1. Problem Definition and Grid
  2. Starting the GUI
  3. Loading PreProcessing
  4. Checking PreProcessing and Saving Information
  5. Solving
  6. Visualizing the Results - PostProcessing

The first case to be simulated is a laminar, incompressible flow of water at 20C in a rectangular duct (Re ~ 100).

To simplify the problem, the grid will not be generated since it already exists in CFX tutorials files. Therefore, the preprocessing file is loaded by copying the needed files as follows :

cp $TASC_DIR/Examples/tutorials/bcc/rct.lam/* .

Do not forget the dot "." at the end of the command line !

Click here to see the grid and the problem parameters ...

Top of page

To start the main CFX-TASCFlow Application Lancher, type the following UNIX command line :


The CFX-TASCflow Application launcher looks as on figure 1 below :

Fig. 1 : CFX-TASCflow Application launcher

Click on Browse... to locate the directory containing the files that have just been copied, then click on Accept to close the file management panel.

Select Pre-process -> CFX-TASCflow from the main menu bar to open the main window of the CFX-TASCflow GUI.

Top of page

Visualizing the grid

In the GUI top menu bar, select File -> Load PreProcessing : the grid will be displayed on the viewer as shown on figure 2.


Fig. 2 : Wireframe representation of the grid

The grid can easily be explored using :

- the left mouse button to rotate the image,

- the middle mouse button to zoom in and out,

- the right mouse button to reposition the image,

- the <R> key on the keyboard to restore the original image,

- the <C> key to center the image.


Setting Up Zones and Attributes

This section aims at defining the different zone attibutes and the materail properties. In this first case, liquid water will be used.

Click on Physics -> Zones & Attributes to display the "Zone Manager" panel.

- In the "Physical Processes" box, check that the Fluid flow toggle is ON and both the Heat Transfer and Chemical Reaction toggles are OFF.

- In the "Models and Materials Properties" box, click on Materials... to open the "Material Properties" panel, and then on Select... to choose the appropriate fluid. Select Water@STP(SI) in the selection list. Click on OK to close the sub-panel, then on Apply and OK to save the changes.


Creating Boundary Conditions

Click on Boundary conditions -> Specify BCs to make the "Boundary Conditions manager" panel appear. Four types of boundary conditions are required in this problem : wall, inflow, outflow and symmetry.

- To create the wall boundary conditions, select 2_WALL in the panel, then General Default for the Attachment in the "WALL" box. Click on Apply to save.

- To create the inflow boundary conditions, select 1_INFLOW. Choose Specified Region for the attachment, and click on Select... to specify the region. Select RCT_W from the list and click on OK to close the sub-panel. Select then Steady for the Mode, and Mass Flow for the Type. Set the Vector Based On button to Normal, and type 0.01981 for the Mass Flow value.

- To create the outflow boundary conditions, select 3_OUTFLOW and repeat the same steps. Replace RCT_W by RCT_E and Mass Flow by Pressure. Select Average for the Applied As specification, and click on Apply.

- To create the symmetry boundary conditions, select 4_SYMMETRY. Repeat the same steps as previously but replace RCT_W by RCT_S, and at the end click on Apply.


Generating an Initial Guess

In the top menu bar, click on Initial -> Generate Guess... . In the "Initial Guess generator panel", enter the parameters values as follows :

- Domain type : General

- Velocity : Uniform Specified Cartesian

- U = 0.00033

- V = 0

- W = 0

- Pressure = 0

- "Write RSO" toggle : ON

Click on OK.

Top of page

Click on Boundary Conditions -> Check Pre-Process... to check the previous datas. In the specific panel, select the 3 options Zones & Attributes, Grid Interfaces and Boundary Conditions, then click on OK.

To write a BCF file containing the information, click on File -> Write PreProcessing, and quit the pre-processing menu by selesting File -> Quit from the main menu bar.

Top of page

The solver Monitor is loaded by clicking on Solve -> CFX-TASCflow from CFX-TASCflow Application Launcher.


Setting Solver Parameters

In the "Numerics" box, enter the following datas :

- Fluid Time Step option selected, value = 6000

- Number of Time Steps : 50

- Maximum Residual Value : 0.0001

In the "Discretization" box, select the Upwind Difference option.

Click on OK to save those parameters and to close the panel.


Running the solver monitor

In the Solver Monitor, select the following buttons :

- Run Priority : Normal

- Solver Mode : System

- Precision : Single

If a message appears for backing up, rewriting or cancelling existing files, click on Backup : the flow solver starts and the backup files are displayed (Fig. 3). The simulation ends when the convergence criterium (Maximum Residual Value = 0.0001) has been reached.

Momentum & Mass Flow Summary

Fig. 3 : Backup files (BCC)

(Put the mouser on the picture to see the Momentum & Mass Flow Summary)

When the "Simulation Completed" message appears, click on Dismiss and close the monitor by selecting File -> Exit.

Top of page

The post-processing mode is activated by selecting PostProcess -> CFX-TASCflow in the CFX-TASCflow Application Launcher. The datas and results previously obtained are reloaded by clicking on File -> Load PostProcess -> Full RSO (RSO means Re Sults Input and Output file), which displays the "Visualization Object Manager" panel.

Many options are then conceivable in terms of postprocessing. Here are some results that have been computed using the steps above (Fig. 3).

Fig. 3 : Some results obtained with the Visualizer

- Top left-hand corner : Contour map of pressure

- Top right-hand corner :Velocity vector plot on the symmetry plane

- Bottom : Relief map of the speed distribution on cross-sections.

As theoretically predicted in this simple case, the velocity field turns out to be parabolic. It reaches its maximum value in the middle of the duct while being equal to zero near the wall. It can be noticed here that the flow is not totally established yet : if it was, the velocity field would be uniform within the duct. This could be seen far from the velocity inlet if the duct was infinitely long in the X direction.

Top of page

| | | |

| |