I.  3-D flow in a partially blocked elbow.

1.1- Physical problem description

The problem geometry is shown in the two next figures. Air at standart pressure and temperature (293 K) enters the channel at the velocity of 10 m/s (Reynolds number = 16910). the fluid, having passed a blockage and a 90 degree elbow, exits vertically through the outlet. Its properties are as
follows :

 density (kg/m3) Molecular viscosity (Pa.s) Specific heat (J/Kg.K) Thermal conductivity (W/m.K) 1.205 1.81 E-5 1006.0 2.637 E-2

1.2- Modelling strategy

The following modelling strategy is used :

• combination of cartesian and cylindrical coordinate systems with uniformly spaced square cells.
• mesh generation based on a multi-block technique.
• inlet, outlet and wall boundariy regions.
• incompressible and steady flow options.
• appropriate physical parameters for the fluid.
• k-eps turbulence model for the turbulence characteristics.

1.3-Mesh generation based on a multi-block technique

Given that there are no geometric complexities, we use one of Prostar's automatic meshing facilities to create the basic grid. The stategy choosen here is to divide the geometry into three sections. The appropriate STAR GUIde panel is then applied to each section in turn to create three subsets of the final mesh. These are finally coupled together to create a mesh covering the entire model. We use the option "Assemble grid " to remove the discontinuities and to merge all the vertices. The following graph shows the geometry and the first mesh :

The mesh is now complete. however, the flow obstruction still needs to be created. this is done simply by deleting the cells occupying the volume corresponding to the obstruction. The definitive mesh is shown on the next picture :

At this point, it is prudent to check the quality of the mesh. PROSTAR provides a number of automated tools that streamline this process. the check tool is accessed by clicking on folder " Check and fix grid "  in the Navigation Centre.

1.3-Boundary conditions

Specification of boundary conditions involves the use of two panels. The first one, "Create Boundaries", enables the boundary regions to be positioned within the model. The second, "Define Boundary Regions", is used to specified the properties of the regions. In this case, there are three boundary regions : an inlet, an outlet and a wall. PROSTAR  automatically assumes that any external surfaces that have not been specified by the user
belong to Region 0 and, by default, Region 0 is a no-slip, adiabatic wall. Therefore, wall boundaries do not have to be specifically identified in this particular problem. For the other two boundary types, we assign a region number to the inlet and outlet regions.
Now that the boundary regions have been physically located, we have to define the particular properties of each region by using in the main PROSTAR window, the folder "Define boundary conditions". the values we have entered are display on the three following figures :

Inlet boundary region settings                                                                            Wall boundary region settings                                                                     Outlet boundary region settings

The model building process is now complete. The next step is to do a final comprehensive check for any errors or inconsistencies before setting up the CFD analysis run by clicking on the folder "Check Model Setup".

1.2-Computing and results

We have studied the case of an incompressible and steady flow with a k-epsilon turbulent model for the turbulence characteristics. Air at pressure
standart and temperature (293 K) enters the channel at velocity of 10 m/s (Re = 16910).
In this section, we plot 3D surface, 2D surface and particles tracks using the folder "Post Processing". Here are our results :

 Dissipation  -  z=0 Dissipation  -  z=0.25 Dissipation  -  z=0.5 Dissipation  -  z=0.75 Dissipation  -  z=0.95 Turbulent energy  -  z=0 Turbulent energy  -  z=0.25 Turbulent energy  -  z=0.5 Turbulent energy  -  z=0.75 Turbulent energy  -  z=0.95

Here are some steps for creating a particle track (file tut.pst) :

• Select the initialisation tab.