Back to all tutorials

Mixing Tank - CFD Simulation SimFlow Tutorial

1. Download SimFlow

SimFlow is a general purpose CFD Software

To follow this tutorial, you will need SimFlow free version, you may download it via the following link:
Download SimFlow

2. Create Case

Open SimFlow and create a new case named mixing_tank

  1. Go to New panel

  2. Provide name mixing_tank

  3. Click Create Case

mt 1 create case

3. Import Geometry

After creating case Download GeometryImpeller

  1. Click Import Geometry

  2. Select geometry file impeller.stl.gz

  3. Click Open

mt 2 import geometry

4. Imported Geometry Units

In a next step we need to select the unit in which the model was exported. The STL format does not contain the unit information which are defined during the geometry export. The Geometry size displays the overall size of the model what allows to select the suitable unit. In this case, the default unit meter is correct.

  1. To confirm default unit meter, press OK

mt 2 unit

5. Geometry - Impeller

After importing geometry, it will appear in the 3D window.

  1. Click Fit View to zoom the geometry

mt 3 geometry

6. Create Geometry - Shaft

The original impeller geometry consists of only blades. To make the impeller complete we will add a shaft using a primitive geometry.

  1. Click Create Cylinder

  2. Rename cylinder_1 to shaft
    (double click on the geometry name to start rename)

  3. 4 Define cylinder origin, length, and radius
    Origin \({\sf [m]}\)00-0.045
    Length \({\sf [m]}\)0.5
    Radius \({\sf [m]}\)0.04

mt 4 crete geometry shaft

7. Create Geometry - Rotating Zone

We want our impeller to be rotating. We will create a cylindrical zone that will be used to divide the mesh into rotating and stationary part.

  1. Click Create Cylinder

  2. Rename cylinder_1 to rotating_zone

  3. 4 Define cylinder origin, length, and radius
    Origin \({\sf [m]}\)00-0.105
    Length \({\sf [m]}\)0.6
    Radius \({\sf [m]}\)0.3

mt 5 create geometry rotating zone

8. Show Impeller

All parts of the geometry are displayed in the graphics window now. Note that rotating_zone encloses the impeller and shaft. In order to see all geometries, we will decrease the opacity of the rotating_zone.

  1. Press Esc to exit edit mode then select rotating_zone if it is not selected

  2. Click Display Properties

  3. Adjust Opacity to 50%

mt 6 show impeller

9. Meshing Properties - Impeller

We will enable meshing for impeller geometry.

  1. Go to Hex Meshing panel

  2. Select impeller

  3. Check Mesh Geometry

  4. Set Refinement to Min 1 Max 2

mt 7 meshing properties impeller

10. Meshing Properties - Rotating Zone

Since our domain will consist of a stationary and a rotating part we need to create a mesh interface between the parts. To do this we will create a baffle using the rotating_zone geometry.

  1. Select rotating_zone

  2. Check Mesh Geometry

  3. Check Create Cell Zone

  4. Change Refinement Max level to 1

  5. Check Create Baffle

mt 8 meshing properties rotating zone

11. Meshing Properties - Shaft

We need to also mesh the shaft geometry.

  1. Select shaft

  2. Check Mesh Geometry

mt 9 meshing properties shaft

12. Base Mesh - Geometry

Now we will define the outer bounds of the computational domain.

  1. Go to Base tab

  2. Select Cylinder as the base mesh type

  3. Define cylinder axis, origin, length, and radius
    Origin \({\sf [m]}\)-0.18
    Length \({\sf [m]}\)0.9
    Radius \({\sf [m]}\)0.6

mt 10 base mesh geometry

13. Base Mesh - Mesh

To have an appropriate mesh density we will use the following divisions and grading of the base mesh.

  1. 2 Define radial division, radial grading, axial division, and central division
    Radial Division15
    Radial Grading1.02
    Axial Division30
    Central Division15

mt 11 base mesh mesh

14. Base Mesh - View

We can preview the Base Mesh in the graphics window.

mt 12 base mesh view

15. Base Mesh - Boundaries

Now we need to assign individual names to each side of the base mesh. Since we are modeling a closed tank all our boundaries will be defined as walls.

  1. Type boundary names accordingly
    First Disk walls
    Second Disk walls
    Cylinder walls

  2. Change type of all boundaries to wall
    First Disk wall
    Second Disk wall
    Cylinder wall

mt 13 base mesh boundaries

16. Material Point

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are modelling flow inside the tank we need to place the material point between the tank walls and the propeller.

