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.
Incompressible Flow
The tutorials in this set illustrate various Simcenter STAR-CCM+ features for incompressible fluid flows as well as porosity and solution recording
Steady Flow: Backward Facing Step
Steady flow over a backward facing step is a typical scenario to investigate the behaviour of reattaching flows. Understanding the behaviour of the flow is crucial for many applications such as designing heat exhangers, evalutating aerodynamic performance and improving flow control strategies.
Setting Up Boundary Conditions
You specify the inflow of gas through the inlet boundary as a parabolic velocity profile as given by GUID-86673B4B-06A3-4351-B3A2-DB31AEFE92CE.html#GUID-86673B4B-06A3-4351-B3A2-DB31AEFE92CE__EQUATION-FIGURE_NQ2_ZXH_WXB. The velocity profile is formulated in terms of two parameters: the step height $H = 1 m$ and the maximum velocity $V_{\max} = 1 m / s$ .

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
  - Steady Flow: Lid-Driven Cavity Flow
    This tutorial demonstrates the performance of Simcenter STAR-CCM+ in solving a traditional square lid-driven cavity flow. The problem geometry consists of a two-dimensional 1 m² cavity. The cavity is covered by an impermeable wall that moves in the x-direction with constant velocity of 1 m/s. A stretched quadrilateral mesh with 6400 cells is used.
  - Steady Flow: Channel Flow with Multiple Meshes
    This tutorial describes a steady airflow simulation over an obstacle that is mounted at the bottom wall of a three-dimensional channel.
  - Steady Flow: Laminar and Turbulent Flow in an S-Bend
    This tutorial demonstrates the flow of an incompressible gas through an s-bend of constant diameter (2 cm), for both laminar and turbulent flow. The first part of the tutorial covers the laminar flow, with a Reynolds number (Re) of 500, and the second part covers the turbulent flow, Re = 50,000. The same pipe geometry is used in both cases.
  - Steady Flow: Backward Facing Step
    Steady flow over a backward facing step is a typical scenario to investigate the behaviour of reattaching flows. Understanding the behaviour of the flow is crucial for many applications such as designing heat exhangers, evalutating aerodynamic performance and improving flow control strategies.
    - Prerequisites
      The instructions in the Backward Facing Step tutorial assume that you are already familiar with certain techniques in Simcenter STAR-CCM+.
    - Creating the Backward Facing Step Geometry
      You define the geometry for the backward facing step in relation to a set parameter for the step height. This approach allows for easy scaling of the model later.
    - Setting Up and Generating the 2D Mesh
      Before you can generate a 2D mesh as part of an automated mesh pipeline, you must badge the part. Badging a part notifies Simcenter STAR-CCM+ that this part will be used to generate a 2D mesh. The requirement for this feature is that one separate surface must lie on the Z = 0 plane. In a previous section, you renamed the surface that lies on the Z = 0 plane to Surface for 2D Mesh, so in this case the requirement is met. A volume mesh is generated using trimmed cells. To make sure the y+ value calculated by the turbulence model is around 50, do not refine the mesh near the walls.
    - Selecting the Physics Models and Specifying the Material Properties
      You model the steady-state turbulent flow of a gas through the backward facing step using the Realizable K-Epsilon model in conjunction with the high y+ wall treatment.
    - Setting Up Boundary Conditions
      You specify the inflow of gas through the inlet boundary as a parabolic velocity profile as given by GUID-86673B4B-06A3-4351-B3A2-DB31AEFE92CE.html#GUID-86673B4B-06A3-4351-B3A2-DB31AEFE92CE__EQUATION-FIGURE_NQ2_ZXH_WXB. The velocity profile is formulated in terms of two parameters: the step height $H = 1 m$ and the maximum velocity $V_{\max} = 1 m / s$ .
    - Visualizing Velocity, Wall Shear Stress, and Nusselt Number
      You visualize the velocity distribution in the form of a line integral convolution plot. You plot the wall shear stress in the x direction and the Nusselt number along the Step Bottom wall boundary.
    - Running the Simulation
      You limit the number of iterations for the solver to 500; this is sufficient for the solution to converge.
    - Analyzing the Results
      After the simulation has finished running, you examine Vector Scene 1, and the Wall Shear Stress (x) and Nusselt Number plots.
    - Modifying the Step Height
      You double the step height and see how this change affects the flow.
    - Summary
      This tutorial demonstrated the flow of an incompressible fluid over a backward facing step.
  - Anisotropic Flow: Cyclone Separator
    The flow inside a cyclone separator is characterised by strong swirling motion and three-dimensional boundary layers. Properly accounting for these effects is a challenging problem for CFD simulations. This tutorial presents the initial step in setting up a coarse mesh cyclone flow simulation.
  - Porous Resistance: Isotropic Media
    This tutorial models flow through a catalyst geometry.
  - Porous Resistance: Orthotropic Media
    This tutorial solves the same problem as the Porous Resistance: Isotropic Media, except that the fluid in the porous region cannot flow in any direction other than the bulk flow (y-) direction.
  - Solution Recording and Playback: Vortex Shedding
    This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.
  - Generalized Newtonian Fluid: Flow in a Static Mixer
    This tutorial demonstrates the process of setting up and analyzing the flow of a viscous fluid through a static mixer.
  - Viscoelastic Flow: Basic Extrusion
    This tutorial illustrates the extrusion of molten rubber through a die.
  - Material Calibration: Curve Fitting Non-Newtonian Model Parameters
    This tutorial illustrates the workflow for calibrating rheological model parameters from experimental rheological data through curve-fitting.
  - Polymer Melt Extrusion: Film Casting
    In industry, film casting is a common process for producing thin polymeric films. Cast films are used for applications such as food and textile packaging, stretch wraps, or plastic bags. Simcenter STAR-CCM+ provides a combination of the Film Casting model and the Free Surface model that allows you to simulate that process and to investigate the impact of various parameters on the resulting film.
- 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 Up Boundary Conditions

