Set Up Volume and Surface Parameters

The volumetric parameters such as Material Model, Body Force and Mesh Motion are defined in the Global Tree.

Volume Parameters

These parameters are assigned to the appropriate volumes using Volume Parameters in the Model Tree. These parameters can be accessed by clicking Model > Volumes. The volume parameters are categorized into three parts, namely Element Set, Element Output and Volume Mesh Attributes.

Element Set

This command defines a set of elements for the given volume in the problem. All elements in the volume have same material model, body force, and so on. Element set defines the following parameters.
Medium
This parameter specifies whether the volume is of type Fluid, Solid, Thermal Shell or None.
A fluid element set solves for all equations specified in the Auto Solution Strategy. A solid or Thermal Shell type element set solves only the temperature and mesh displacement equations, while all other equations such as flow, turbulence and species are ignored. A type of none effectively deactivates the element set and all of its surfaces, the elements do not contribute to any equation. The nodes may still be moved through the use of the Mesh Motion parameter.
This parameter defines the quadrature rule used to integrate element contributions.
The actual quadrature rule used depends on the element shape.
Full Reduced Nodal Higher Order 1 Higher Order 2
Four node tet 4-point 1-point 4-point nodal 4-point nodal 20-point
Five node pyramid 5-point 1-point 5-point nodal 13-point 13-point
Six node wedge 3x2 1-point 6-point nodal 6x3 7x4
Eight node brick 2x2x2 2x2x2 8-point nodal 3x3x3 4x4x4
10 node tet 8-point 4-point 10-point nodal 20-point 35-point
All of the points in quadrature rules except for nodal satisfy the following properties:
• Are inside the elements
• Have positive weights
• Are node order independent
• Use minimal number of points for a given integration order
Appropriate surface and edge quadrature rules corresponding to these interior rules are used automatically for those surface and edges associated with a given element set.
Material Model
This parameter assigns the material properties using the Material models defined in Global section. Only those models defined in the Material Model section in Global are applicable for this parameter.
Reference Frame
This parameter specifies frame of reference for the volume. Only those reference frames defined in Reference Frame section in Global are applicable for this parameter.
Residual Control
Residual control provides stabilization of the equations by adding additional diffusion in areas where unresolved gradients are present. This option improves the robustness of the solver and should be left on.
Oscillation control
Oscillation control triggers the use of an operator that is designed to prevent over/under shoot of scalar equations. This option improves the accuracy and robustness of the solution and should be left on.
Mesh Motion
This parameter specifies the type of mesh motion to be imposed on the element set. Only those Mesh Motion models defined in Mesh Motion section in Global are applicable for this parameter.
Mesh Motion Precedence
This parameter specifies precedence of the mesh motion command above, in case of conflict from other commands. The higher the precedence value the higher the priority. It is active only when the Mesh Motion parameter is set to a mesh motion model.
Mesh distortion correction factor
This parameter determines if correction needs to be applied to the element jacobian for highly distorted elements.
Mesh distortion tolerance
Amount of correction for highly distorted elements.

Element Output

This command specifies parameters for the output of the average of quantities integrated through the volume. This command then outputs the averaged quantities to the disk. By default, AcuSolve writes out this output at the last time step of the simulation.
Time step frequency
This parameter specifies time step frequency at which to output averaged element quantities. If zero, this option is ignored.
Time frequency
This parameter specifies time frequency at which to output averaged element quantities. If zero, this option is ignored.
Number of user-defined quantities
Apart from the average of standard quantities such as pressure, temperature and velocity you can also define specific quantities for output. This parameter specifies a number of such user-defined quantities to be defined. If zero, this option is ignored.
User function name
This parameter specifies the name of the user defined function that returns user defined quantities. This option is active only when Number of user-defined quantities is greater than zero.
User function values
This parameter specifies the array of values to be passed to the user-defined function. This option is active only when Number of user-defined quantities is greater than zero.
User function strings
This parameter specifies array of strings to be passed to the user-defined function. This option is active only when Number of user-defined quantities is greater than zero.

Surface Parameters

Surface parameters specify the boundary conditions pertaining to the surface.

