Solution Information Object

You can track, monitor, or diagnose problems that arise during any solution as well as view certain finite element aspects of the engineering model, using a Solution Information object, which is inserted automatically under a Solution object of a new environment or an environment included in a database from a previous release. You can also manually insert a Solution Information object under a Connections object for solver feedback.

When you select a Solution Information object in the tree, the following controls are available in the Details view under the Solution Information category:

Solution Output

The Solution Output property defines how you want solution response results to display. All of the options, described below, display results in real time as the solution progresses.


Important:  The Solution Output property is not applicable to the Connections object.


  • Solver Output (default): Displays the solution output file (in text format) from the appropriate solver (Mechanical APDL, Explicit Dynamics, etc.). This option is valuable to users who are accustomed to reviewing this type of output for diagnostics on the execution of their solver of choice.

Choosing any of the following options displays a graph of that option as a function of Cumulative Iteration/Cycle (availability depends on the solver).

  • Force Convergence1

  • Displacement Convergence1

  • Rotation Convergence1

  • Moment Convergence1

  • Participation Factor Summary: This property displays Participation Factor Summary in the Worksheet. When selected, the property Summary Type also displays and its options include:

    • All (default): All tables are displayed in the Worksheet, including Participation Factor, Effective Mass, and Cumulative Effective Mass Ratio.

    • Participation Factor: Only Participation Factor table is displayed in the worksheet.

    • Effective Mass: Only Effective Mass table is displayed in the worksheet.

    • Cumulative Effective Mass Ratio: Only Cumulative Effective Mass Ratio table is displayed in the worksheet.

      Participation Factor Summary Contents

      Complex eigenvalues are available when the Damping property is set to Yes (except when the Reduced Damped Solver Type is selected and the Store Complex Solution property is set to No). When the Damping property is set to No, only the Unsymmetric Solver Type provides complex Eigenvalues.

      When you have a complex eigenvalue solution, the Participation Factor Summary Worksheet tables display Mode, Frequency, X Direction (Real), Y Direction (Real), Z Direction (Real), X Direction (Imaginary), Y Direction (Imaginary) and Z Direction (Imaginary). Otherwise the worksheet tables display Mode, Frequency, X Direction, Y Direction, Z Direction, Rotation X, Rotation Y and Rotation Z.


    Important:  The unit system for all of the data displayed in the Participation Factor Summary Worksheet is the unit system for the Solver Unit System property in the Analysis Data Management category of the Analysis Settings object.



    Note:
    • The Participation Factor Summary output option is not available when cyclic symmetry is active.

    • If the Campbell Diagram property is set to On in the Modal system's Analysis Settings (multi-step Modal analysis), the Participation Factor Summary reported in the Worksheet is for the last rotational velocity/load step.


  • Max DOF Increment

  • Line Search

  • Time

  • Time Increment

  • CSG Convergence1 (magnetic current segments)

  • Heat Convergence1

  • Energy Conservation: shows plots of total energy, reference energy, work done, and energy error.

  • Momentum Summary: shows plots of X, Y and Z momentum and X, Y and Z impulse for the model.

  • Energy summary: shows plots of internal energy, kinetic energy, hourglass energy and contact energy.

  • Post Output: displays the output of a Post Command snippet.

  • Solver Output (default): Displays the solution output file (text) from the appropriate solver (for example, the Mechanical APDL application, Explicit Dynamics). This option is valuable to users who are accustomed to reviewing this type of output for diagnostics on the execution of their solver of choice.

  • Solve Script Output: (Design Assessment system only) Displays the log file from the python Solve script specified for the current Design Assessment system.

  • Evaluate Script Output: (Design Assessment system only) Displays the log file from the python Evaluate script specified for the current Design Assessment system.

  • Optimization Output: This option displays the solution output (in text format) from the Topology Optimizer solver.