You specify the inflow of gas through the inlet boundary as a parabolic velocity profile as given by Eqn. (5243). The velocity profile is formulated in terms of two parameters: the step height $H = 1 m$ and the maximum velocity $V_{\max} = 1 m / s$ .

You set the turbulent length scale at the inlet to 5% of the inlet width. To facilitate correct adaption when changing the step height, the turbulent length scale is parameterized as:

I = 0.05 * 4 * H

(5244)

To set up the boundary conditions:

Create a parameter to define the value of the maximum velocity:

Right-click the Automation > Parameters node and select New > Scalar.
Rename the new scalar parameter to Vmax.

Edit the Vmax node and set the following properties:


Property	Value
Value	1.0
Dimensions > Velocity	1

Create a field function to define the parabolic velocity profile:

Right-click the Automation > Field Functions node and select New > Scalar.
Rename the new node to Parabolic Profile.

Edit the Field Functions > Parabolic Profile node and set the following properties:


Property	Setting
Function Name	parabolicProfile
Dimensions	Velocity	1
Definition	`${Vmax}($${Position}[1]-${StepHeight})(5${StepHeight}-$${Position}[1])/(${StepHeight}${StepHeight})/4`

Define the inlet boundary using a parabolic velocity profile:

Edit the Regions > Backward Facing Step > Boundaries > Inlet > Physics Conditions > Turbulence Specification node and set the Method to Intensity + Length Scale.
Edit the Inlet > Physics Values > Turbulent Length Scale node and set Value to 0.05*${StepHeight}*4.

Edit the Inlet > Physics Values > Velocity Magnitude node and set the following properties:


Property	Setting
Method	Field Function
Scalar Function	Parabolic Profile

Set the heat flux on the bottom wall:
1. Edit the Boundaries > Step Bottom > Physics Conditions > Thermal Specification node and set Condition to Heat Flux.
2. Edit the Physics Values > Heat Flux node and set Value to 500 W/m^2
Save the simulation.