• Author / Uploaded
• Raul Dionicio

Citation preview

Flow and Blend Simulations in Mixing tank using Fluent

Sravan Kumar. N ANSYS Inc.

© 2009 ANSYS, Inc. All rights reserved.

1

ANSYS, Inc. Proprietary

Agenda • Geometry & Mesh • Single phase simulation – Case setup – Results • Blend simulation – Case setup – Results

© 2009 ANSYS, Inc. All rights reserved.

2

ANSYS, Inc. Proprietary

Bioreactor: Geometry

Tank Diameter (in)

40

Operating volume (m^3)

1.0725

Liquid level (in)

55

Number of impellers

2

Impeller(s)

Rushton Turbine & LA310

Impeller diameter (in)

RT-18” & LA310-16”

Shaft Diameter (in)

1.6

Sparger

Straight sparger with bottom facing gas inlet

Number of baffles

4

Baffle dimensions (in.)

3.6” & 10” from tank bottom

© 2009 ANSYS, Inc. All rights reserved.

3

ANSYS, Inc. Proprietary

Bioreactor: Geometry • Working volume: 1072L – Impellers:2 • Rushton turbine • LA-310 (downward pumping) – Baffles: 4 – Straight sparger • Mesh – Tetragonal elements – Number of cells:~ 725K

© 2009 ANSYS, Inc. All rights reserved.

4

ANSYS, Inc. Proprietary

Bioreactor: Mesh distribution • Working volume: 1072L – Impellers:2 • Rushton turbine • LA-310 (downward pumping) – Baffles: 4 – Straight sparger • Mesh – Tetragonal elements – Number of cells:~ 725K

© 2009 ANSYS, Inc. All rights reserved.

5

ANSYS, Inc. Proprietary

Flow simulation: Reading mesh file • Opening Fluent – You can open the fluent by double clicking on the Fluent case file – Or StartAll ProgramsANSYS 13.0Fluid DynamicsFLUENT – This opens up the Fluent session launcher – Make sure that 3D is selected as Dimension and Double Precision is selected in Options

• Reading the mesh file – In Fluent menu bar, go to FileRead Mesh and browse to the location where the mesh file is present and select the appropriate file

© 2009 ANSYS, Inc. All rights reserved.

6

ANSYS, Inc. Proprietary

Mesh: • In Problem Setup – GeneralMeshScale • Make sure that the dimensions of the domain are proper • You can scale the domain by selecting the unit used to create the geometry or specify a scaling factor to scale the geometry

– Check the mesh using GeneralMeshCheck option

© 2009 ANSYS, Inc. All rights reserved.

7

ANSYS, Inc. Proprietary

Solver: Models • Models – Select ModelsViscous to open the turbulence model panel – Select k-epsilon model with Realizable option • Keep the Near-wall Treatment as default.

– If there are no baffles in the tank, Reynolds Stress model (RSM) will be accurate for highly swirling flows • Since convergence can be difficult with RSM, you can run the simulation with RKE for few thousand iterations before switching over to RSM.

© 2009 ANSYS, Inc. All rights reserved.

8

ANSYS, Inc. Proprietary

Selecting fluid material • Materials – Select Materials option and select Fluid and click Edit option to open the material properties panel. – Click on Fluent Database to open the material properties database. Browse through the materials and select water-liquid, click copy and close the database. – Edit the water properties accordingly and click on Change/Create. – Close the material properties window.

© 2009 ANSYS, Inc. All rights reserved.

9

ANSYS, Inc. Proprietary

Cell zone conditions • Click on cell zone conditions and select a fluid zone and click Edit • Change the material from air to water-liquid • If the zone is rotating zone, select Frame motion option – In the details below provide rotational axis origin and rotational axis direction vector – Provide the angular velocity •

You can change the units of angular velocity to rpm using top menu bar DefineUnitsAngular Velocityrpm

– Click OK to close the window.

• Similarly set similar conditions to other rotational zone. • For stationary zone, simply change the material from air to water-liquid. © 2009 ANSYS, Inc. All rights reserved.

10

ANSYS, Inc. Proprietary

Boundary conditions • Single phase flow simulation can be used under the assumption that the liquid level will not change appreciably at the chosen operating conditions and can be considered as flat surface. • Since flow simulation in mixing tank is a batch process, make sure that there are no inlet or outlet boundaries defined. • If there is any boundary that exists in rotational zone but is stationary in absolute frame, make sure you specify the boundary condition in absolute frame by selecting wall motion as zero.

© 2009 ANSYS, Inc. All rights reserved.

