Solver Controls

The properties provided by the Solver Controls category vary based on the specified Analysis Type. This table denotes which Details view properties are supported for each analysis type. The remainder of the section describes the functions and features of the properties.

Details View Properties

Analysis Type
Static Structural Transient Structural Rigid Dynamics Modal Modal Acoustics Eigenvalue Buckling Steady - State Thermal Transient Thermal Magnetostatic Electric Thermal Electric

Topology Optimization

Damped    
       
Solver Type
 
Mode Reuse    
        
Store Complex Solution    
        
Weak Springs
          
Solver Pivot Checking
     
     
Large Deflection
          
Inertia Relief
           
Include Negative Load Multiplier      
      
Time Integration and Constraint Stabilization   
         

Damped

The Damped property options include Yes and No (default). Set the property to Yes to enable a damped system where the natural frequencies and mode shapes become complex.

Solver Type

The options of the Solver Type property can vary based upon the type of analysis you are performing. In general, the Solver Type options include:

See the Help for the EQSLV command in the Mechanical APDL Command Reference for more information about solver selection.

Based on the analysis type, additional Solver Type options are described below.

Modal Analysis

For a Modal Analysis when the Damped property is set to No, Solver Type options include the common settings, Program Controlled (default), Direct, and Iterative as well as the following:

  • Unsymmetric

  • Supernode

  • Subspace

The Direct, Iterative, Unsymmetric, Supernode, and Subspace types are used to solve a modal system that does not include any damping effects (the Damped property is set to No). Except for the Unsymmetric option, the solver types are intended to solve Eigen solutions with symmetric mass and stiffness. For a large model, the Iterative solver is preferred over the Direct solver for its efficiency in terms of solution time and memory usage.

During a Modal analysis the:

  • Direct solver uses the Block Lanczos extraction method that employs an automated shift strategy, combined with a Sturm sequence check, to extract the number of eigenvalues requested. The Sturm sequence check ensures that the requested number of eigen frequencies beyond the user supplied shift frequency (FREQB on the MODOPT command) is found without missing any modes. See the Block Lanczos help in the Eigenvalue and Eigenvector Extraction section of the Mechanical APDL Theory Reference.

  • Supernode solver is recommended for extracting a large number of modes. Selecting Supernode as the Solver Type automatically sets the Limit Search to Range property to Yes in the Options category. This selection also displays the Range Minimum and Range Maximum properties and requires a Range Maximum frequency entry. Alternatively, you may reset the Limit Search to Range property to No to find all of the possible modes without any restrictions on the frequency range.

  • Subspace solver (unlike the Direct solver) does not perform Sturm sequence check by default (STRMCK is OFF by default in SUBOPT command), making it relatively faster than Direct solver and also has reasonable accuracy. In addition, the Subspace solver supports DANSYS allowing you to take advantage of a distributed architecture to perform faster computations.

  • Unsymmetric solver (for modal systems with unsymmetric mass and/or stiffness) is required for solving the Eigen solutions. See the Help for the MODOPT command in the Mechanical APDL Command Reference for more information about solver selection.

If the Damped property is set to Yes, the Solver Type options include:

  • Program Controlled (default)

  • Full Damped

  • Reduced Damped

The Reduced Damped solver is preferred over the Full Damped solver for its efficiency in terms of solution time. However, the Reduced Damped solver is not recommended when high damping effects are present because it can become inaccurate.

Modal Acoustics Analysis

If the Damped property is set to Yes, Full Damped is the only supported option for this analysis.

For a Modal Acoustics Analysis when the Damped property is set to No, Solver Type options include:

  • Program Controlled (default)

  • Direct

  • Subspace

  • Unsymmetric


Note:  When you have Fluid Solid Interface object defined in your model or the Element Type property is set to Coupled in the Acoustic FSI Definition of a Physics Region object, you must select Unsymmetric or Damped solver type to proceed with the solution.

Based on your configuration, select your solver type based on the following:

Element Type

Symmetric Formulation Setting

FSI Load

Required Solver Type

Coupled

Off

No

Unsymmetric/Damped

Coupled

On

No

Direct/Subspace/Damped

Uncoupled

Off

No

Direct/Subspace/Damped

Uncoupled

On

No

Direct/Subspace/Damped

Coupled

Off

Yes

Unsymmetric/Damped

Coupled

On

Yes

Direct/Subspace/Damped

Uncoupled

Off

Yes

Unsymmetric/Damped

Uncoupled

On

Yes

Direct/Subspace/Damped


Eigenvalue Buckling Analysis

For an Eigenvalue Buckling Analysis, the Solver Type options include:

  • Program Controlled (default)

  • Direct

  • Subspace

The Program Controlled option uses the Direct solver. Refer to the BUCOPT command for additional information about buckling analysis solver selection.

Topology Optimization

The Topology Optimization analysis Solver Type options include:

  • Program Controlled (default)

  • Sequential Convex Programming

  • Optimality Criteria

Mode Reuse (Modal Analyses Only)

The Mode Reuse property is only available for Modal analyses when you specify the Solver Type as Reduced Damped. This property allows the solver to compute complex eigensolutions efficiently during subsequent solve points by reusing the undamped eigensolution that is calculated at the first solve point. The default setting is Program Controlled. Set this property to Yes to enable it or No to disable the property.

Store Complex Solution (Modal Analyses Only)

This property is only available for a Modal Analysis and only when the Damped property is set to Yes and the Solver Type is set to Reduced Damped. It allows you to solve and store a damped modal system as an undamped modal system.

Weak Springs

For stress simulations, such as thermal-stress or press fit modeling, the addition of weak springs can facilitate a solution by preventing numerical instability, while not having an effect on real world engineering loads. The following Weak Springs settings are available in the Details view:

The default setting for this property can be modified using the Options dialog box. See the Specifying Options section of the Help under Analysis Settings and Solution.

Solver Pivot Checking

In the case of an underconstrained model or contact related issue, an ill conditioned solver matrix will produce an error message in the solver and abort the solution. This property instructs the solver how to handle such an instance. Options include:

The default setting for this property can be modified using the Options dialog box. See the Specifying Options section of the Help under Analysis Settings and Solution.

Large Deflection

This property, applicable to static structural and Transient Structural analyses, determines whether the solver should take into account large deformation effects such as large deflection, large rotation, and large strain. Set Large Deflection to On if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem).

When using hyperelastic material models, you must set Large Deflection On.

Inertia Relief (Linear Static Structural Analyses Only)

Calculates accelerations to counterbalance the applied loads. Displacement constraints on the structure should only be those necessary to prevent rigid-body motions (6 for a 3D structure). The sum of the reaction forces at the constraint points will be zero. Accelerations are calculated from the element mass matrices and the applied forces. Data needed to calculate the mass (such as density) must be input. Both translational and rotational accelerations may be calculated.

Requirements

The use of the Inertial Relief property requires the following:

Include Negative Load Multiplier (Eigenvalue Buckling Analysis Only)

For an Eigenvalue Buckling Analysis, this property allows you to select the range of eigenvalues (load multipliers) to be extracted. The default option Program Controlled and the option Yes will extract both the negative and positive eigenvalues (load multipliers). The No setting extracts only positive eigenvalues (load multipliers).

Time Integration Type (Rigid Dynamics Solver Only)

This feature is applicable to a Rigid Dynamics analysis.

The Time Integration Type feature employs the fourth and fifth order polynomial approximation of the Runge-Kutta algorithm to enable the Mechanical application to integrate the equations of motion during analyses. This feature allows you to choose time integration algorithms and specify whether to use constraint stabilization.

The Details view Solver Controls options for the Time Integration Type include:


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