  1. Go to Point tab

  2. Specify location inside the mesh
    Material Point0-0.3-0.1

mt 14 material point

17. Meshing

Everything is now set up for meshing.

  1. Go to Mesh tab

  2. Click Mesh button to start meshing process

mt 15 meshing

18. Mesh

After the meshing process is finished the mesh will appear in the 3D graphics window. The mesh used in this tutorial is created for demonstration purposes only, and its resolution should be considerably finer in real case scenario.

  1. Click Fit View to zoom the geometry

mt 16 mesh view

19. Merge Boundaries - Impeller and Shaft (I)

In order to simplify the definition of boundary conditions, we will merge the shaft and propeller boundaries into a single boundary.

  1. Hold CTRL key and select impeller and shaft boundaries

  2. On the impeller boundary select Options

  3. Choose Merge operation from the dropdown menu

mt 17 merge boundaries impeller and shaft 1

20. Merge Boundaries - Impeller and Shaft (II)

  1. Make sure you have selected impeller and shaft boundaries

  2. Click Merge Boundaries to confirm the operation

mt 18 merge boundaries impeller and shaft 2

21. Merge Boundaries - Impeller and Shaft (III)

  1. Rename newly created boundary from impeller_merged to impeller

  2. Change impeller’s boundary type to wall

mt 18 merge boundaries impeller and shaft 3

22. Split Baffles

Even though we requested the creation of baffles for the rotating_zone, two sides of the baffle can still share some common nodes. In order to make sure that each side has its own nodes, we need to perform the Split Baffles operation on the mesh. This is a very important step when using dynamic mesh model.

  1. Expand Options of the default region

  2. Select Split Baffles from the drop-down list

mt 19 split baffles

23. Create Mesh Interface

In the mesh setup, we requested creating baffles for rotating_zone, so that it can be a slip surface for the dynamic mesh. Now we will create the interface between the baffles.

  1. Hold CTRL key and select rotating_zone and rotating_zone_slave

  2. Click Create Arbitrary Interface

mt 20 create mesh interface 1

24. Setup Solver - Inter

We will use the Inter (interFoam) solver. This solver is able to model two-phase flow with free surface and supports dynamic mesh capabilities.

  1. Go to Setup panel

  2. Select Transient filter

  3. Select Dynamic Mesh model filter

  4. Pick Inter (interFoam) solver

  5. Select solver

mt 23 setup solver

25. Dynamic Mesh

We will apply a rotational speed of 2 revolutions per second to the zone with the impeller. Due to the orientation of our geometry, our rotation axis will be the -Z-axis of the global coordinate system.

  1. Go to Dynamic mesh panel

  2. Select Rigid type

  3. Check Move selected zone

  4. Make sure rotating_zone is selected as Cell Zone

  5. Expand Motion options

  6. Set Axis \({\sf [-]}\)00-1

  7. Set rotational speed Omega \({\sf [rad/s]}\)12.56

mt 24 dynamic mesh

26. Turbulence

For turbulence modeling we will use \(Realizable \; k{-} \varepsilon\) model.

  1. Go to Turbulence panel

  2. Select RANS turbulence formulation

  3. Select \(Realizable \; k{-} \varepsilon\) model

mt 25 turbulence

27. Boundary Conditions - Impeller (Flow)

We need to make sure that impeller velocity is taken from the properties of the rotating zone. For this purpose, we need to apply the Moving Wall Velocity boundary condition.

  1. Go to Boundary Conditions setup

  2. Select impeller boundary

  3. Change velocity type to Moving Wall Velocity

mt 26 bc impeller flow

28. Geometry - Initial Conditions Patch

As an initial state, we want the mixing tank to be partly filled with water. For this purpose, we need to create geometry to indicate the initial water location.

  1. Go to Geometry panel

  2. Click Create Cylinder

  3. Rename cylinder_1 to water_patch

  4. 5 Define cylinder origin, length, and radius
    Origin \({\sf [m]}\)00-0.18
    Length \({\sf [m]}\)0.45
    Radius \({\sf [m]}\)0.6

mt 27 geometry initial conditions patch

29. Initial Conditions - Patch

For initial conditions, we will leave all the default values, except inside the water patch, where the water phase fraction will be different.