11

ANSYS, Inc. Proprietary

Boundary conditions • In boundary conditions, – Select the boundary that represents the top surface of the tank and click Edit • In shear condition select Specified Shear option and keep default value of zero. • Click OK to close the panel. • This is similar to symmetry boundary condition where there are no vertical gradients across the surface are present © 2009 ANSYS, Inc. All rights reserved.

12

ANSYS, Inc. Proprietary

Boundary conditions • In boundary conditions, – Select the boundary that represents the shaft surface in the stationary zone of the tank and click Edit • Under Wall Motion, select Moving Wall. • Under Motion, select Absolute and Rotational – Provide the rotational speed and the rotational axis origin and direction similar to what is provided in cell zone conditions

• Click OK to close the window

© 2009 ANSYS, Inc. All rights reserved.

13

ANSYS, Inc. Proprietary

Boundary conditions • In boundary conditions, – If the baffles are of zero thickness, make sure that the boundary type is selected as wall – If the boundary type is selected as interior, change it to wall boundary condition • Fluent will create a shadow wall for zero thickness wall surfaces

© 2009 ANSYS, Inc. All rights reserved.

14

ANSYS, Inc. Proprietary

Solution Methods • SolutionSolution Methods – Select Second order Upwind scheme for Momentum – Use first order upwind scheme for turbulence quantities • After running the simulation for few thousand iterations, you can switch the turbulent quantities to second order upwind scheme • This can be automatically done using Calculation Activities

– If RSM model is used, keep the first order upwind scheme for Reynolds stresses.

© 2009 ANSYS, Inc. All rights reserved.

15

ANSYS, Inc. Proprietary

Solution Controls • SolutionSolution Controls – Change the pressure URF to 0.5 – Momentum: 0.5 – If the residuals are not converging well, • Reduce the momentum to 0.3 • Reduce the turbulent kinetic energy and dissipation rate URFs to 0.8

© 2009 ANSYS, Inc. All rights reserved.

16

ANSYS, Inc. Proprietary

Monitors • MonitorsResidual –

–

Lower the absolute residual criteria for all varialbles Click OK to close the panel.

• MonitorsMoment – – –

Select the impeller boundaries under Wall Zones Select Plot and Write option Provide the Moment center and Moment axis inputs similar to the rotational axis inputs specified in the cell zone conditions

• MonitorsVolume –

Create a volume monitor for volume average velocity over all fluid zones

• These three monitors will help checking whether the simulation has reached a steady state or not. • Make sure that you check both moment and velocity monitor for checking the steady state apart from checking residuals

© 2009 ANSYS, Inc. All rights reserved.

17

ANSYS, Inc. Proprietary

Solution Initialization • SolutionSolution Initialization – Provide an initial value of 0.01 for turbulent kinetic energy and 0.1 for turbulent dissipation rate – Click Initialize button to initialize the solution

© 2009 ANSYS, Inc. All rights reserved.

18

ANSYS, Inc. Proprietary

Calculation activities • SolutionCalculation activities – Autosave • Specify autosave frequency so that intermediate files are saved

– Automatically Initialize and Modify Case • This option allow the specification of any commands to modify the case setup during the simulation • Select this option and click on Edit

© 2009 ANSYS, Inc. All rights reserved.

19

ANSYS, Inc. Proprietary

Calculation activities • SolutionCalculation activities –

Automatically Initialize and Modify Case • • • •

Keep the default value for initializing the case Select Case Modification tab Increase the defined modifications to 2. We can enter the commands that can change the discretization scheme from first order to second order after specified number of iterations. –

• •

•

The image here shows that the simulation is run with default settings for 2000 iterations and discretization schemes for k and epsilon are changed to second order after 2000 iterations and simulation is run for 8000 more iterations after changing the discretization schemes.

Click OK to close the panel A Question dialog box may appear. If the Original Settings field is empty, then you may be notified that the original settings will be lost if the case is saved after the modifications are applied. It will prompt you for a response when asked if you would like to add commands that specify the original settings. You can select No.

© 2009 ANSYS, Inc. All rights reserved.

20

ANSYS, Inc. Proprietary

Run Calculation • Save the initial case and data files through FileWriteCase & Data • SolutionRun Calculation – Click Calculate button to start the calculation • Monitor the solution for residuals, moment and average velocity – Interrupt the calculation if a steady state is reached in both moment and average velocity

© 2009 ANSYS, Inc. All rights reserved.

21

ANSYS, Inc. Proprietary

Results: Flow simulation

Moment monitor

Volume average velocity monitor

Velocity vectors on Y=0 plane © 2009 ANSYS, Inc. All rights reserved.

