This blog is the continuation of the series of blogs on the pump cavitation analysis in ANSYS CFX and to automate this process by using CEL (CFX Expression Language) and Perl script. The previous blogs can be found under the following links;
In this blog we are introducing to the post-processing step in the pump cavitation analysis in ANSYS CFX.
3.1 Opening the Results File:
- Open the “.res” file from the run directory by double clicking on it or
- Start CFX launcher from Start > All Programs > ANSYS [version] > Fluid Dynamics > CFX
Select the working directory and then click on CFD-Post [version] icon or
Go to: CFX > CFD POST [version] or click on Load Results icon or press Ctrl+O on the keyboard, which will then launch CFD post. Specify the file name as and click Open.
This will open Domain Selector dialogue, select all the domains and click OK.
3.2 Inserting Streamlines:
This will open a new dialogue, select the name of streamlines and click OK.
For Geometry tab select BC_In for Start From option and LiquidWater.Velocity in the Variable option.
For Color tab choose variable in Mode option, while select LiquidWater.Velocity as the Variable with local Range.
For Symbol tab choose Tube as Stream Type, with 0.5 Tube Width and click Apply.
Streamlines will look like following.
3.3 Inserting Plane:
Select a plane that is parallel to the inlet face and passes through the blades of the impeller, use the following settings for the Geometry tab.
For Color tab use the settings as described below, leave the default settings for Render and View tabs and click Apply.
The resulting plane will look like the following.
3.4 Inserting Pressure contour:
Go to: Insert > Location > Contour or click on Contour icon , which will open a new dialogue, select the name of the Contour and click OK. In Geometry tab settings, select the name of the plane (already created in previous step) as the Location, pressure as the Variable and select local in the Range options. Leave the remaining settings as default and click Apply.
The pressure contour will look like as the following.
3.5 Inserting Isosurface:
For Geometry tab, select VapourWater.Volume Fraction in the Variable setting, while 0.1 as the Value.
For Color tab select constant Mode and red color in Color option. Leave the remaining settings as default and click Apply.
Also highlight the impeller blades for the cavitation to be more visible, the resulting Isosurface will look like the following.