Engineering Design and Analysis with Innovation

Close Icon
   
Contact Info     +44 141 582 1416

Pump Cavitation Analysis in ANSYS CFX (Part I)

 

In this series of blogs we will be introducing to the basics of the pump cavitation analysis in ANSYS CFX and how to automate this process by using CEL (CFX Expression Language) and Perl script. These blog articles are intended to the people having basic knowledge of using CFX-Pre, CFX-Solver and CFX-Post. If you are not familiar with ANSYS CFX, then please visit the following links for basic information and also go through the ANSYS CFX tutorials, which are available with the software.

ANSYS CFX basic information (http://www.ansys.com/Products/Simulation+Technology/Fluid+Dynamics/Fluid+Dynamics+Products/ANSYS+CFX)
ANSYS CFX technical specification (http://www.ansys.com/staticassets/ANSYS/staticassets/resourcelibrary/brochure/ansys-cfx-tech-specs.pdf)
WIKIPEDIA (http://en.wikipedia.org/wiki/CFX)

1.1  Introduction:

“Cavitation” is the formation and implosion of cavities/bubbles, caused by the partial evaporation of the liquid in a fluid system. A vapour filled cavity/bubble is created when the local static pressure in the flow stream drops below its vapour pressure. This phenomenon is caused by sudden excessive increase in the local velocities, causing pockets of low static pressure to be formed, resulting in local evaporation of the liquid and formation of two phase flow. Once the fluid gets the chance to slow down and the local static pressure is raised above the vapour pressure; these cavities/bubbles “implode”, causing noise and in severe conditions physical damage to the solid surfaces surrounding the flow.

1.2  Analysis Setup:

In ANSYS CFX we use homogeneous multiphase model for the pump applications as the vapour velocity field in this model is assumed to be the same as that of the liquid. Cavitation analysis for the pump application is normally done in two steps. In the first step, cavitation model is turned off to achieve the required convergence of the solution.  While in the second step the cavitation model is turned on and the solution is initialized by the results from the step 1.

Step 1: High Pressure Simulation of Pump with Cavitation Model turned off

1.2.1 Starting a new case File

Go to: File > New Case or click at the New Case icon new case

A new dialogue window will open; Select General and click OK

newcase

1.2.2 Importing Mesh

Go to: File > Import > Mesh or click at the Import Mesh icon  mesh

A new dialogue window will open; Select the mesh file name, location, type and units.

Click Open

browse01

1.2.3 Setting up Analysis Type

Go to: Insert > Analysis Type or double click Analysis Type in the outline tree.

Choose the settings of the Analysis Type tab as in the picture below and click OKanalysistypeanalysistype_01

1.2.4 Loading Materials

Since we are using water at 25 °C and water vapour at 25 °C, we need to load these materials from the Library Data.

In the outline tree, right click on: Simulation > Materials and select Import Library Data.

librarydata_00

Select both, Water at 25 C and Water Vapour at 25 C, holding the Ctrl key.

Click OK.

librarydata

1.2.5 Creating Domains

We will be creating the following three domains for this analysis:

  • Stationery domain for inlet extension.
  • Rotating Impeller domain
  • Stationery domain for outlet extension.

1.2.5.1 Stationery domain for inlet extension.

1.2.5.1.1 Inserting New Domain

Go to: Insert > Domain or click at the Domain icon domain

A new dialogue window will open; Select the domain name as “InletExtension”, and click OK

domainname

1.2.5.1.2 Basic Settings

Go to: Domain: InletExtension > Basic Settings tab and use the following settings.

inletDomain0001inletExt

Under Fluid and Particle Definitions, delete Fluid 1 and create a new fluid definition named LiquidWater.

1.2.5.1.3 Defining Fluid Materials

For defining these Fluid definitions click on Add New Item icon   new case

Create the new material named “LiquidWater” and click OK

liquidWater

The default material in the Fluid and Particle Definitions is set to “Air at 25 C”, to change this material selection, click the Ellipsis icon ellipsis  to open the Material dialogue box.

Select “Water at 25 C” and click OK.

Then click on Apply at Basic Settings tab.

materialdef

Repeat this process for the second fluid “VapourWater”.

Then click on Apply at Basic Settings tab.

vapourwater

1.2.5.1.4 Defining Fluid Models

Go to: Domain:InletExtension > Fluid Models tab and make the settings as shown in figure below and click on Apply. (Please note that the Mass Transfer option is set to None, which turns the cavitation option off for the current analysis.)

domainFluidModel

1.2.5.1.5 Defining Fluid Pairs

Go to: Domain:InletExtension > Fluid Pairs tab and make the settings as shown in the following figure and click on Apply

domainBasicFluidPair

1.2.5.2 Rotating domain for Impeller

Go to: Insert > Domain or click at the Domain icon domain

A new dialogue window will open; Select the domain name as “Impeller”, and click OK

Go to: Domain: Impeller > Basic Settings tab and use the following settings.

rotatingimpellerimpeler

 

Please note that the importance of selecting the correct axis/direction of rotation for the impeller. Right hand rule can be used to define the axis/direction of rotation of the impeller. If you consider the fingers of your right hand in the direction of impeller as indicated by the blue arrow, then thumb will be pointing towards the axis of rotation. If this is along positive axis of the coordinate frame (being used for the impeller domain) then angular velocity as defined in the domain Motion section will have a positive value, otherwise a negative value.

