Solid Stress Model Reference

Reference Values

Geometry Refinement Specification

When you constrain a surface, Simcenter STAR-CCM+ applies the constraint on the mesh vertices that lie on that surface (see Solid Stress Constraints). For accurate boundary conditions, it is important that the geometry of the surface is locally captured.

To represent the geometry of curved surfaces, Simcenter STAR-CCM+ evaluates unique vertex normals at each mesh vertex by averaging the normals of the adjacent mesh faces [131]. The vertex normals provide a more accurate representation for radial (normal) directions.

On a feature edge, where two different surfaces meet, Simcenter STAR-CCM+ must retain multiple normals per vertex. Simcenter STAR-CCM+ recognizes a feature edge between two surfaces based on the specified Dihedral Angle Tolerance. If the angle between the adjacent face normals exceeds the specified tolerance, Simcenter STAR-CCM+ retains multiple normals. If the angle between the adjacent face normals is within the specified tolerance, Simcenter STAR-CCM+ generates a unique vertex normal.

In general, you are advised to leave the Dihedral Angle Tolerance as the default value.

For surfaces meeting at small angles, you can decrease the Dihedral Angle Tolerance so that Simcenter STAR-CCM+ recognizes the feature edge shared by the two surfaces. For coarse meshes, where different faces of the same surface meet at large angles, you can increase the Dihedral Angle Tolerance so that Simcenter STAR-CCM+ recognizes the surface as continuous and generates the unique vertex normal.

You can specify the Dihedral Angle Tolerance independently in each region using the Geometry Refinement Option. See Region Inputs.

注	For vertices that lie on symmetry plane boundaries, the calculation of vertex normals is consistent with the full geometry resulting from the symmetry condition.

Initial Conditions

Displacement

Allows you to specify the initial displacement as a vector profile.

Stress analysis requires you to constrain the solid structure by prescribing the displacement vector at appropriate surfaces, curves, or points (see Applying Constraints). In dynamic analyses, the specified constraints take precedence over the initial conditions when conflicts occur. During the first iteration, the displacement solution transitions from the initial condition to the specified constraint. After the first iteration, the solid structure deforms under the specified loads and constraints. Specifying a nonzero initial displacement for the unconstrained degrees of freedom can lead to unbalanced residual forces and divergence of the solution.

Velocity

Allows you to specify the initial velocity as a vector profile.

Boundary Types

Wall

By default, wall boundaries are free from loads and constraints. Wall boundaries present a Stress/Displacement physics condition, which is always set to Free. This condition is read only, as you define loads and constraints on the associated part surfaces using segments. See Segments (Loads and Constraints) Reference.

Symmetry Plane

At symmetry plane boundaries, Simcenter STAR-CCM+ automatically sets the normal component of displacement to zero. As with wall boundaries, you can define loads and constraints on the associated part surfaces using segments (see Segments (Loads and Constraints) Reference.). However, do not define constraints that specify a nonzero normal displacement, as this would result in conflicting constraints.

Region Settings

Applies to solid regions.

Body Load Derivative

Only available when you set Body Load Option to Specified.

Allows you to define the partial derivatives of the body force with respect to displacement, velocity, or acceleration. You can define more than one derivative in the same simulation.

Properties	Corresponding Physics Value Nodes
Displacement Derivative Allows you to specify the displacement derivative ( $D_{u}b$ in Eqn. (4571)).	Body Load Displacement Derivative Specifies the derivative as a Composite Symmetric Tensor, Composite Tensor, Isotropic Tensor, or Principal Tensor.
Velocity Derivative Allows you to specify the velocity derivative ( $D_{v}b$ in Eqn. (4572)). Only available for unsteady simulations.	Body Load Velocity Derivative Specifies the derivative as a Composite Symmetric Tensor, Composite Tensor, Isotropic Tensor, or Principal Tensor.
Acceleration derivative Allows you to specify the acceleration derivative ( $D_{a}b$ in Eqn. (4573)). Only available for unsteady simulations.	Body Load Acceleration Derivative Specifies the derivative as a Composite Symmetric Tensor, Composite Tensor, Isotropic Tensor, or Principal Tensor.

For each body load derivative you can also define the Coordinate System the tensor is defined in under the Physics Values > [Derivative] > [Tensor] node. If you are using a local coordinate system, it is recommended you use the same coordinate system for both the Body Load Derivative and Body Load Option. In this case, you can also express the body load in terms of the displacement field function with respect to the local coordinate system (see Referencing Local Coordinate Systems).

Body Load Option

Allows you to apply a body force on the region. Its counterpart in CFD is the Momentum Source Option. The Body Load Option is intended for body loads which are independent of the stress and strain, but may be a function of the displacement field.