    Mechanical also provides the following convergence charts for the Topology Optimization analysis. These options provide plots (in the Worksheet) for convergence values determined during the solution. This is useful for determining if the simulation is nearing convergence. All of these options have a plot for the combined objective value versus the Convergence Accuracy as defined in the Definition Analysis Settings for the Topology Optimization environment. Note that individual objective values can occur separately in a multi-step analysis. These options also include a plot for the convergence of the Response Constraint that you wish to observe (Mass, Volume, etc.).

    • Objective and Mass Response Convergence: This option is the default option for a Topology Optimization Analysis. This property plots the Mass Response Convergence against the criterion you specify in the Percent to Retain property of the Mass Constraint object (Response Constraint). The convergence chart will plot convergence against Percent To Retain (Min) and Percent To Retain (Max) criterion, if the constraint is defined by Range.

    • Objective and Volume Response Convergence: This property plots the Volume Response Convergence against the criterion you specify in the Percent to Retain property of the Volume Constraint object (Response Constraint). The convergence chart will plot convergence against Percent To Retain (Min) and Percent To Retain (Max) criterion, if the constraint is defined by Range.

    • Objective and Global Stress Response Convergence (Static Structural analyses only): Plots the stress response convergence against the criterion specified in the Maximum property of the Global Von-Mises Stress Constraint object. For multi-step analyses, the application provides fields to enable you to choose which Step Number corresponds to the stress constraint you wish to observe.

    • Objective and Local Stress Response Convergence (Static Structural analyses only): Plots the local stress response convergence against the criterion specified in the Maximum property of the Local Von-Mises Stress Constraint object. For multi-step analyses, the application provides fields to enable you to choose which Step Number corresponds to the stress constraint you wish to observe.

    • Objective and Displacement Response Convergence (Static Structural analyses only): Plots the displacement response convergence against the criterion specified in X Component (Max)/Y Component (Max)/Z Component (Max) of the Displacement Constraint object. For multi-step analyses, the application provides fields to enable you to choose which Step Number corresponds to the displacement constraint you wish to observe.

    • Objective and Reaction Force Response Convergence (Static Structural analyses only): Plots the reaction force response convergence against the criterion specified in X Component (Max)/Y Component (Max)/Z Component (Max) of the Reaction Force Constraint object. For multi-step analyses, the application provides fields to enable you to choose which Step Number corresponds to the reaction force constraint you wish to observe.

    • Objective and Natural Frequency Convergence (applicable for Modal analyses): Plots the Natural Frequency Response convergence against the criterion specified in the Minimum Frequency and Maximum Frequency properties of the Natural Frequency Constraint object (Response Constraint). The application provides a field to enable you to specify a Mode Number corresponding to a natural frequency range you wish to observe.

    • Objective and Manufacturing Convergence (applicable when criterion is entered for the Maximum property of the Manufacturing Constraint object): Plots the manufacturing response convergence against the criterion specified in the Maximum property of the Member Size category of the Manufacturing Constraint object when the Maximum property is set to Manual.


Note:
  • The frequency at which data is written can be specified as a time step frequency or a physical time frequency. By default information is displayed for every 100 time steps.

  • For ease of viewing solutions with many substeps/iterations, the Substep Converged and Load Step Converged lines are not displayed when the number of lines exceeds 1000. Also, graphs are shown as lines only, rather than lines and points, when the number of points exceeds 1000.


1 - All convergence plots include designations where any bisections, converged substeps, converged steps, or remesh points occur. These designations are the red, green, blue, or orange lines (solid or dotted) shown in the example below of a Force Convergence plot.

Newton-Raphson Residuals

This property is applicable only to Structural environments solved with the Mechanical APDL application. It specifies the maximum number of Newton-Raphson residual forces to return. The default is 0 (no residuals returned). You can request that the Newton-Raphson residual restoring forces be brought back for nonlinear solutions that either do not converge or that you aborted during the solution. The Newton-Raphson force is calculated at each Newton-Raphson iteration and can give you an idea where the model is not satisfying equilibrium. If you select 10 residual forces and the solution doesn't converge, those last 10 residual forces will be brought back. The following information is available in the Details view of a returned Newton-Raphson Residual Force object:

  • Results: Minimum and Maximum residual forces across the model

  • Convergence: Global convergence Criterion and convergence Value

  • Information: Time based information

These results cannot be scoped and will automatically be deleted if another solution is run that either succeeds or creates a new set of residual forces.

