Home
Tutorials
Tutorials show you how to use Simcenter STAR-CCM+ for various applications in a step-by-step format with recommendations for setup, initialization and steps of the solution process specific to the application. Macro and simulation files are available for download for a large proportion of cases.
Introduction
Welcome to the Simcenter STAR-CCM+ introductory tutorial. In this tutorial, you explore the important concepts and workflow. Complete this tutorial before attempting any others.
Setting Boundary Conditions
Boundary conditions define the solved-for quantities—or how the solver is to treat them—around the perimeter of the computational domain. Here, you set boundary conditions for the inlet and wall boundaries.

Share

Link: copied

Breadcrumb: copied

Tutorials
Tutorials show you how to use Simcenter STAR-CCM+ for various applications in a step-by-step format with recommendations for setup, initialization and steps of the solution process specific to the application. Macro and simulation files are available for download for a large proportion of cases.
- Using Tutorial Macros and Files
  Macros, input files, and final simulation files for a range of tutorials are provided as an optional download package on the Support Center website. These macros and final simulation files are provided as an aid to the written tutorials, so that you can check your final results against the downloaded files, or against a simulation that is built and run using the macros.
- Introduction
  Welcome to the Simcenter STAR-CCM+ introductory tutorial. In this tutorial, you explore the important concepts and workflow. Complete this tutorial before attempting any others.
  - Starting a Simcenter STAR-CCM+ Simulation
    Simcenter STAR-CCM+ is a client-server application. That is, the interactive user interface is a client process that connects to a server process running on the same machine or on a remote machine. The server process hosts the simulation. Changes that you make through the user interface are transmitted immediately to the simulation held by the server process.
  - Importing the Geometry
    Simcenter STAR-CCM+ provides tools to generate the geometry, but for this tutorial you import a Parasolid file containing the design. The imported geometry represents the fluid volume around the body in the wind tunnel.
  - Defining Boundary Surfaces
    Before you convert geometry parts to regions, you are generally advised to identify and name part surfaces according to their final boundary conditions. You can split and combine part surfaces until you have the set of surfaces that best represent the boundary topology.
  - Assigning Parts to Regions
    Geometry parts are used to prepare the spatial representation of the model. The computational model to which physics can be applied is defined in terms of regions, boundaries, and interfaces. An important step in the setup procedure is when you assign parts to regions.
  - Setting Boundary Types
    The type of a boundary determines the default behavior for the prism layer mesher next to the boundary surface. For inflow and outflow boundary types, no prism layers are formed by the prism layer mesher. Therefore, setting the boundary types before you generate a mesh saves time during setup.
  - Generating the Volume Mesh
    After assigning geometry parts to regions, you can proceed to define and generate the volume mesh using mesh operations. Mesh operations are defined within the Geometry > Operations node.
  - Selecting the Physics Models
    A physics continuum defines a set of physics models and their associated material. You associate a physics continuum with one or more regions although you can also have dormant continua not associated with any region. Within a physics continuum, physics models collectively define the primary quantities that the simulation solves for during run-time.
  - Specifying the Initial Conditions for the Simulation
    Initial conditions in a continuum specify the initial field data for the simulation. Each model requires sufficient information so that the primary variables of the model are set to a sensible value throughout the computational domain at the start of the simulation.
  - Setting Boundary Conditions
    Boundary conditions define the solved-for quantities—or how the solver is to treat them—around the perimeter of the computational domain. Here, you set boundary conditions for the inlet and wall boundaries.
  - Visualizing the Solution
    Simcenter STAR-CCM+ allows you to create scenes before running the solvers. As these scenes are updated as the simulation progresses, you can obtain early indications of the result towards which the solution is converging. Here, you set up a scalar scene for visualizing the Mach number.
  - Monitoring the Drag Force Coefficient
    To help in assessing convergence, Simcenter STAR-CCM+ allows you to define and monitor integral quantities of interest while the solution develops. Here, you define a report for the drag force coefficient, and subsequently create a monitor and plot from the report.
  - Setting Stopping Criteria
    Set the appropriate stopping criteria for the simulation.
  - Running the Simulation
    Preparation of the simulation is now complete, and the simulation can be run.
  - Visualizing the Results
    At the end of the calculation, the Residuals display show most of the residuals flattening out, which is a good indicator of convergence. The force coefficient plot also confirms this state. You can now review the results of the simulation using the scalar scene that you prepared earlier.
  - Summary
    This tutorial has introduced the following Simcenter STAR-CCM+ features:
- Foundation Tutorials
  The foundation tutorials showcase the major features of Simcenter STAR-CCM+ in a series of short tutorials.
- Geometry
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for creating and working with parts and 3D-CAD.
- Mesh
  The tutorials in this set illustrate various STAR-CCM+ features for building CFD meshes.
- Incompressible Flow
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for incompressible fluid flows as well as porosity and solution recording
- Compressible Flow
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for compressible fluid flows as well as harmonic balance.
- Heat Transfer and Radiation
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for heat transfer, radiation, and thermal comfort.
- Multiphase Flow
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for simulating multiphase fluid flow problems
- Discrete Element Method
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for simulating Discrete Element Method problems
- Motion
  The tutorials in this set illustrate various STAR-CCM+ features for simulating problems with moving geometries and meshes, dynamic fluid body interaction, and rigid body motion:
- Reacting Flow
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for simulating reacting flows such as combustion.
- Solid Stress
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for computing deformation, strain, and stresses in solid regions. They also show how such computations can be coupled to the fluid behavior in an analysis of fluid-structure interaction.
- Aeroacoustics
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for solving aeroacoustic simulations.
- Electromagnetism
  The following tutorials illustrate features for solving problems that involve electromagnetic fields.
- Electrochemistry
  The following tutorial demonstrates chemical reactions induced by an electrical current.
- Battery
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for setting up a battery model:
- Automation
  The tutorials in this set illustrate various Simcenter STAR-CCM+ automation and macro features.
- Design Exploration
  The tutorials in this set illustrate various features for running design exploration studies in Design Manager.
- Coupling with CAE Codes
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for coupling with CAE codes:
- Analysis Methods
  The tutorials in this set illustrate various Simcenter STAR-CCM+ features for analysing and visualizing simulation data.
- Simcenter STAR-CCM+ In-cylinder
  The tutorials in this set illustrate features for simulating internal combustion engines in Simcenter STAR-CCM+ using the dedicated add-on Simcenter STAR-CCM+ In-cylinder.