All the remaining settings for Material definition, Fluid Models and Fluid Pair Models tabs will remain same as were in the section 1.2.5.1

1.2.5.3 Stationery domain for outlet extension.

Go to: Insert > Domain or click at the Domain icon domain

A new dialogue window will open; Select the domain name as “OutletExtension”, and click OK

Go to: Domain: Impeller > Basic Settings tab and use the following settings.

outlet_Domain

 

All the remaining settings for Material definition, Fluid Models and Fluid Pair Models tabs will remain same as were in the section 1.2.5.1

1.2.6 Creating Boundaries

1.2.6.1 Inlet Boundary

Go to: Insert > Boundary > in InletExtension or click at the Boundary icon boundaryicon

Or right click on the InletExtension domain in the outline tree and select Insert > Boundary

boundarycond

A new dialogue window will open; Select the boundary name as “BC_In”, and click OK

BC_In

Basic Settings: Select Inlet as the Boundary Type and the face being used for the inlet boundary in Location and click on Apply

In_basic

Boundary Details: Select the following settings and click on Apply

In_Details

Fluid Values: Select the following settings and click Apply.

In_vapourIn_Liquid

 

1.2.6.2 Outlet Boundary

Go to: Insert > Boundary > in OutletExtension or click at the Boundary icon boundaryicon

Or right click on the OutletExtension domain in the outline tree and select Insert > Boundary

outlet_boundary

A new dialogue window will open; Select the boundary name as “BC_Out”, and click OK

BC_Out

 

Basic Settings: Select Outlet as the Boundary Type and the face being used for the inlet boundary in Location and click on Apply

out_basic

Boundary Details: Select the appropriate mass flow setting and click on Apply

out_detail

 

1.2.7 Creating Domain Interfaces: 

Go to: Insert > Interface or click at the Interface icon interface_icon

A new dialogue window will open; Select the interface name as “Interface_01”, and click OK

Basic Settings: Select the following settings for Interface_01 and click on Apply

interface_01

Go to: Insert > Interface or click at the Interface icon interface_icon

A new dialogue window will open; Select the interface name as “Interface_02”, and click OK

Basic Settings: Select the following settings for Interface_02 and click on Apply

interface_02

 

1.2.8 Defining Expressions:

Go to: Insert > Expressions, Functions and Variables > Expressions or click at the Expression icon expression. A new dialogue window will open; Select the expression name as “P1”, and click OK

expressionname

Type in the following expression and click Apply;

massFlowAve(Total Pressure in Stn Frame)@Domain Interface 2 Side 1

(Please note that this expression is case sensitive.)

P1

In similar way also insert the following expressions P2, dP, dH, den, Hs.

expressions

1.2.9 Defining Monitor Points:

Go to: Insert > Solver > Output Control or click at the Output Control icon outputcontrol

Go to Monitor tab and check the option button for Monitor Options and click on Add new item icon new case . A new dialogue window will open; Select the monitor point name as “NPSH”, and click OK

monitor

Select Expression in the monitor option and Hs as the Expression Value.

monitorvalues

In similar way create another monitor point named Head by selecting dH as the expression value for that monitor point.

MonitorPoints

1.2.10 Defining Solver Control:

Go to: Insert > Solver > Solver Control or click at the Solver Control icon solvercontrol

Use the following settings.

solver_Control

1.2.11 Saving Case File:

Go to: File > Save Case or click at the Save Case icon saveicon

Specify the file name as “CFX_CAV_Off.cfx“, specify the location and click Save.

1.2.12 Defining run and starting Solver:

Click at the Define Run icon defineRun

Specify the name and location of the definition file and click Save.

A new dialogue window will open; Select the solver input file and working directory location, for the first run we are not using any initialization file, you can also specify settings for parallel processing. Specify the settings and click Start Run.

runsolver

 

Post Tagged with , , , ,

5 Responses so far.

  1. [...] offers part 1 of a series of blog posts about pump cavitation analysis using [...]

  2. [...] ANSYS CFX and to automate this process by using CEL (CFX Expression Language) and Perl script. Pump Cavitation Analysis in CFX (Part I) Pump Cavitation Analysis in CFX (Part II) Pump Cavitation Analysis in CFX (Part III) [...]

  3. Adarsh says:

    Just one question. Where can I find the mesh?

Leave a Reply

Your email address will not be published. Required fields are marked *

You may use these HTML tags and attributes: <a href="" title=""> <abbr title=""> <acronym title=""> <b> <blockquote cite=""> <cite> <code> <del datetime=""> <em> <i> <q cite=""> <strike> <strong>