22

ANSYS, Inc. Proprietary

Blend time simulation setup

© 2009 ANSYS, Inc. All rights reserved.

23

ANSYS, Inc. Proprietary

Blend time simulation: Introduction • Blend time simulation will be performed using the flow field data obtained from flow simulation. • Flow field will be frozen and the tracer mass fraction is solved in transient way to calculate the time taken to reach the uniform concentration. • A small region containing few cells will be marked and tracer mass fraction will be patched in this region with a value of 1. • Point monitors will be defined where the tracer mass fraction will be tracked w.r.t time. • These saved monitors will be analyzed later to calculate the blend time with desired uniformity.

© 2009 ANSYS, Inc. All rights reserved.

24

ANSYS, Inc. Proprietary

Blend simulation: Opening Fluent simulation • Opening Fluent – You can open the fluent by double clicking on the Fluent case file – Or StartAll ProgramsANSYS 13.0Fluid DynamicsFLUENT – This opens up the Fluent session launcher – Make sure that 3D is selected as Dimension and Double Precision is selected in Options

• Reading the case and data files – If the case file is already read, Fluent displays the mesh and you can read the data file through FileRead Data option in menu bar – Or, In Fluent menu bar, go to FileRead Case & Data and browse to the location where the fluent files are present (previous slide) and select the appropriate file

© 2009 ANSYS, Inc. All rights reserved.

25

ANSYS, Inc. Proprietary

Blend simulation: Setup • Open fluent session as specified in previous slide and read the saved case and data files of the flow simulation. • Click on General in Problem Setup column – Change the Time option from Steady to Transient • Click on Models option and select Species option in the column and click Edit • Select Species Transport and deselect Inlet Diffusion and Diffusion Energy Source in Options column. • Click Apply • You will get a notification that material properties are changed. Click OK to close the notification window • Click Ok to close the Species model panel. © 2009 ANSYS, Inc. All rights reserved.

26

ANSYS, Inc. Proprietary

Blend simulation: Material properties • Click on Materials and select waterliquid under Fluid and click Create/Edit button • Material properties panel for water liquid will be opened. Change the Name to tracer and remove the chemical formula and leave the rest of the properties same. • Click Change/Create button • A Question window appears asking whether to overwrite the water-liquid. Click No. This will create a separate tracer material with similar properties that of water.

© 2009 ANSYS, Inc. All rights reserved.

27

ANSYS, Inc. Proprietary

Blend simulation: Mixture properties • Under Material Type, select Mixture • In the Properties column, against Mixture Species, click Edit • Add tracer to the Selected Species followed by waterliquid. Remove the other species from the Selected Species list. • Now the mixture material contains tracer and water. Click Ok to close the panel

© 2009 ANSYS, Inc. All rights reserved.

28

ANSYS, Inc. Proprietary

Blend simulation: Mixture properties • Under Properties, change the Density formulation to Volume-Weighted-Mixing-Law • Similarly change the Viscosity formulation to Mass-Weighted Mixing-Law • Provide the Mass Diffusivity as 1e-9 as liquid-liquid diffusivities are of this range • Click Change/Create button and Close the Materials panel.

© 2009 ANSYS, Inc. All rights reserved.

29

ANSYS, Inc. Proprietary

Blend simulation: Solution settings • In Problem setup, click on ModelsEnergy and switchoff the energy equation • SolutionSolution Methods – Under Spatial discretization change the tracer scheme to QUICK scheme

• SolutionSolution Controls – Click on Equations – Select only tracer and deselect other equations

© 2009 ANSYS, Inc. All rights reserved.

30

ANSYS, Inc. Proprietary

Blend simulation: Residuals • Solution – Click on MonitorsResiduals • Change the Absolute criteria for tracer residual from 0.001 to 5e-5

– Switch off the other monitors like Moment monitor and volume monitors if defined.

© 2009 ANSYS, Inc. All rights reserved.

31

ANSYS, Inc. Proprietary

Blend simulation: Iso-surface • In top Menu bar, select SurfaceIsoSurface – Create a surface by choosing appropriate x, y or z-coordinate and give a name. – Click Create to create the surface and Close the panel

© 2009 ANSYS, Inc. All rights reserved.

