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.
Aeroacoustics
The tutorials in this set illustrate various Simcenter STAR-CCM+ features for solving aeroacoustic simulations.
Sponge Layer Modeling: Simplified Tailpipe
Unsteady aeroacoustics simulations require effective non-reflective boundary conditions to prevent spurious reflected acoustic waves from the boundaries of the computational domain interfering with the aeroacoustic results.
Setting Up the Solvers and Running the Simulation
You run the simulation for a physical time of 0.4 s. The iterations per time-step stop when the relative change in residuals of the continuity equation is less than 2% or the maximum number of inner iterations of 15 is reached. To enhance the accuracy of the simulation, you set the temporal discretization of the implicit unsteady solver as well as those of the continuity equation and the energy equation to a second-order scheme. To speed up convergence per time-step, you increase the under-relaxation factors from their defaults.

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.
- 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.
  - Broadband Models: Noise from a Cylinder (Preparation)
    This tutorial demonstrates how to set up aeroacoustics problems in Simcenter STAR-CCM+. The flow around a cylinder is used in the simulation to describe the required steps.
  - DES and FW-H On-The-Fly: Noise from a Cylinder (Unsteady Analysis)
    In the previous section of this tutorial, you completed the steady-state analysis runs for qualifying the volume mesh. In this section, continuing from the previous simulation file, you set up the final transient run for an unsteady analysis of the near field and an FW-H analysis of the far field.
  - Ffowcs Williams-Hawkings: Sound Propagation
    This tutorial compares the Post FW-H model with the FW-H On-The-Fly model.
  - Signal Post-Processing: FFT and Wavenumber
    Several further analyses are possible using the simulation history file from the earlier tutorial, DES and FW-H On-The-Fly: Noise from a Cylinder (Unsteady Analysis). These analyses are covered in this tutorial.
  - Acoustic Wave Modeling: Noise from a Cylinder
    This tutorial demonstrates how to set up an acoustic wave simulation in Simcenter STAR-CCM+. The flow around a cylinder is used in the simulation to describe the required steps.
  - Lighthill Wave and Perturbed Convective Wave Modeling: Simplified HVAC Duct
    Noise generated by the air handling components in heating, ventilation, and air conditioning (HVAC) systems is a large contributor to interior cabin sound levels. Investigating the sources of noise and modifying the design accordingly, leads to better and quieter systems.
  - Sponge Layer Modeling: Simplified Tailpipe
    Unsteady aeroacoustics simulations require effective non-reflective boundary conditions to prevent spurious reflected acoustic waves from the boundaries of the computational domain interfering with the aeroacoustic results.
    - Prerequisites
      The instructions in the Sponge Layer Modeling: Simplified Tailpipe tutorial assume that you are already familiar with certain techniques in Simcenter STAR-CCM+.
    - Loading the Starting Simulation File
      For this tutorial, you are provided with an input file that contains the mesh around the pipe bounded by the spherical pressure outlet boundary.
    - Selecting the Physics Models
      You set up an LES physics continuum for an ideal gas including the Sponge Layer model.
    - Setting the Inlet and Outlet Boundary Conditions
      At the inlet boundary of the tailpipe, you set a mass flow rate of 15 kg/s and a total temperature of 700 K. Reflections of acoustic disturbances emerging from the tailpipe need to be damped only next to the pressure outlet boundary that confines the computational domain. For this boundary, you enable fluctuation damping using a sponge layer.
    - Preparing the Scenes for Visualization
      Here, you create a user-defined field function that calculates the pressure fluctuations. You visualize the calculated field on a pre-defined plane section that cuts through the origin. You write the pressure fluctuations scene to image files after each time-step. Additionally, you create a scene that displays the sponge layer damping coefficient on the plane section.
    - Setting Up the Solvers and Running the Simulation
      You run the simulation for a physical time of 0.4 s. The iterations per time-step stop when the relative change in residuals of the continuity equation is less than 2% or the maximum number of inner iterations of 15 is reached. To enhance the accuracy of the simulation, you set the temporal discretization of the implicit unsteady solver as well as those of the continuity equation and the energy equation to a second-order scheme. To speed up convergence per time-step, you increase the under-relaxation factors from their defaults.
    - Analyzing the Results
      When the simulation is complete, you analyze the results. At the point probe, you compare the pressure and sound pressure levels with the provided data from the simulation without using the Sponge Layer model.
- 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 Up the Solvers and Running the Simulation

You run the simulation for a physical time of 0.4 s. The iterations per time-step stop when the relative change in residuals of the continuity equation is less than 2% or the maximum number of inner iterations of 15 is reached. To enhance the accuracy of the simulation, you set the temporal discretization of the implicit unsteady solver as well as those of the continuity equation and the energy equation to a second-order scheme. To speed up convergence per time-step, you increase the under-relaxation factors from their defaults.

For the time-step size, you set up the following step function:

Δ t = {\begin{matrix} 10^{- 3} & ; & if t < 0.1 s \\ 5 \times 10^{- 4} & ; & if 0.1 \leq t < 0.15 s \\ 10^{- 4} & ; & if t \geq 0.15 s \end{matrix}

To set up the solvers and run the simulation:

Select the Solvers > Implicit Unsteady node and set the following properties:


Property	Setting
Time-Step	$Time < 0.10 ? 1e-3 : ($Time <0.15 ? 5e-4 : 1e-4)
Temporal Discretization	2nd-order

Right-click the Solvers > Implicit Unsteady > Stopping Criteria node and select New Monitor Criterion....
In the Select Monitor dialog, select Continuity.
Select the Stopping Criteria > Continuity Criterion node and set Criterion Option to Relative Change.
Select the Continuity Criterion > Relative Change node and set Relative Change to 0.02.

Edit the Solvers node and set the following properties:


Node	Property	Setting
Segregated Flow
Velocity	Under-Relaxation Factor	0.9
Pressure	Under-Relaxation Factor	0.7
High-Accuracy Temporal Discretization	Option	Optimized 2nd-order (5)
Segregated Energy	Enable High-Accuracy Temporal Discretization	On
High-Accuracy Temporal Discretization	Option	Optimized 2nd-order (5)

Edit the Stopping Criteria node and set the following properties:


Node	Property	Setting
Maximum Inner Iterations	Maximum Inner Iterations	15
Maximum Physical Time	Maximum Physical Time	0.4 s
Maximum Steps	Enabled	Off

Select the Monitors > Pressure Monitor node and set Trigger to Time Step.
Click (Run) to run the simulation.
When the simulation is complete, save it.