Method	Corresponding Physics Value Nodes
None No body forces are applied.	None
Specified Allows you to apply a body force on the region. For the body force, you can also specify its derivatives with respect to displacement, velocity, and acceleration.	Body Load Defines the body force vector $b$ in Eqn. (4570) along with the Coordinate System the vector is defined in. Body Load Derivatives Allows you to define the partial derivatives of the body force with respect to displacement, velocity, or acceleration (see Body Load Derivatives).

Geometry Refinement Option

For a given region, allows you to overwrite the Dihedral Angle Tolerance specified in the physics continuum (see Geometry Refinement Specification).

Option	Corresponding Physics Value Nodes
Use Continuum Values Sets the Dihedral Angle Tolerance to the value specified in the associated physics continuum. See Geometry Refinement Specification	None
Specified Sets the Dihedral Angle Tolerance to a specified value.	Geometry Refinement Specification Specifies the Dihedral Angle Tolerance for the region. This value overwrites the physics continuum Geometry Refinement Specification.

Mid-side Vertex Option

Allows you to add or remove mid-side vertices. By default, Simcenter STAR-CCM+ mesh operations generate linear elements without mid-side vertices.

Although you can change this setting at any time during a simulation, Simcenter STAR-CCM+ adds or removes the vertices during initialization, when you run the simulation. To verify the mesh element topology, you can visualize the Element Type field function in a scalar scene for the part. For more information, see Mesh Requirements and Guidelines.

The available methods are:

• Add -- Linear Interpolation—adds mid-side vertices (nodes) as linear interpolates of the vertices on either end of an edge. This option adds mid-side nodes to each edge of every element of the mesh. When you add mid-side nodes, Simcenter STAR-CCM+ also interpolates any previous solution, computed on the linear mesh, to the mid-side vertices. The addition of mid-side nodes forces a new evaluation and factorization of the stiffness matrix.
• Keep Original—keeps the original mesh element configuration. If you generated the mesh in Simcenter STAR-CCM+, and you have not added mid-side nodes, the mesh elements remain linear. If you have added mid-side nodes, the mesh elements remain quadratic. If you imported the mesh through an imported CAE model, the element topology remains linear/quadratic, based on the original configuration.
• Remove All—removes any mid-side nodes. This option includes mid-side nodes that were added in Simcenter STAR-CCM+, or mid-side nodes that were imported with a CAE model. The removal of mid-side nodes forces a new evaluation and factorization of the stiffness matrix.

Region Controls

Segments

Activating the Solid Stress physics model automatically creates a Segments folder in the regions node. If you deactivate the Solid Stress model, and no segments are present, Simcenter STAR-CCM+ also removes the Segments folder. See Segments (Loads and Constraints) Reference.

Interface Settings

Interfaces can be conformal or non-conformal, but not imprinted. Imprinting may create polyhedral cells, which are not supported in finite element analysis. The available conditions are:

Mechanical Interaction

Available for solid/solid interfaces of type Mapped Contact Interface.

Specifies the type of interaction between the contacting surfaces. This condition is available for mapped contact interfaces with Topology other than Periodic. The available options are:

• Bonded—the contacting surfaces undergo continuous displacements. If the solid regions are different materials, discontinuities in the strain are preserved across the material interface. Activates the Constraint Mapping condition.

  Simcenter STAR-CCM+ automatically treats periodic interfaces, contact interfaces, and internal interfaces as Bonded.

• Small Sliding Frictionless—allows the contacting surfaces to slide over each other in the direction tangential to the interface, whereas movement in the normal direction is prohibited. The shear stress at the interface is equal to zero, and the normal forces are equal and opposite.

  This option is intended for small sliding at flat interfaces. Sliding of vertices at curved interfaces, or sliding of vertices that exceed the mesh element length, leads to inaccurate results.

  This option targets applications where unrealistic stress concentrations would otherwise occur. For example, thermal-stress analysis involving interfaces between materials with different thermal expansion coefficients.

  This type of interaction is not compatible with the Solid Displacement motion.

