Solid Stress Solver Reference

The Solid Stress Solver node allows you to access computation parameters, such as the Sparse Direct Solver settings, the update method for the stiffness matrix in nonlinear applications, and the Static Analysis option for quasi-static analysis with the Implicit Unsteady model. The Solid Stress Solver node also allows you to estimate the simulation memory requirements.

Solid Stress Solver Properties

Load Stepping

When activated, Simcenter STAR-CCM+ adds the Solid Stress Load Step solver under the Solvers node. This solver allows you to apply external loads gradually and is suitable for simulations with large nonlinearities.

启发式解析约束冲突

激活时，Simcenter STAR-CCM+ 使用启发式方法解析约束冲突和循环依赖性。在某些情况下，该解析方法会影响求解并导致出现不切实际的结果。当此选项处于活动状态时，确保评估求解的有效性。

默认情况下，此属性处于停用状态。在 15.06 之前的 Simcenter STAR-CCM+ 版本中，启发式冲突解析是默认方法。

Temporary Storage Retained

When activated, the solver retains the residuals that are computed at each iteration. These are available through the following field functions:

Displacement Increment [m] (see Eqn. (4833))
Residual Force [N] (see Eqn. (4833))

For other common properties, see Finite Element Solvers Reference: Common Properties.

Uzawa Method Controls

Stopping Criteria

The Augmented Lagrangian (Uzawa algorithm) contact constraint enforcement option has stopping criteria based on the convergence of displacement, force, and the number of iterations used per update:

Uzawa Update Displacement Criterion
Uzawa Update Force Criterion
Maximum Steps per Uzawa Update

When you set the solver Verbosity to High Simcenter STAR-CCM+ reports the residual values in the Output window. You can control the normalization of the residual values by setting the Normalization Option of the corresponding Force, and Displacement monitors, under the Monitors node. For more information on the Normalization Option, see Monitor Properties.

When you use the Uzawa algorithm with the Solid Stress solver, the Uzawa update loop is embedded within the iterations of the Solid Stress solver. An Uzawa augmentation is performed when the stopping criteria are satisfied.

The Uzawa Update Displacement Criterion and Uzawa Update Force Criterion have the following properties:

Minimum Value: The minimum value of the residual that satisfies the criterion. The criterion is satisfied when the value of the residual is less than the Minimum Value. The default value is the product between the Multiplier property value and the Minimum Limit that you specify for the corresponding Reference Stopping Criterion.
Use Reference Minimum Value: When activated (default), the Minimum Value is equal to the Minimum Limit of the Reference Stopping Criterion times the Multiplier. When deactivated, you specify the minimum value directly using the Minimum Value property. Specifying a value for the Minimum Value automatically deactivates Use Reference Minimum Value. You can activate Use Reference Minimum Value only when the Criterion Option of the Reference Stopping Criterion is set to Minimum.
Multiplier: The value of the multiplicative factor applied to the Minimum Limit of the Reference Stopping Criterion, to determine the Minimum Value of the Uzawa Method Controls > Stopping Criteria.
Reference Stopping Criterion (read-only): The Stopping Criterion whose Minimum Limit is used as a reference value by the Uzawa Method Controls > Stopping Criteria. The Uzawa Update Displacement Criterion uses Displacement Criterion as the Reference Stopping Criterion, and the Uzawa Update Force Criterion uses Force Criterion.
Criterion Satisfied: Indicates if the stopping criterion has been satisfied (read-only).

The Maximum Steps per Uzawa Update criteria has the following properties:

Maximum Steps: Defines the maximum number of steps used during the Uzawa Augmentation loop.

For more information on the common properties of stopping criteria, see 使用自动生成的停止条件.

Solid Stress Solver Right-Click Actions

Estimate Memory

Estimates the memory required by the Solid Stress Solver, based on the Sparse Direct Solver settings. When the estimate is complete, the Output window reports the following information:

N—model degrees of freedom
NZ(A)—number of non-zero elements in the stiffness matrix
mem(A) (MB)—memory required to store the stiffness matrix
mem(fact) (MB)—memory required to factorize the stiffness matrix
mem (MB)—total memory required by the Solid Stress Solver

When you set the Sparse Direct Solver mode to AUTO, the report displays the memory requirements for both In-Core and Out-of-Core running modes. If you set the solver mode to either In-Core or Out-of-Core, the report only displays the memory requirements for the relevant running mode. For more information, see FE 稀疏直接求解器参考.

Solid Stress Solver Controls

Integration Method

The time integration method depends on the temporal discretization scheme for the Implicit Unsteady solver.

When the Implicit Unsteady solver uses 1st-order discretization, Simcenter STAR-CCM+ sets the Integration Method to Backward-Euler (see Eqn. (4600)).
When the Implicit Unsteady solver uses 2nd-order temporal discretization, you can set the Integration Method to either Backward Differentiation (2nd Order) (see Eqn. (905)), Generalized-α (see Eqn. (4605)), or Newmark (see Eqn. (4601)).

You cannot change the time integration scheme during the computation of the solution. For the Generalized-α method, you can change the properties of the integrator when the simulation is paused or through a field function. However, the change to the parameters only takes effect at the end of the current time-step.

Integration Method > Backward Differentiation (2nd Order)

This integration method is recommended for unstable simulations and second-order FSI simulations.