32

ANSYS, Inc. Proprietary

Blend simulation: Creating dose point • • • •

•

In the top horizontal menu bar, select DisplayMesh Select the shaft, impeller and the iso-surface created in previous slide under Surfaces. Click Display and Close the panel. In the top menu bar, select AdaptRegion – Select Sphere under shapes – Click on “Select points with mouse” option – Right click button is the mouse probe button. Right click on the desired location to select center – Right click on another point, which will decide the radius as distance between previously selected point and this point – Click on Mark – Number of cells marked will be displayed in console. Make sure that atleast 10 cells are marked. If not, select the center and radius again. – Click Close to close the window – You can also select the points in different locations or give the center and radius manually. This marked region will act as dose point for tracer

© 2009 ANSYS, Inc. All rights reserved.

33

ANSYS, Inc. Proprietary

Blend simulation: Creating points to monitor mass fraction • In the top menu bar, select SurfacePoint – Click on “Select points with mouse” option – Right click on the mesh at desired location to select a point where tracer mass fraction needs to be monitored – Give a name to the point surface and click Create – Similarly create more points in the tank to monitor tracer mass fraction – Click Close button to close the panel

© 2009 ANSYS, Inc. All rights reserved.

34

ANSYS, Inc. Proprietary

Blend simulation: Defining monitors • In Solution, click on Monitors • Under Surface Monitors, click Create… – Under Report Type, select Vertex Average – Under Field variable, select Species – Under surfaces, select the point monitor created to monitor tracer mass fraction – Select Plot and Write options to enable plotting and writing of monitor – Under X-Axis, select Flow Time and select Time Step to get the data – Click Ok to define the monitor and close the panel.

• Similarly define other monitors in the same way if there are multiple point surfaces

© 2009 ANSYS, Inc. All rights reserved.

35

ANSYS, Inc. Proprietary

Blend simulation: Initial conditions • Under Solution, select Solution Initialization – Click Patch – Select tracer under Variable – Select the recent spherical register under Register to Patch column – Provide 1 as value – Click Patch and Close the panel.

© 2009 ANSYS, Inc. All rights reserved.

36

ANSYS, Inc. Proprietary

Blend simulation: Setup procedure for animation • An iso-surface of tracer mass fraction will be created with a value equals to half of average mass fraction in the domain • This iso-surface represents the tracer mass fraction front. • Displaying this isosurface at specified interval of time steps will show the movement of tracer front in the domain. • Images will be saved at this interval to create an animation which shows the tracer front movement.

© 2009 ANSYS, Inc. All rights reserved.

37

ANSYS, Inc. Proprietary

Blend animation setup: Calculate volume average tracer mass fraction • Under Results column, go to ReportsVolume integrals and click Setup – Under Report Type, select Volume-Average – Under Field Variable, select speciesMass fraction of tracer – Under Cell zones, select all the fluid zones – Click Compute – The average mass fraction will be displayed in the window and the console – Click Close button to close the window. – Calculate the value of half of the average concentration.

© 2009 ANSYS, Inc. All rights reserved.

38

ANSYS, Inc. Proprietary

Blend animation setup: Create isosurface of tracer

• In the top menu bar, select SurfaceIsosurface – Create a Surface of Constant SpeciesMass fraction of tracer and provide an Iso-Value of half the average concentration – Give the name of the surface as tracer-front – Click Create to create the surface and Close the panel © 2009 ANSYS, Inc. All rights reserved.

39

ANSYS, Inc. Proprietary

Blend animation setup: Setting a view • Displaying the surfaces – In menu bar, go to DisplayMesh – Select Edges in options, Outline in Edge Type – Click on Outline button twice to select all the boundary surfaces. Include tracer-front surface in the Surfaces list – Click Display and Close the window

• In the Menu bar, select DisplayViews – Select a view in the Views list and click Apply to setup a view – Adjust the view by rotating the geometry in the graphics window using left mouse button for better view. – Give this view a name as view-0 and click on Save – Close the Views panel.

© 2009 ANSYS, Inc. All rights reserved.

40

ANSYS, Inc. Proprietary

Blend animation setup: Recording journal file • In the top menu bar – FileWriteStartJournal – Give the name of the journal file as tracerimages.jou and click Ok. – From this point all the operations done in fluent will be recorded in the journal file. © 2009 ANSYS, Inc. All rights reserved.

41

ANSYS, Inc. Proprietary

Blend animation setup: Recording journal file • Setting a window for display – In menu bar, go to DisplayOptions – Change the Active Window to 5 and click Set – Click Apply and Close the window

• Displaying the surfaces – In menu bar, go to DisplayMesh – Remove Edges in options and select Faces and include tracerfront surface in the Surfaces list along with other tank boundaries like baffles, tank wall etc. – Remove the post-processing surfaces (e.g., x=0 surface) – Click Display and Close the window. © 2009 ANSYS, Inc. All rights reserved.

