The follwing modelling strategy is used:

Figure 2 : Mesh structure for the combustion chamber model


    This sub-tutorial presents the basic model set-up. The various steps needed to create the mesh for the idealised combustor are described, including the creation of baflfe cells. The specification of boundary locations and conditions, material properties and control parameters are fully explained.


            We present the main commands to create a geometry
  1. In the NavCenter section of the window, select Create and Import Grids
  2. Select Create Grids and open the panel create 3-D Grids
    As we work in cylindrical coordinate, we can change the previous by select Coordinate System and choose in the scroll list.
To define the continium we select Cell Type , go to Cell Table Editor, Specified your choose(for this example we use Fluid)and confirmed
To define baffles in our mesh , we collect and display the cells :
  1. In the PROSTAR   I/O window , type command :Cset News Gran Xmin,Xmax,Ymin,Ymax,Zmin,Zmax
  2. To visualise click Cell Plot
To attach baffles to the appropriates cells:
  1. Select Tools>Cell Tool
  2. working from the Cell Tool,highlight Cell Type(baffle) in the scroll list and active it
  3. Choose Add Baffles>Surface and pick a vertex on the top surface of the mesh.
  4. In the Define Cset , select Add>Type(Current) and click Cell Plot to confirm that the baffles were created correctly
To create baffle holes :
  1. In the Cell Tool ,highlight Cell Type(baffle) in the scroll list and active it, after select New>Type(Current)
  2. Click Cell Plot
  3. In the main window, change the viewpoint to have the top of the geometry
  4. In the Cell Tool, select Delete Cells>Cursor Select and then mark the following cells with screen cursor
  5. Click Done
  6. Select a new cell set C>All and then click Cell plot
After terminated the first part we store the model data
  1. File>Save Model

This module can  specify the location and the properties of the model's

  1. In the main window choose the View> to display the region
  2. Choose the Boundary  Regions in scroll list, use the appropriate button(Pick Cell Faces, Select a Zone, Surface Based on Edges,Surface Based on Vset)  to pick the region
  3. Define the region Type by selecting the  correct boundary
  4. Repeat this operation for all surfaces
  1. File>Save Model

  This module can set up appropriate materials properties and  thermofluid models
  1. In the STARGUIde window, click the Thermophysical models and properties
  2. Select Liquids and Gases , go to Molecular Properties to define all kinds of properties
  3. Select Turbulence Models to specify the flow state
  4. Select Thermal Model ,  to input the the temperature equation
  5. Select Initialization to put the initial condition

  This module Check the current boundary condition definitions and specify boundary condition values where appropriate.We are going to presente in details how to put Cyclic condition
  1. Select Define Boundary  Conditions
  2. Click Define Boundary Regions to display the corresponding panel
  3. In the scroll list ,select the regions goto Tools>Boundary Tool>Other> Choose  the Cyclic Set List
  4. Click Integral Match to display the Cyclic Set Match dialog
  5. Enter cyclic region parameters in the appropriate text boxes, as shown below :
            Box Region #1-1
            Box Regions#2-2
            Box DY-(-60)
  1. Leave all others parameters at their default values , click Apply and then Close.This operation should create 200 cyclic pairs
  2. Close the Cyclic Set List dialog
  3. Close the Boundary Tool
To specify boundary conditions for the inlet boundaries, we choose the '"Mixing lengt" option as the input form for turbulence parameters. We can note that all fluid streams except the one flowing through the cooling passage have swirl  velocity components on entry into the combustor.In each box of inlet component we indicate the differentes values of velocities and turbulence model.

Before all calculous we have to write all files to run STAR(files tut.geom and tut.prob)

  1. In the main window ,choose File>Write Geometry File
  2. In the Geometry File Write dialog, click Apply
  3. File>Write Problem File
  4. In the Problem File Write dialog, click Apply and thnen Close
  5. File>Save Model
In this module we specify the number of ieration and  how to restart a calculous.
  1. Select Analysis Preparation/Running
  2. Go to Set Run Time (enter the number of iteration)
  3. And Click to Analysis (Re)Start ot restart a calculous