约束映射

可用于映射接触交界面类型的固体/固体交界面。

指定 Simcenter STAR-CCM+ 用于约束粘合表面的方法。可用选项如下：

• 节点至表面：
  默认选项。在两个有限元之间的交界面处，次单元上的节点被约束到主单元上重叠表面的节点。通常，此方法所需的计算工作量较少，但它不保留线动量和角动量（在固体应力计算中）或热通量（在固体能量计算中），并且可能导致计算的应力或温度局部不精确。
  
  
• 表面至表面：
  在两个有限元之间的交界面处，次单元与主单元的重叠表面将细分在三角形中。在重叠表面上广义积分或弱积分以满足约束。与节点至表面方法相比，此方法保留线动量和角动量（在固体应力计算中）或热通量（在固体能量计算中），从而提高了计算的应力或温度的精度。但是，此方法需要更多的计算量，并且所需内存会随着使用的内核数而增加。
  
  

此选项仅适用于粘接映射接触交界面。滑动交界面自动使用节点至表面方法。

对于共享周长和节点的相邻交界面，建议使用相同的约束映射方法。使用这两种方法可能会导致过度约束共享节点。

Monitors

Displacement

Solid displacement increment [m] (see Eqn. (4833)).

Force

Residual force [N] (see Eqn. (4833)).

Strain Energy

Strain energy, defined with the unit of [Nm] (see Eqn. (4838)). This monitor is available when you activate the Strain energy property for the Solid Stress Solver (see Solid Stress Solver Reference).

With these monitors they have corresponding stopping criteria that automatically becomes available when Solid Stress Solver is activated. See Stopping Criteria.

Field Functions

Contact Gap

Scalar field function that represents the contact gap between the solid surface and rigid obstacle. The contact gap is defined as the distance between a point on the solid surface and the closest-point projection on the rigid obstacle surface. For the contact gap calculation, Simcenter STAR-CCM+ considers a single closest point for all the surfaces of the rigid obstacle. For very large penetrations, this closest point may not correspond to the expected physical contact direction.

The contact gap field function reflects the geometric contact gap calculated by Simcenter STAR-CCM+ as well as any additional Contact Gap Offset applied to the Rigid Contact segment. For regions and contacting boundaries containing more than one Rigid Contact segment, the region or face value is equal to the minimum contact gap defined by the segments. For regions and boundaries which do not belong to a Rigid Contact segment, the region or face value is equal to the maximum contact gap available.

This scalar field function is available on:

• All Rigid Contact segments.
• Solid boundaries with at least one Rigid Contact segment specified on the region. The part surfaces of the boundary do not need to be assigned to a Rigid Contact segment.
• Any solid region with at least one Rigid Contact segment specified.

Contact Pressure

For Mortar discretization of a rigid contact, represents the Cauchy contact pressure ( $p_n^s$ in Eqn. (4482)) between the solid surface and the rigid obstacle. Positive pressure corresponds to a compressive load.

The Contact pressure field function is available on:

• All Rigid Contact segments.
• Solid boundaries with at least one Rigid Contact segment specified on the region. The part surfaces of the boundary do not need to be assigned to a Rigid Contact segment.
• Any solid region with at least one Rigid Contact segment specified.

For regions, the contact pressure is equal to the area-weighted contact pressure on the part surfaces that form the Rigid Contact segments.

Discrete Contact Gap

For Mortar discretization of a rigid contact, represents the average contact gap from the projection of the continuous contact gap to the finite element nodes ( ${\hat{g}}_i$ in Eqn. (4500)).

The discrete contact gap field function is available on:

• All Rigid Contact segments.
• Solid boundaries with at least one Rigid Contact segment specified on the region. The part surfaces of the boundary do not need to be assigned to a Rigid Contact segment.
• Any solid region with at least one Rigid Contact segment specified.

For regions, the discrete contact gap is equal to the minimum discrete contact gap defined by the part surfaces that form the Rigid Contact segments.

Displacement

Vector field function that represents the displacement $u$ in Eqn. (4426).

Element Type

Scalar field function that identifies each element topology with a unique number. To visualize the mesh element type, display this field function in a scalar scene. If all the elements in the mesh are of the same type, the color bar will display a single number. The values associated with each element topology are listed in the section, Element Type Reference.

Log Strain Tensor

For non linear stress-strain analysis, the tensor field function represents the spatial logarithmic strain tensor, as defined in Eqn. (4449)

Rigid Body Acceleration

Defines the acceleration, $a_N$ , in [eqnlink]. When you activate the Coriolis - Solid Displacement Velocity Effect model, the additional Coriolis acceleration term ([eqnlink]) is added to the rigid body acceleration.

Rigid Body Velocity

Defines the velocity of the body due to rotational and translational motions.

Strain Tensor

For linear stress-strain analysis, the tensor field function represents the infinitesimal strain tensor, as defined in Eqn. (4444). For non linear stress strain analysis, tensor field function represent the Green-Lagrange Strain tensor, as defined in Eqn. (4445)

Stress Max. Shear

Scalar field function that represents the maximum shear stress, as defined in Eqn. (4437).