42

ANSYS, Inc. Proprietary

Blend animation setup: Recording journal file • Setting the transparency – In menu bar, go to DisplayScene – Under Names, select all the faces except tracer-front and click on Display button • •

This will open the display properties window Select Visible, Faces, Lighting under Visibility and set the Transparency to 60 and click Apply and Close the window.

– Under Names, deselect all the surfaces and select tracer-front surface and click on Display button •

Select Visible, Faces, Lighting under Visibility, Adjust the color, set the Transparency to 0, click Apply and Close the window.

– Click on Close button to close the window

© 2009 ANSYS, Inc. All rights reserved.

43

ANSYS, Inc. Proprietary

Blend animation setup: Recording journal file • In the Menu bar, select DisplayViews – Select the already saved view view0 in the Views list and click Apply – Click Close button to close the window.

• In the Menu bar, select FileSave Picture – – – – –

Select JPEG as Format Select Color De-select white Background Click Save Give the name as tracer-%t.jpg and click OK. •

This will attach the time step to the file name

– Click Close button to close the Save Picture window.

© 2009 ANSYS, Inc. All rights reserved.

44

ANSYS, Inc. Proprietary

Blend animation setup: Recording journal file • Setting the window to default – In menu bar, go to DisplayOptions – Change the Active Window to 1 and click Set – Click Apply and Close the window

• In the top menu bar – FileWriteStop-Journal

© 2009 ANSYS, Inc. All rights reserved.

45

ANSYS, Inc. Proprietary

Blend simulation: Calculation activities • In Solution, select Calculation Activities – Under Execute Commands, click on Create/Edit button • Increase the Defined Commands to 1 • Select Active • Specify the interval after which the images need to be saved under Every • Select Time Step under When • Under command, give “file read-journal tracer-images.jou” • Click Ok to close the window.

• This will read the journal file saved previously after specified time steps and save the tracer-front image

© 2009 ANSYS, Inc. All rights reserved.

46

ANSYS, Inc. Proprietary

Blend simulation: Calculation activities • In Solution, select Calculation Activities – Click on Edit button under Autosave Every option

• Autosave data files – You can specify the interval after which the intermediate data files will be saved – Click OK to close the window.

© 2009 ANSYS, Inc. All rights reserved.

47

ANSYS, Inc. Proprietary

Blend simulation: Run Calculation • Under Solution, select Run Calculation – Specify the Time Step Size • A value of 0.01 sec can be used by default

– Specify the Number of Time Steps such that number of time steps * time step size gives the desired flow time until which the simulation needs to run.

• In the top menu bar, select FileWriteCase&Data and give the appropriate name to save the initial blend case and data files. • Under SolutionRun Calculation

– Click Calculate to start the simulation. © 2009 ANSYS, Inc. All rights reserved.

48

ANSYS, Inc. Proprietary

Blend simulation: • During the simulation – Monitor files will be displayed and written in the directory where case and data files are present – Tracer mass fraction front images will be saved at each specified interval – Run the simulation until the point monitors reach the uniform concentration and the value do not change with additional simulation time.

© 2009 ANSYS, Inc. All rights reserved.

49

ANSYS, Inc. Proprietary

Blend simulation: • After the simulation, – Save the final case and data files of blend simulation – Process the point monitors in Microsoft Excel to calculate the time taken for each monitor to reach desired uniformity (E.g.,95% or 99%) – An animation can be created using the saved tracer image files. The procedure to create the animation files from image files can be found here: http://www.bakker.org/cfm/graphics01.htm © 2009 ANSYS, Inc. All rights reserved.

50

ANSYS, Inc. Proprietary

Results: Blend simulation • Evolution of species mass fraction at different points is shown here. • Maximum blend time considering all the four monitors – ~13 sec (for 95% homogeneity)

© 2009 ANSYS, Inc. All rights reserved.

51

ANSYS, Inc. Proprietary

Blend simulation: Animation with ImageMagick software • If the ImageMagick is already installed, you can create the animation using these steps – Open command prompt – Go to the directory where the tracer image files are present

© 2009 ANSYS, Inc. All rights reserved.

In command prompt, go to the directory where the compressed file (.zip) is present using cd command.

52

ANSYS, Inc. Proprietary

Blend simulation: Animation with ImageMagick software • Use the following command to convert tracer-%t.jpg image files to .gif images – “mogrify –format gif tracer*.jpg”

• To create animation – “convert –adjoin –delay 5 *.gif blendanimation.gif”

© 2009 ANSYS, Inc. All rights reserved.

53

ANSYS, Inc. Proprietary