For nonlinear solid-only simulations, you are best to use the Generalized-α method, as it provides a high fidelity solution whilst allowing you to control the amount of numerical dissipation.

Integration Method > Generalized-α

This integration method damps unphysical high frequency modes in the numerical solutions. For example, for elastodynamic simulations. This method offers higher accuracy in the final solution compared to the Newmark method.

The effective stiffness matrix for the Generalized-

α

method is given by Eqn. (4610).

The following options are available:


Property	Setting
Amount of Dissipation Allows you to choose how much numerical dissipation is introduced to the system. You are advised to set this property as low as possible.	None—no numerical dissipation is applied. Low—Simcenter STAR-CCM+ automatically sets an Amplitude Decay Factor (see Eqn. (4614)), which introduces a small amount of numerical dissipation. Moderate—Simcenter STAR-CCM+ automatically sets an Amplitude Decay Factor, which introduces a moderate amount of numerical dissipation. User Specified—allows you to specify the Amplitude Decay Factor, and ρ_inf ( $ρ_{\infty}$ , see Eqn. (4614)), to control the amount of numerical dissipation. Only recommended for expert users.
Amplitude Decay Factor Defines $λ$ in Eqn. (4614). Only available if Amount of Dissipation is set to User Specified.	N/A
Method Allows you to define the method used to calculate the $α$ coefficients.	Optimal (Chung-Hulbert)—implements the Chung-Hulbert method. HHT (Hilber-Hughes-Taylor)—implements the HHT (Hilber-Hughes-Taylor) method. WBZ (Wood-Bossak-Zienkiewicz)—implements the WBZ (Wood-Bossak-Zienkiewicz) method.
α_f (Read Only) Defines $α_{f}$ in Eqn. (4616) or Eqn. (4617), depending on the method used.	N/A
α_m (Read Only) Defines $α_{m}$ in Eqn. (4615) or Eqn. (4618), depending on the method used.	N/A
ρ_inf Defines the spectral radius of the amplification matrix. See Eqn. (4614). Only available if Amount of Dissipation is set to User Specified	N/A

Integration Method > Newmark

If you set the Integration Method to Newmark, you can specify the Newmark parameter

γ

(as defined in Eqn. (4601)) using the Integration Method > Newmark node. The stiffness matrix for the Newmark method is given by Eqn. (4604).

注

If you specify initial displacements using the Tabular method, Simcenter STAR-CCM+ calculates the initial acceleration (see Eqn. (4602)) without considering the stresses that arise from the initial displacements. Additionally, if one of the finite elements has zero density or a 6-DOF solver is present, the initial acceleration is assumed to be zero.

Direct > Sparse Direct Solver

For linear materials and linear geometry, the algebraic equations for the static and dynamic problems, Eqn. (4595) and Eqn. (4598), are linear and can be solved implicitly using a linear direct solver in only one iteration, or time-step. For nonlinear geometry, the equations are nonlinear and the solution requires updates of the stiffness matrix using Newton iteration methods. At each iteration step, the direct solver solves the linearized system of equations.

For linear problems, Simcenter STAR-CCM+ factorizes and stores the stiffness matrix only once, in the first iteration. Thereafter, if you change the constraints type, the Implicit Unsteady solver time-step, the mesh, or the settings for the mid-side vertex option, Simcenter STAR-CCM+ detects the changes in the stiffness matrix and refactorizes it during the next iteration. For nonlinear problems, Simcenter STAR-CCM+ factorizes the stiffness matrix every time the matrix is updated, based on the specified Newton update method.

For information on the properties available to this solver, see FE 稀疏直接求解器参考.

Static Analysis

When using the Implicit Unsteady solver for dynamic analysis, you can choose to run the analysis in static mode by activating Static Analysis. When you activate this option, the solver neglects the inertial terms and damping in the dynamic equations, and solves the equations for the static problem. In this case, you can create profiles for loads and constraints based on the pseudo-time.

Initialize Acceleration

Only available for implicit unsteady simulations when you set the Intergration Method to either Newmark or Generalized-α, and you have deactivated Static Analysis.

When active, Simcenter STAR-CCM+ calculates the initial acceleration at

t = 0

using Eqn. (4602). Otherwise the acceleration is initialized to zero.

Stiffness Matrix Update

Available when the Nonlinear Geometry model is active.

Allows you to choose the method that Simcenter STAR-CCM+ uses to update the stiffness matrix. The available options are:

Full Newton:
Simcenter STAR-CCM+ updates the stiffness matrix at each iteration step.
Modified Newton:
Allows you to specify the stiffness matrix Update Frequency, M. In static simulations, Simcenter STAR-CCM+ updates the stiffness matrix every M iterations. In quasi-static or dynamic simulations, Simcenter STAR-CCM+ updates the stiffness matrix for the first M iterations in a time-step. For example, if you specify M=1, the stiffness matrix is updated upon the first iteration of each time-step. If you specify M=3, the stiffness matrix is updated upon the first, second and third iteration of each time-step.

注

Every update of the stiffness matrix requires a new factorization step. The Modified Newton method allows for reuse of the decomposed stiffness matrix, saving overall run time, but it is less robust than the Full Newton method. You are advised to use the Modified Newton method only for moderately nonlinear problems.