TUTORIAL - Simulation of a Flow. Step 1.

Flow Simulation. Step 1.

Author: E.O. Pankova, Moscow Baumann State Technical University

This tutorial shows how to set up and run the simulation of laminar flow of air with neither friction nor heat exchange at the walls.

The geometry is 2-dimensional, of (y-direction) depth 1.0 m, with the vertical (z-direction) dimension 1m and the horizontal (x-direction) dimension 2m :

wherein:

INLET is an aperture through which air at 20 degrees C enters at a prescribed velocity of 0.05m/s.
OUTLET is a fixed-pressure aperture, where the pressure is held close to 0.0 Pa, relative to the external pressure.

Preliminary remarks

In addition to physically-meaningful data of the above kind, all CFD codes, and therefore PHOENICS also, require non-physical inputs such as:

a grid of computational cells;
instructions about how many iterations to make of the trial-and-error solution process;
how much data to print.

The non-physical settings suggested below are such as to make the calculations rapid rather than accurate.
Other tutorials will be provided which will enable you to explore the influences of the settings on accuracy and speed of calculation.

Choosing the working directory

Your working directory is the folder in which will appear all the files which the tutorial creates. Your first step will be to choose this by:

clicking on the 'Top Page' of the Commander;
clicking on the 'Customise' icon;
clicking on the 'Choose Working Directory' icon, which will elicit a window such as this:
Open the 'd_pc' folder (by clicking on its '+' sign) ; then 'tuts'; click on 'beginnrs' and then on 'OK'.

Your working directory is now \phoenics\d_pc\tuts\beginnrs.

Starting the tutorial

First close any windows which are already running PHOENICS modules (Satellite, Earth or Viewer).

Then activate the PHOENICS Satellite module, in its VR-Editor mode by entering the 'Run Modules' panel of the PHOENICS Commander, and then clicking the 'VRE' button.

You can change the background colour, if you wish, by clicking on 'Options' - 'Background Colour' and then making your choice.

In PHOENICS-VR Editor

When the Editor starts execution, what it shows on the screen at first will depend on what Q1 file happens to be in your working directory.
If there is none, you can proceed immediately. Otherwise, make a fresh start, as follows.
1. [If you see the words: 'Display From Current Q1', click the top-right X so as to close the panel ]
2. clicking first on 'File';
3. then on 'Start New Case';
4. then on 'Core';
5. then on 'OK' to confirm the resetting.
You are now ready to begin.

Set the domain size

Click on 'Menu' or 'M' (according to whether the 'Control panel' is visible) [If it is not, you can make it so by clicking on 'View'].
Set 'Flow Simulation. Step 1' as the title (or any other which you prefer).
Click on 'Geometry'.
Note that clicking on '?' at the top right of any panel and then on a menu button will provide 'help'.
.
Change the X-Domain Size from its default (1.0 m) to 2.0 m.
Click 'OK' to close the Grid mesh settings dialog.

Select the working fluid

Click on 'Properties' which will elicit a page like this:
Note that the properties are already those of "Air at 20 deg C, 1 atm" by default. Since these correspond to the present case, there is no setting to make.
Click on 'Top menu' to accept.

Indicate for which variables solution is required

Click on 'Models'.
Leave 'Solution for velocities and pressure' at the default setting: ON.
Click on 'Turbulence models' and select 'Laminar'. Click on 'OK'.
Click on 'Top menu', then on 'OK' to exit the Main Menu.

Re-sizing the domain

The domain no longer fits the screen; to resize, click on the pull-down arrow next to the 'R' icon on the toolbar; then 'Fit to window'.

Introduce the required objects

Click on the 'object-management' button ('O' on the toolbar or on the Control panel, also sometime called 'hand set').
This will display the 'object-management' window with a list of objects of which only 'DOMAIN' is currently present.
You will now introduce the objects which you require, one-by-one, giving each a position and size.
You will also introduce 'attributes', for example material, velocity or temperature, so completing the description of the situation to be simulated.

