Defining Physics Workflow

Simcenter STAR-CCM+ contains a wide range of physics models and methods for the simulation of single- and multi-phase fluid flow, heat transfer, turbulence, solid stress, dynamic fluid body interaction, aeroacoustics, and related phenomena. These physics models are all selected using a physics continuum.

Although you can create and define physics continua without having any regions or volume mesh present, you must have both in order to run a simulation.

To create physics continua and define supporting objects:

Create one physics continuum for each material or material mixture that you require in the simulation. If you have multiple adjacent solid parts, you can use the multi-part solid model to define multiple solid materials in the same continuum. To create a physics continuum:
1. Right-click the Continua node and select New > Physics Continuum
The new continuum receives the next logical sequential name such as Physics 2 but can be renamed if necessary. Manager nodes for Models, Reference Values, and Initial Conditions are added as child nodes to the new continuum node. Once the new physics continuum has been created, you can proceed to select the physics models for it.

Note If you import a mesh into the simulation, Simcenter STAR-CCM+ automatically adds a physics continuum for you.
Choose the physics models and materials. For each physics continuum:
1. Right-click the Continua > [physics continuum] > Models node and click Select Models....
2. In the Physics Model Selection dialog, for each group of choices on the left-hand side, choose a model. Some groups require a choice, indicated by <Select One>. Other groups present optional choices.
  By default, the option Auto-select recommended models is active. When this option is active, Simcenter STAR-CCM+ selects default models for some groups in the dialog. For example, if you select the K-Epsilon Turbulence option from the Turbulence group, Simcenter STAR-CCM+ automatically chooses the Realizable Two-Layer K-Epsilon model.
3. If Simcenter STAR-CCM+ makes an automatic selection that you wish to change:
  1. Deactivate Auto-select recommended models.
  2. Within Enabled Physics Models, deactivate unwanted selections until you return to the earlier state.
  3. Choose the correct sequence of models.
For multiphase flow simulations, and for single-phase flow simulations that use phase models (for example, porous media), you can create the necessary phases and select the appropriate models for each. For multiphase flow simulations, you can also define the necessary phase interactions.

For more information, see Using the Physics Model Selection Dialog.
Assign a physics continuum to each region in the simulation. To do this, for each region, either:
- select the Regions > [region] node and set Physics Continuum, or
- drag the physics continuum object onto the region node.
Region nodes update their icon according to whether the region is assigned to a solid or fluid continuum.
Complete the setup for materials and physics models.
The actual steps you must follow varies depending on the physics models that you choose. Other parts of the user guide provide detail on specific models.
Model settings, once made, are retained if models are deselected and are still available if the model is reselected.
To return model settings to their default values, right-click the model and select Restore Default Settings from the menu. This function is not available for models that have phase models under them.
Define any required global parameters and user field functions.
If you wish to use the same input value (scalar or vector quantity) in more than one location in a simulation, you can set the value using a global parameter or a user-defined field function, and access this where required. Global parameters define constant quantities, whereas field functions can depend on space and time. For details, see Global Parameters and Creating a User Field Function.
For each physics continuum, set reference values.
For each physics continuum, set initial conditions:
1. Expand the Continua > [physics continuum] > Initial Conditions node.
2. Select the child nodes in turn and set the Method and Value properties appropriately.
For each region in the simulation, set any quantities that act on the region as a whole:
1. Expand Regions > Physics Conditions, select each child node, and set options appropriately. Some nodes, such as the Initial Condition Option, allow you to override continuum values at the region level.
2. If you have multiple parts within the region, decide whether you want to set values for the whole region, or for subgroups of parts within the region.
  - To set values on subgroups of parts, select the [region] node and activate Allow Per-Part Values.
3. Within [region] > Physics Values, select each node and set values according to the real scenario you are modeling.
  - To set values on subgroups of parts, select the value node and set Method to By Part Subgroup. Then select the child nodes within By Part Subgroup and set the Method and Value properties for the parts within the subgroup.
  Simcenter STAR-CCM+ provides several methods for specifying scalar and vector input values. The most common methods are:
  - Constant, which allows you to specify a scalar or vector input that does not depend on space, although it can depend on time.
  - Field Function, which allows you to use an existing field function as input. Field functions can be both space-dependent and time-dependent.
  For more information, see Conditions, Values, and Profiles.
4. If you wish to add motion to a region, review the information provide on motion objects.
Define boundary conditions for each region. Within a region:
1. Expand the Boundaries > [boundary] > Physics Conditions node and its corresponding Physics Values node.
2. Review each condition. Choose methods or options that suit the data that you have for that boundary. As you modify conditions, Simcenter STAR-CCM+ adds or removes nodes within the [boundary] > Physics Values manager node.
3. If you have multiple part surfaces within the boundary, decide whether you want to set values for the whole boundary, or for subgroups of part surfaces within the boundary.
  - To set values on subgroups of part surfaces, select the [boundary] node and activate Allow Per-Surface Values.
4. Within [boundary] > Physics Values, select each node and set values that match the real scenario that you are modeling.
  - To set values on subgroups of part surfaces, select the value node and set Method to By Surface Subgroup. Then select the child nodes within By Surface Subgroup and set the Method and Value properties for the part surfaces within the subgroup.
  Similarly to region values, you can set boundary values using several methods, such as the Constant method for spatially-invariant inputs, and the more generic Field Function method, which allows for space-dependent inputs. See Conditions, Values, and Profiles.
Define interface conditions. This procedure requires similar steps to those for boundary conditions:
1. Expand the Interfaces > [interface] > Physics Conditions node and its corresponding Physics Values node (if present).
2. Review each condition. If you choose an option that requires a value,Simcenter STAR-CCM+ adds the node within the Physics Value node for the interface.
3. If the interface is based on part surfaces, and has multiple parts assigned to it, you can choose to set values for the whole interface, or for subgroups of part contacts within the interface.
  - To set values on subgroups of part contacts, select the [interface] node and activate Allow Per-Contact Values.
4. Within [interface] > Physics Values, select each node and set values that give you the behavior you require.
  - To set values on subgroups of part contacts, select the value node and set Method to By Contact Subgroup. Then select the child nodes within By Contact Subgroup and set the Method and Value properties for the part contacts within the subgroup.
Many physics models expose specific solvers that control the solution of the model equations. Expand the Solvers node and review the properties provided for each solver.
For models that solve transport equations using the finite-volume method, the Under-relaxation Factor is often a property that you can adjust to reduce solution times. However, you must make sure that transport equations are adequately converged by the end of the simulation.