The premise of increasing the stiffness near small mesh volumes is that mesh quality will benefit from having larger control volumes absorb more mesh motion. This option is desirable because it does not require the solution of additional equations (as for boundary dependent options). However, its behavior does depend on the initial mesh distribution (for example, having a fine mesh in regions where the motion is likely to be most significant).

The following relationship is used to determine the mesh stiffness, , applied in the displacement diffusion equation:

(1–2)

This relationship provides an exponential increase in the mesh stiffness as the control volume size, , decreases. The stiffness Model Exponent, , determines how quickly this increase occurs. For example, large values will yield a much more abrupt stiffness variation. This exponent is set to 2.0 by default. is the reference volume, which can be automatically computed (Reference Volume > Option set to Mean Control Volume) or directly specified (Reference Volume > Option set to Value, with a default value of 1 [m^3]). The reference volume should be representative of a typical control volume within the domain. Stiffness values are clipped between minimum and maximum values that are by default 1e-15 and 1e15, respectively.

When using Increase Near Small Volumes combined with Displacement Relative To set to Initial Mesh, then control volume size, , is computed using the initial mesh in Equation 1–2.

The premise of increasing the stiffness near certain boundaries (wall, inlet, outlet, and opening) is that mesh quality will benefit from having the mesh interior (that is, away from wall, inlet, outlet, and opening boundaries) absorb more mesh motion. Although this option requires the solution of an additional boundary scale equation, it is useful because it does not depend upon the original mesh distribution (that is, control volume size distribution) and it treats regions near all wall, interface, inlet, outlet, and opening boundaries identically. However, the mesh stiffness is unaffected near symmetry and one-to-one periodic interfaces.

The following relationship is used to determine the mesh stiffness, , applied in the displacement diffusion equation:

(1–3)

This relationship provides an exponential increase in the mesh stiffness as the distance from the nearest boundary, , decreases. The stiffness Model Exponent, , determines how quickly this increase occurs. For example, large values will yield a much more abrupt stiffness variation. This exponent is set to 2 by default. is the reference length, which can be automatically computed (Reference Distance > Option set to Global Length Scale) or directly specified (Reference Distance > Option set to Value, with a default value of 1 [m]). The reference length should be representative of a typical length within the model. Stiffness values are clipped between minimum and maximum values that are by default 1e-15 and 1e15, respectively.

Detailed information on the boundary scale equation is available at Wall and Boundary Distance Formulation in the CFX-Solver Theory Guide.

This option provides a more general model that adapts itself to cases, reducing the need for tuning. It combines features of Increase Near Small Volumes and Increase Near Boundaries and makes use of information about the local domain mesh.

The model has the following form:

(1–4)

Here, and are the local values as before, but the reference values are instead found from the properties of the local domain mesh. For example:

= mean control volume in domain

= 0.5 * (volume of domain)^1/3

= 10.0 * (minimum control volume in domain)^1/3

The factors and are simple default weights that indicate a dominance of one term over the other, or equality, and should sum to unity.

The mesh stiffness can also be specified directly using the CEL. As suggested above, the mesh stiffness should increase in regions where mesh folding is most likely to occur. For example:

This option is similar to Unspecified because no constraints on mesh motion are applied to nodes. The important difference is that motion of nodes in all domains adjacent to the interface influence, and are influenced by, the motion of the nodes on the interface.

No constraints on mesh motion are applied to nodes. Their motion is determined by the motion set on other regions of the mesh. When this option is used on a domain interface boundary condition, only motion from other nodes in the current domain is "felt". It is worth noting that this motion will enable the mesh on one side of a domain interface to pull away from the mesh on the other side of the interface.

Nodes are not permitted to move relative to the local boundary frame.

Nodes are displaced according to the specified CEL expression or User CEL. This displacement is always relative to the initial mesh and the local coordinate frame, if defined.

The following displacement options exist:

All nodes are located according to the specified CEL expression or User CEL.

The Periodic Displacement option allows you to set a transient periodic mesh motion that repeats itself at a given frequency and has an associated phase offset.

The periodic mesh displacement input vector components can be specified as:

For all of the above options, you need to provide the vibration Frequency as well as a Phase Angle that offsets the displacement in time. The following Phase Angle options are available:

The Parallel to Boundary option allows the mesh to slide over an arbitrary boundary definition, with no component of deformation normal to it. This option attempts to preserve the geometry of the boundary as defined by its initial mesh.

The Surface of Revolution option allows the mesh to slide over a boundary definition while maintaining the radial profile defined by the initial boundary mesh, and the axis of revolution.

For the Surface of Revolution option you can specify the Axis Definition either as a Coordinate Axis of an existing coordinate frame, or a local cylindrical axis defined by Two Points.

Nodes are displaced according to the displacement data received from the System Coupling system. For more information about simulations involving System Coupling and CFX, refer to Coupling CFX to an External Solver: System Coupling Simulations in the CFX-Solver Modeling Guide.

Set Rigid Body to the name of the rigid body object that will govern the motion of the boundary/subdomain.

You can restrict which aspects of the rigid body motion are applied to the boundary/subdomain by selecting Motion Constraints and choosing one of the following options:

For additional information on modeling rigid bodies, see Rigid Body Modeling in the CFX-Solver Modeling Guide.

If we limit the class of relevant solutions to cases similar to blade flutter calculations, for example, then the imposed displacements at a boundary are of the form:

(1–6)

If we assume that all displacements satisfy Equation 1–5, and that all prescribed boundary conditions are either stationary or of the form in Equation 1–6, then it can be shown that the solution of the mesh displacement equations can be found in frequency space, rather than the time-domain. Posed as a complex number problem we find:

(1–7)

With boundary conditions:

where represents the phase angle at each boundary/blade, and the prescribed amplitude of oscillation. By using a separation of variables, we can solve directly for the real and imaginary parts, subject to known boundary conditions:

(1–8)

And the periodic solution at any point in time is reconstructed from:

(1–9)

The big advantage with this approach is that the equations in Equation 1–8 can be solved to convergence right at the start of the simulation before any other equation systems (Note that in 3D simulations, R and A are essentially vectors but the 3 components of R can be solved independently with 3 Laplacian equations). Once the solution is found, Equation 1–9 is used on all time steps. Note that Equation 1–9 represents a linear system, which is why the mesh vertices only travel in straight lines.