Identify Element Violations

This property is a diagnostic tool that enables you to identify and view elements on your model that have failed to meet certain solver criteria during the solution process. The application generates an error message and creates Named Selection objects that contain the elements that violate the following criteria:

  • Distortion too large (HDST)

  • Elements that contain nodes that have near zero pivots (PIVT) for nonlinear analyses

  • Plastic/creep strain increment is too large (EPPL/EPCR)

  • Elements for which mixed u-P constraints are not satisfied (MXUP) - mixed U-P option of 18x solid elements only

  • Radial displacement (RDSP) is not converged

For the system generated Named Selections that are scoped to the failed elements, the application generated "name" includes a reference to the specific failed criterion, such as "HDST" for a distortion that is too large. These Named Selections are placed under the Solution Information object.

The default setting for this property is 0 (no violations are returned). This value can be set to an n, where n is an integer value greater than 0. This value defines the last n solver iterations for which the failed elements are stored.

The system generated Named Selections behave as user-defined element-based named selections and as desired, you can scope results to these named selections. In addition, unlike other diagnostic features, these Named Selections are not automatically deleted or overwritten upon subsequent solutions. As needed, you need to delete then manually.

You can find additional details in the Element Components That Violate Criteria topic of the NLDIAG command section of the Mechanical APDL Command Reference. Also see the Performing Nonlinear Diagnostics topic in the Nonlinear Structural Analysis section of the Mechanical APDL Structural Analysis Guide.

Update Interval

This property appears only for synchronous solutions. It specifies how often any of the result tracking items under a Solution Information object get updated while a solution is in progress. The default is 2.5 seconds.

Display Points

This property is not applicable to Connections object. It specifies the number of points to plot for a graphical display determined by the Solution Output setting (described above).

Display Filter During Solve

This property is applicable only when using Result Tracker filtering in Explicit Dynamics analyses. When set to Yes, it displays filtered data from Result Trackers in the Worksheet at each refresh interval of the Result Tracker. As shown below, a legend is included in the Worksheet to help distinguish the filtered data from the non-filtered data. Typically there are two curves, non-filtered data is displayed in red, and filtered data is displayed in green.

Solution Output (Design Assessment System Only)

[Not applicable to Connections object] For a Design Assessment system, this property presents the following options for determining the display of (real time) solution response results.

  • Solver Output (default): Displays the solution output file (text) from the appropriate solver (for example, the Mechanical APDL application, Explicit Dynamics). This option is valuable to users who are accustomed to reviewing this type of output for diagnostics on the execution of their solver of choice.

  • Solve Script Output: Displays the log file from the python Solve script specified for the current Design Assessment system.

  • Evaluate Script Output: Displays the log file from the python Evaluate script specified for the current Design Assessment system.


Note:  If an error occurs during a solve when using the ANSYS solver, the Solution Information worksheet may point you to files (for example, file.err) in temporary scratch folders whose purpose is for solving only (this is the folder where ANSYS actually ran). After the solution, these files are moved back to the project structure, so you may not find them in the scratch folders (or sub-folders).


Viewing Finite Element Connections

During the solution, the Mechanical application will sometimes create additional elements or Constrain Equations (CE) for certain objects such as a remote boundary condition, spot weld, joint, MPC based contact, or weak spring. So that you might better understand how the boundary conditions are applied, the Mechanical application allows you to “view” these connections after a solution is completed. The following controls are available in the Details view under the FE Connection Visibility category:


Note:  Finite element connection information is not available for Response Spectrum analyses when the Spectrum Type property is set to Single Point.


Tracking Background Solutions

When running background solutions, you can check the status of the solution by using the Retrieve feature, which is available in a context menu when you right-click the mouse button on the Solution Information object. A Retrieve button is also available on the Solution Information toolbar. In rare instances, the Retrieve feature could fail if the necessary files do not become available at a particular time. Simply choosing Retrieve again will likely solve the issue.


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