Stress Mean

Scalar field function that represents the mean stress measure, as defined in Eqn. (4438).

Stress Tensor

Tensor field function that represents the Cauchy stress tensor (see Cauchy Stress).

Stress Von Mises

Scalar field function that represents the von Mises stress measure, as defined in Eqn. (4440).

Forces

Applied Force

Vector field function that represents the resultant of the applied surface and point loads. At a node $M$ , it is defined as:

$$f_M^a={\displaystyle {\int }_S{\mathcal{N}}_M^T}\tau dS+{\displaystyle {\int }_C{\mathcal{N}}_M^T}\overline{q}dC+f_M$$

(344)

where ${\mathcal{N}}_M$ is a nodal shape function (see Eqn. (4550)), $\tau$ is the prescribed surface traction integrated over the relevant surfaces $S$ , $\overline{q}$ is the prescribed line load integrated over the relevant curves $C$ , and $f_M$ is the point load prescribed at node $M$ .

Body Force

Vector field function that represents the resultant of the body forces. At a node $M$ , it is defined as:

$$f_M^b={\displaystyle {\int }_V{\mathcal{N}}_M^T}bdV-C_{MN}{\dot{u}}_N-M_{MN}({\ddot{u}}_N+a_N-g_N)$$

(345)

where $b$ is the prescribed body load, $M_{MN}$ and $C_{MN}$ are the mass and damping matrices (see Eqn. (4559) and Eqn. (4576)), $a_N$ is the prescribed acceleration and $g_N$ is gravity.

When the Coriolis - Solid Displacement Velocity Effect model is activated, the Coriolis acceleration ([eqnlink]) is included in the rigid body acceleration $a_N$ .

Constraint Force

Vector field function that represents the reaction forces at constrained boundaries and at interfaces.

The residual forces at a mesh node $M$ , $r_M=f_M^a+f_M^b-f_M^{\mathrm{int}}$ can be expressed in terms of free and constrained degrees of freedom, $r_M=\{r_M^f,r_M^c\}$ . The residual forces of the free degrees of freedom must approach zero at convergence, $r_M^f=0$ . The negative residual forces of the constrained degrees of freedom, $-r_M^c$ , are called constraint forces.

Internal Force

Vector field function that represents the internal elastic forces, as defined in Eqn. (4558).

Rigid Body Force

Defines the forces acting on the body due to the rigid body motions.

The internal force, applied force, and body force at a mesh node $M$ are calculated as the sum of all element contributions connected to $M$, that is, the integrals Eqn. (344), Eqn. (345), and Eqn. (4558) are the sum over each element volume, surface, or edge associated with $M$.

For more information on how to use these field functions in scenes and reports, see Reports and 求解分析准则.

Reports

The Sum Force and Sum Moment reports allow you to check for equilibrium of all the forces and moments acting on specified input parts, as required by conservation of linear and angular momentum. Each part and the sum of all input parts must be in equilibrium. The Sum Force and Sum Moment reports are defined with respect to a Cartesian coordinate system.

Sum Force

Reports the resultant of the applied, body, internal, or constraint forces on the specified input parts. The input parts for this type of report can either be geometry parts or regions.

Simcenter STAR-CCM+ first calculates the force resultants per input part, by summing all the forces at the part nodes, and then sums the resultants calculated for each input part.

For example, to calculate the Sum Force of the Applied Force, Simcenter STAR-CCM+ calculates the resultant of the Applied Force for each input part, as:

$$f^a={\displaystyle \sum _M{f}_M^a}$$

(346)

and then sums the resultants calculated for each input part.

Sum Moment

Reports the resultant moments of the applied, body, internal, and constraint forces, acting on the selected input parts, with respect to a specified location $x_0$ . Simcenter STAR-CCM+ first calculates the resultants of the moments per input part, by summing all the moments at the part nodes, and then sums the moment resultants calculated for each input part.

For example, to calculate the Sum Moment of the Applied Force, Simcenter STAR-CCM+ calculates the resultant of the moment of the Applied Force for each input part, as:

$$m^a={\displaystyle \sum _M(x_M-x_0)}\times f_M^a$$

(347)

and then sums the resultants calculated for each input part.

Stopping Criteria

The Solid Stress Solver has additional Stopping Criteria based on the convergence of the displacement, force, contact constraint, contact pressure, and strain energy residuals. For this solver, Simcenter STAR-CCM+ automatically adds the Displacement and Force stopping criteria. You can add the Strain energy Criterion manually by activating the Strain energy property of the Solid Stress Solver.

For more information on the properties of the stopping criteria, see 基于监视器的属性.