Setting Boundary Conditions

Boundary conditions define the solved-for quantities—or how the solver is to treat them—around the perimeter of the computational domain. Here, you set boundary conditions for the inlet and wall boundaries.

To achieve a Mach number of approximately 0.75 at the inlet, isentropic relations were used to determine the inlet total pressure and outlet static pressure for a given total temperature. For an outlet static pressure equal to one atmosphere (absolute) and a static temperature of 300 K, the inlet total pressure is 164,904 Pa (absolute). The inlet total temperature is 344.8 K.

The boundary values are specified as gauge pressures. Therefore, using the default reference pressure of 101,325 Pa (one atmosphere),you set the inlet total pressure to 63,579 Pa (gauge). The outlet static pressure is 0 Pa (gauge), the default value.

To set the inlet condition:

Expand the Regions > subdomain-1 > Boundaries node.
Expand the Inlet > Physics Values node, and select the Total Pressure node.
Set Value to 63579 Pa.

The total pressure setting is relative to the operating pressure value of 101,325 Pa. A supersonic static pressure is also required as part of a stagnation inlet condition but is only used if the inlet velocity becomes supersonic at some instance during solution iteration. The default value of 0.0 Pa relative pressure is sufficient as long as supersonic flow does not occur.

Within the same Physics Values node, select the Total Temperature node and set Value to 344.8 K.

To simulate the body in a wind tunnel, the upper boundary is set to a slip wall, thus avoiding the need to resolve the boundary layer on this wall.

To set the slip wall condition:
1. Select the Slip_wall > Physics Conditions > Shear Stress Specification node.
2. Set Method to Slip.

Default turbulence settings are acceptable for this tutorial. Also, as no backflow is expected through the pressure outlet, default settings are again acceptable.