  1. Go to Initial Conditions panel

  2. Switch to Patch tab

  3. Select water_patch geometry

  4. Enable initialization on water_patch

  5. Expand Fields list

  6. Select \(\alpha_{phase1}\) fraction for initialization

  7. Set \(\alpha_{phase1}\) to 1

mt 28 initial conditions patch

30. Run - Time Control

We will now adjust the time controls in order to capture the motion of the moving mesh in the output files. We will also enable automatic time step control for the simulation with reduced Courant number for better convergence.

  1. Go to Run panel

  2. Set Simulation Time [s] to 1

  3. Change Time Stepping to Automatic

  4. Set initial time step, time step limit and Courant number accordingly
    Initial \(\Delta t\) \({\sf [s]}\)5e-03
    Max \(\Delta t\) \({\sf [s]}\)1e-02
    Max Co \({\sf [-]}\)0.5

mt 29 run time controls

31. Run - Output

Now we just have to specify the frequency of writing results to the disk and start the simulation.

  1. Switch to Output panel

  2. Set Write Control Interval [s] to 1e-02

mt 30 run output

32. Run - CPU

To speed up the calculation process increase the number of CPUs basing on your PC capability. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for 2 processors: 30 minutes

  1. Switch to CPU tab

  2. Use parallel mode

  3. Increase the Number of processors

  4. Click Run Simulation button

mt 30 run cpu

33. Residuals

When the simulation is finished we should see a similar residual plot.

mt 30 residuals

34. Calculate Additional Fields

When the simulation is finished we want to calculate additional flow variables to use later for postprocessing.

  1. Go to Calculate panel

  2. Select Full Time Range

  3. Select Vorticity field

  4. Click Calculate

mt 28 calculate

35. Start Postprocessing - ParaView

Start ParaView when the simulation is finished. Optionally you can start ParaView when the simulation is still in progress to observe the intermediate results.

  1. Go to Postprocessing panel

  2. Start ParaView

mt 29 start postprocessing paraview

36. ParaView - Load Results

After opening ParaView, we have to load the results of the simulation.

  1. Select your case mixing_tank.foam

  2. Click Apply

  3. Click Last Frame

  4. Click Rescale to Data Range

  5. After rescale the contour will be shown in the 3D window.

mt paraview 1

37. ParaView - Coloring (I)

We can change the coloring scheme in ParaView to have nicer colors.

  1. Click Edit Color Map from the menu placed on the left side, if the panel is not already shown.

  2. Select Choose Preset from the Color Map Editor placed by default on the right side of the ParaView

mt paraview 2

38. ParaView - Coloring (II)

We can now select a new Color Preset.

  1. Expand Advanced Options

  2. Choose Blue to Red Rainbow preset

  3. Apply changes

  4. Close Choose Preset window

mt paraview 3

39. ParaView - Coloring (III)

To use the same color preset for all variables, we will save the current choice.

  1. Click Save current color map settings values as default for all arrays

mt paraview 3 1

40. ParaView - Display Water Surface (I)

We will now plot the water surface colored by the water height.

  1. Create Contour

  2. Select phase fraction alpha.phase1 field as a contour variable

  3. Define water surface threshold at 0.01

  4. Click Apply

mt paraview 4 1

41. ParaView - Display Water Surface (II)

  1. Select contour coloring variable p_rgh

After change the coloring variable and opacity the contour will be shown in the 3D window. Note that the pressure on the water surface is constant.

mt paraview 6

42. ParaView - Calculator (I)

  1. Select mixing_tank.foam

  2. Clcik Calculator

mt paraview 7

43. ParaView - Calculator (II)

  1. Change name to magVorticity

  2. Write the formula mag(vorticity)

  3. Click Apply

mt paraview 8

44. ParaView - Create Contour (I)

  1. Select Calculator 1

  2. Create Contour

mt paraview 9

45. ParaView - Create Contour (II)

  1. Select magVorticity as a contour variable

  2. Set contour value to 30

  3. Click Apply

mt paraview 10

46. ParaView - Create Contour (III)

  1. Select contour coloring variable p_rgh

mt paraview 11

47. ParaView - Load geometry (I)

  1. Select mixing_tank.foam

  2. Click Open

mt paraview 12

48. ParaView - Load geometry (II)

  1. Click mixing_tank

  2. Select mixing_tank.foam from file selection dialog

  3. Click OK

mt paraview 13

49. ParaView - Load geometry (III)

  1. Select impeller and walls zones to plot

  2. Click Apply

mt paraview 14

50. ParaView - Load geometry (IV)

  1. Set Coloring to Solid Color

  2. Set the opacity to 0.3

mt paraview 15

51. ParaView - Results

The results are displayed in the graphics window

mt paraview 16