Simple Boundary Condition

This section defines the preliminary boundary conditions for the surface.
Type
Specifies the type of boundary condition for the surface.
Active type
Determines which surfaces in this surface set will have boundary conditions imposed by this command.
All: All surfaces in this set are active.
None: No Surface in this set is active.
No interface: Only surfaces that are not in an interface surface set or do not find a contact surface of an appropriate medium are active.
Precedence
Sets the priority for this boundary condition.
Surface tension model
Specifies the surface tension model to be used for boundary condition type free surfaces. Only those models defined in the Surface Tension Model section in Global are applicable for this parameter.
Contact angle model
Specifies the contact angle model to be used for the boundary condition type free surface. Only those models defined in the Contact Angle Model section in Global are applicable for this parameter. If set to none, the contact angle defaults to 90 degrees.
Pressure
Specifies the value of pressure on the surface. It is used for Outflow, Far-Field, Free Surface and Inflow with pressure type boundary conditions.
Pressure loss factor
Pressure loss at the Inflow, Outflow and Far Field surfaces can be modeled using this parameter. The following term is added to the pressure element boundary condition. (1)
Where =-1 for inflow and =1 for outflow.
Back flow Conditions
Specifies whether to specify nodal boundary conditions for scalar variables on nodes on outflow surfaces where there is flow into the fluid domain. This parameter is active only for Outflow and Far-Field boundary types.
Temperature back flow type
TSpecifies how the temperature condition is defined under back flow condition. Options for this parameter are shown below.
• Value: Specifies a value for temperature.
• Area Average: Average of solution over entire outflow surface.
• Exiting Area Average: Area average of solution over subset of outflow surface that has flow exiting the domain.
• Bulk: Bulk average of solution over entire outflow surface.
• Exiting Bulk: Bulk average of solution over subset of outflow surface that has flow exiting the domain.
Eddy frequency back flow type
Specifies how the turbulence eddy frequency condition is defined under back flow condition. Various options for this parameter are shown below.
• Value: Specifies a constant value for eddy frequency.
• Area Average: Average of solution over entire outflow surface.
• Exiting Area Average: Area average of solution over subset of outflow surface that has flow exiting the domain.
• Mass Flux Average: Mass flux average of solution over the entire outflow domain.
• Exiting Mass Flux Average: Mass flux average of solution over subset of outflow surface that has flow exiting the domain.
Kinetic energy back flow type
Specifies how the turbulent Kinetic energy condition is defined under back flow condition. It has the options similar to the eddy frequency back flow type.
Eddy viscosity back flow type
Specifies how the turbulent eddy viscosity condition is defined under back flow condition. It has the options similar to the eddy frequency back flow type.
Species 1 back flow type
Specifies how the back flow condition is defined for Species 1. It has the options similar to the eddy frequency back flow type.
Mesh displacement BC type
Specifies the type of mesh displacement on the wall. This option is not available for Free surface type. The following options are available.
• None: No mesh boundary condition. Mesh is free to move based on other boundary conditions.
• Fixed: Mesh fixed to the wall.
• Slip: Mesh slips tangentially along the wall. Note that the wall must be planar for slip mesh boundary conditions.
• Flexible body: Mesh follows a flexible body. Requires definition of Flexible Body under Global.
• Guide surface: Mesh follows a guide surface. Requires definition of Guide Surface.
Flexible Body
Specifies the name of Flexible Body. It is active only with Flexible Body mesh displacement type.
Nodal x modes
Specifies the array of node number and x-component Eigen vector values. It is active only with Flexible Body mesh displacement type.
Nodal y modes
Specifies the array of node number and y-component Eigen vector values. It is active only with Flexible Body mesh displacement type.
Nodal z modes
Specifies the array of node number and z-component Eigen vector values. It is active only with Flexible Body mesh displacement type.
Guide Surface
This parameter specifies name of the Guide Surface for the mesh to follow. It is used only when mesh displacement boundary condition type is Guide Surface.
Mesh Motion
This parameter gives the name of the Mesh motion for determining mesh displacement boundary conditions. If None this parameter has no effect. This feature is used with Fixed and‘Flexible Body mesh displacement types.

Surface Output

This command specifies parameters for the output of the average of quantities integrated through the surface. This command then outputs the averaged quantities to disk. By default, AcuSolve writes out this output at the last time step of the simulation.
Integrated time step frequency
Specifies time step frequency at which to output integrated surface quantities. If zero this option is ignored.
Integrated time frequency
specifies time frequency at which to output integrated surface quantities. If zero this option is ignored.
Statistics Output frequency
specifies time step frequency at which to output statistics of surface nodal quantities. If zero this option is ignored.
Statistics time frequency
specifies time frequency at which to output statistics of surface nodal quantities. If zero this option is ignored.
Nodal time step frequency
specifies time step frequency at which to output surface quantities at the nodes of the surface. If zero this option is ignored.
Nodal time frequency
Specifies time frequency at which to output surface quantities at the nodes of the surface. If zero this option is ignored.
Number of saved states
Specifies the number of solution steps to retain on disk. If zero all solution time steps are retained.