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 | ||
| 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 |
![]() | |||||||||||
The Damped property options include and (default). Set the property to to enable a damped system where the natural frequencies and mode shapes become complex.
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:
(default): this setting enables the application to select the optimal solver.
: this setting uses the Sparse solver.
: this setting uses the PCG or ICCG (for Electric and Electromagnetic analyses) solver.
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.
For a Modal Analysis when the Damped property is set to , Solver Type options include the common settings, (default), , and as well as the following:
The , , , , and types are used to solve a modal system that does not include any damping effects (the Damped property is set to ). Except for the option, the solver types are intended to solve Eigen solutions with symmetric mass and stiffness. For a large model, the solver is preferred over the solver for its efficiency in terms of solution time and memory usage.
During a Modal analysis the:
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.
solver is recommended for extracting a large number of modes. Selecting as the Solver Type automatically sets the Limit Search to Range property to 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 to find all of the possible modes without any restrictions on the frequency range.
solver (unlike the solver) does not perform Sturm sequence check by default (STRMCK is OFF by default in SUBOPT command), making it relatively faster than solver and also has reasonable accuracy. In addition, the solver supports DANSYS allowing you to take advantage of a distributed architecture to perform faster computations.
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 , the Solver Type options include:
(default)
The solver is preferred over the solver for its efficiency in terms of solution time. However, the solver is not recommended when high damping effects are present because it can become inaccurate.
If the Damped property is set to , is the only supported option for this analysis.
For a Modal Acoustics Analysis when the Damped property is set to , Solver Type options include:
(default)
Note: When you have Fluid Solid Interface object defined in your model or the Element Type property is set to in the Acoustic FSI Definition of a Physics Region object, you must select or 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 |
For an Eigenvalue Buckling Analysis, the Solver Type options include:
(default)
The option uses the solver. Refer to the BUCOPT command for additional information about buckling analysis solver selection.
The Topology Optimization analysis Solver Type options include:
(default)
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 . Set this property to to enable it or to disable the property.
This property is only available for a Modal Analysis and only when the Damped property is set to and the Solver Type is set to . It allows you to solve and store a damped modal system as an undamped modal system.
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:
: Mechanical determines if weak springs will facilitate the solution, then adds a standard weak spring stiffness value accordingly.
: Mechanical always adds a weak spring stiffness. Choosing causes a Spring Stiffness option to appear that allows you to control the amount of weak spring stiffness. Your choices are to use the standard stiffness mentioned above for the setting of Weak Springs or to enter a customized value. The following situations may prompt you to choose a customized stiffness value:
The standard weak spring stiffness value may produce springs that are too weak such that the solution does not occur, or that too much rigid body motion occurs.
You may judge that the standard weak spring stiffness value is too high (rare case).
You may want to vary the weak spring stiffness value to determine the impact on the simulation.
The following Spring Stiffness settings are available:
(default setting): Adds a standard weak spring stiffness (same as the value added for the setting of Weak Springs).
Factor: Adds a customized weak spring stiffness whose value equals the standard value times the value you enter in the Spring Stiffness Factor field (appears only if you choose Factor). For example, setting Spring Stiffness Factor equal to 20 means that the weak springs will be 20 times stronger than the standard value.
Manual: Adds a customized weak spring stiffness whose value you enter (in units of force/length) in the Spring Stiffness Value field (appears only if you choose Manual).
(default setting): Weak springs are not added. By default, the application does not include weak springs for the solution.
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.
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:
(default): Allows the solver to determine the response.
: Instructs the solver to continue upon detection of the condition and attempt the solution.
: Instructs the solver to stop upon detection of the condition and issue an error message.
: Pivot checking is not performed.
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.
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.
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:
This option applies only to the linear static structural analyses. Nonlinearities, elements that operate in the nodal coordinate system, and axisymmetric or generalized plane strain elements are not allowed.
Models with both 2D and 3D element types or with symmetry boundary constraints are not recommended. Loads may be input as usual. Displacements and stresses are calculated as usual.
Symmetry models are not valid for an inertia relief analysis.
If the Inertial Relief property is set to On, then any analysis linked to the Static Structural analysis is invalid. This includes a Static Structural analysis linked to the following analysis types:
Pre-stressed Modal
Eigenvalue Buckling
Pre-stressed FULL Harmonic Response
Pre-stressed MSUP Harmonic Response
Pre-stressed MSUP Transient
Pre-stressed Response Spectrum
Pre-stressed Random Vibration
For an Eigenvalue Buckling Analysis, this property allows you to select the range of eigenvalues (load multipliers) to be extracted. The default option and the option will extract both the negative and positive eigenvalues (load multipliers). The setting extracts only positive eigenvalues (load multipliers).
This feature is applicable to a 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:
Time Integration Type field. Available time integration algorithms include:
Program Controlled (default setting): The application selects the most appropriate method based on the current model. If the model contains only rigid bodies, 4th order Runge-Kutta is used. If the model contains flexible bodies (Condensed Parts), the Implicit Generalized Alpha option is selected automatically.
Runge-Kutta 4: Fourth Order Runge-Kutta.
Runge-Kutta 5: Fifth Order Runge-Kutta.
Implicit Generalized Alpha: Implicit time integration based on the Generalized-α method.
MJ Time Stepping: Moreau-Jean time-stepping integration.
Use Stabilization: When specified, this option provides the numerical equivalent for spring and damping effects and is proportional to the constraint violation and its time derivative. If there is no constraint violation, the spring and damping has no effect. The addition of artificial spring and damping does not change the dynamic properties of the model. Stabilization options include:
(default setting): constraint stabilization is ignored.
: Because constraint stabilization has a minimal impact on calculation time, its use is recommended. When specified, the Stabilization Parameters field also displays. Stabilization Parameters options include:
: valid for most applications.
: manual entry of spring stiffness () and damping ratio () required.
Note: Based on your application, it may be necessary to enter customized settings for and . In this case, start with small values and use the same value in both fields. and values that are too small have little effect and values that are too large cause the time step to be too small. The valid values for and are > = 0 and > = 0. If Both and are zero, the stabilization will have no effect.
Use Position Correction: (default) or .
Use Velocity Correction: (default) or .
Correction Type: (default) or .

Assembly Type: (default) or .

Drop-Off Tolerance