XY, YZ, XZ) strain values from the elements at a common node;
Calculate the equivalent strain from the averaged component strains.
The calculation for Technique Two proceeds as follows:
Calculate the equivalent strain values (from the six component strains) on a per element basis;
Average these values from the elements at a common node.
The two techniques produce similar (but not necessarily identical) contours.
New at 14.0, when Mechanical post-processes MAPDL and AUTODYN result files, the equivalent strain formulations are the same as those in MAPDL POST1. That is, Mechanical will use Technique Two at 14.0.
Before 14.0, Mechanical used Technique One, except for Equivalent Total Strain results(Solution->Strain->Equivalent Total). Equivalent Total Strain results were always derived via Technique Two.
Effect Upon the Solution Worksheet (User Defined Result Expressions):
The user defined results EPELEQV, EPPLEQV, EPCREQV, EPTTEQV, and EPTOEQV, which represent the pre-14.0 formulation, are no longer listed in the Worksheet at 14.0.
The Worksheet (for structural analyses) will list (if they exist) EPELEQV_RST, EPPLEQV_RST, EPCREQV_RST, EPTTEQV_RST, and EPTOEQV_RST, which represent Technique Two.
Exceptions
Technique Two has NOT been installed into the post-processing of result files for other solvers (e.g. SAMCEF and SNECMA).
For cyclic symmetric models in modal environments, the older (pre-14.0) formulation is still in effect.
If the MAPDL/AUTODYN result files were created by a revision previous to 14.0 (e.g., 13.0), then equivalent strain contours (and probes) will employ the older (pre-14.0) formulation. Hence, if you resume a pre-14.0 database with pre-14.0 result files and insert an equivalent strain, then Technique One will be attempted.
If you resume a pre-14.0 database which already contains an equivalent strain result/probe in the Solution tree, then the older (pre-14.0) formulation remains in effect.