Introduce the INLET object
- Click on 'Object', 'New' and New Object'.
- Change name, if you wish, for example to MY_INLET (not more than 8 characters can be used)
- Click on 'Size' and set SIZE of object as:
  - Xsize: 0.0
  - Ysize: 1.0
  - Zsize: 1.0
- Click on 'Place' and note that the default Position of object (Xpos=0.0, Ypos=0.0, Zpos=0.0) need not be changed.
- Click on 'General'.
  - Select 'Type': INLET.
  - Click on 'Attributes' and set the velocity in X-direction to 0.05 m/s.
  - Click on 'OK' to close the Attributes menu,
  - and on 'OK' in the Object Specification Dialogue Box.
Introduce the OUTLET object
- Click on 'Object', 'New' and New Object'.
- Change name to MY_OUT, for example.
- Click on 'Size' and set SIZE of object as:
  - Xsize: 0.0
  - Ysize: 1.0
  - Zsize: 1.0
- Click on 'Place' and set Position of object as:
  - Xpos: 2.0
  - Ypos: 0.0
  - Zpos: 0.0
- Click on 'General'.
  - Define 'Type': OUTLET.
  - Leave the default values in the Attributes dialogue box.
  - Click on 'OK' to exit the Object Dialogue Box.
  - Close the Object Management window by clicking the button with X in the top right-hand corner of the window.
Set the grid
Once the PHOENICS satellite has been told what objects are present, it sets a 'default' computational grid. This may or may not be satisfactory for computational accuracy.
- Click on the 'Mesh toggle' button to display the default mesh on the screen. This shows subdivision in X-direction but none in Y or Z, because no indication has been given that variations in the latter directions exist.
- Click anywhere on the image, and the 'Gridmesh settings' dialog box will appear. The grid in all three directions is set to 'Auto'.
  To understand what this means, click on the top-right '?', and then on the word 'Auto'. An explanatory screen will then appear.
  In the present case 'Auto' gives 20 cells in X, 1 cell in Y and Z.
- This does not give a very interesting picture; therefore change the number of cells in Z-direction to 15. To do so, click on Z-Auto button to switch to Manual mode and then type the proper number in the corresponding box. Click on 'OK' to close the dialog box.
- The mesh will now be shown as blue and red lines. The latter show the edges of the objects (or domain); the former are those introduced by PHOENICS.
- Click on 'Mesh toggle' again to turn off the mesh display.
The remaining solution-control parameters
In later tutorials, you will be invited to click on 'Menu' and then on 'Numerics', in order to inspect and modify other solution-control parameters. However, the defaults which have been set will suffice for the present purposes.

Running the Solver

You are now ready to perform the simulation by activating the PHOENICS solver module (known as 'Earth').

In order to do so, click on 'Run', 'Solver, and click on 'OK' to confirm.

You will then see, in quick succession, indications on the screen of:

the activation of the module;
the reading by the solver of the input data which your tutorial session has prepared for it;
the progress of the calculation, represented by the generation of curves which look something like this:

Upon the end of the calculation, the VR Editor window will be displayed again.

You are now able to launch the VR Viewer, in order to inspect the results of your calculation.

Using the VR Viewer.

Click on 'Run', 'Post processor',then GUI Post processor (VR Viewer) . Click 'OK' on the file names dialog to accept the default files.

To select the 'coloring variable', i.e. that which gives color to vectors, contours and streamlines, do the following:
- To select Pressure - click on the 'Select Pressure button' .
- To select Velocity - click on the 'Select Velocity button' .

To view:

Velocity vectors - click on the 'Vector toggle' . Vectors are coloured by the current plotting variable, but their length is always related to the absolute velocity. In this case they are all of the same length because there is nothing to cause significant variations of velocity.
Contours - click on the 'Contour toggle'
Streamlines - click on the 'Streamline management' button
Iso-surfaces - click on the 'Iso-Surface toggle'

To change the direction of the plotting plane, set the slice direction to X, Y or Z

To change the position of the plotting plane, move the probe using the probe position buttons

probe position (927 bytes) .

Alternatively, click on the probe icon on the toolbar or double-click the probe itself to bring up the Probe Location dialog.

One plot from this case is:

The small differences of velocity (between 0.050002 and 0.049993) on this plot may be attributed to the small inaccuracies associated with all numerical calculations.

Another plot displays the pressure distribution. It is to be expected that the pressure should be uniform; but in fact small variations (between 5.946E-5 and 5.938E-5) appear, which are explained in a similar manner.

Saving the results.

In the VR Viewer click on 'File' then 'Save as a case'. At this point you will see that the folder 'step1' already exists. Open it. (If this were not a prepared tutorial, you would have to create your own new folder and choose for it whatever name you wish.)

Save as 'step1'.

You will find in the folder the following files created during this run:

step1.q1, a copy of the Q1 file created in the tutorial;
step1.res, a copy of the RESULT file printed by the solver at the end of its execution;
step1.phi, a copy of the PHI file which the VIEWER uses as the basis of its displays;
step1.gif, an image representing the approach to convergence, such as was shown above;
step1.pat and
step1.pbc, which there is no need to describe now.

You will also find there the file step1mod.q1 which is provided for your convenience at installation time.

Your step1.q1 should be identical with step1mod.q1, which you could run in case you prefer not to follow tutorial recommendations.

Next Step

Flow Simulation. Step 1.

Preliminary remarks

Choosing the working directory

Starting the tutorial

In PHOENICS-VR Editor

Set the domain size

Note that clicking on '?' at the top right of any panel and then on a menu button will provide 'help'.

Select the working fluid

Indicate for which variables solution is required

Re-sizing the domain

Introduce the required objects

Introduce the INLET object

Introduce the OUTLET object

Set the grid

To understand what this means, click on the top-right '?', and then on the word 'Auto'. An explanatory screen will then appear.

The remaining solution-control parameters

Running the Solver

Using the VR Viewer.

Saving the results.