Back to all tutorials

# Mixing Tank - CFD Simulation CFD Software Tutorial

## 1. Introduction

In this tutorial, we will demonstrate how to use Dynamic Mesh to model rotating components. We will simulate the rotation of an impeller in a cylindrical tank partially filled with water. The impeller is located within the inner cylinder mesh zone and rotates inside the tank’s larger domain. At the sliding mesh interface, which links the rotating and stationary mesh sections, data interpolation occurs. This tutorial uses a 2-phase Volume of Fluid (VoF) simulation to indicate a free surface vertex resulting from the rotation of the impeller.

SimFlow is a general purpose CFD Software

## 3. Create Case

Open SimFlow and create a new case named mixing tank

1. Click
2. Provide name mixing tank
3. Click to open a new case

## 4. Import Geometry

1. Click
2. Select geometry file impeller.stl.gz
3. Click

## 5. 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

## 6. Geometry - Impeller

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

1. Click to zoom the geometry

## 7. 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

## 8. 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

## 9. 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

## 10. 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

## 11. 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

## 12. Meshing Properties - Shaft

We need to also mesh the shaft geometry.

1. Select shaft
2. Check Mesh Geometry

## 13. 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
AxisZ
Origin $${\sf [m]}$$-0.18
Length $${\sf [m]}$$0.9
Radius $${\sf [m]}$$0.6

## 14. Base Mesh - Mesh

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

Axial Division30
Central Division15

## 15. Base Mesh - View

We can preview the Base Mesh in the graphics window.

## 16. 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

## 17. 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

## 18. Meshing

Everything is now set up for meshing.

1. Go to Mesh tab
2. Click button to start meshing process

## 19. 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 to zoom the geometry

## 20. 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

## 21. Merge Boundaries - Impeller and Shaft (II)

1. Make sure you have selected impeller and shaft boundaries
2. Click to confirm the operation

## 22. Merge Boundaries - Impeller and Shaft (III)

1. Rename newly created boundary from impeller_merged to impeller
2. Change impeller’s boundary type to wall

## 23. 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

## 24. 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

## 25. 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 filter
3. Select Dynamic Mesh model filter
4. Pick Inter (interFoam) solver
5. solver

## 26. 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

## 27. 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

## 28. Operating Conditions

Incompressible solver like an Inter, operates on relative pressure (more here). In the incompressible Navier-Stokes equation, pressure is only related to the gradient and has no specific bounds. The pressure distribution can be determined by solving the N-S equation, but the exact value of pressure is irrelevant as long as the pressure difference between two points is the same.

To define precise value, it is necessary to define the pressure at a specific point. While the pressure at inlet or outlet boundaries is usually defined, if the domain is enclosed, a reference point must be established within the domain.

1. Go to Operating Conditions panel
2. Change the Location to Point
3. Set Point0.400.5

## 29. 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

## 30. 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

## 31. 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

## 32. 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

## 33. 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

## 34. Run - CPU

To speed up the calculation process, take advantage of parallel computing and increase the number of CPUs based on your PC’s capability. The free version allows you to use only one processor (serial mode). To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for serial mode: 50 minutes

1. Switch to CPU tab
2. Click button

## 35. Residuals

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

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

## 37. 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

## 38. ParaView - Load Results

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

2. Click
3. Click Last Frame
4. Click Rescale to Data Range
5. After rescale the contour will be shown in the 3D window.

## 39. 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

## 40. ParaView - Coloring (II)

We can now select a new Color Preset.

2. Choose Blue to Red Rainbow preset
3. changes
4. Choose Preset window

## 41. 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

## 42. 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

## 43. 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.

## 44. ParaView - Calculator (I)

1. Select mixing_tank.foam
2. Clcik Calculator

## 45. ParaView - Calculator (II)

1. Change name to magVorticity
2. Write the formula mag(vorticity)
3. Click

## 46. ParaView - Create Contour (I)

1. Select Calculator 1
2. Create Contour

## 47. ParaView - Create Contour (II)

1. Select magVorticity as a contour variable
2. Set contour value to 30
3. Click

## 48. ParaView - Create Contour (III)

1. Select contour coloring variable p_rgh

## 49. ParaView - Load geometry (I)

1. Select mixing_tank.foam
2. Click

## 50. ParaView - Load geometry (II)

1. Click mixing_tank
2. Select mixing_tank.foam from file selection dialog
3. Click

## 51. ParaView - Load geometry (III)

1. Select impeller and walls zones to plot
2. Click

## 52. ParaView - Load geometry (IV)

1. Set Coloring to Solid Color
2. Set the opacity to 0.3

## 53. ParaView - Results

The results are displayed in the graphics window

## 54. Advanced Postprocessing with ParaView

This concludes the tutorial, covering all the aspects we intended to showcase. For a finely tuned presentation of the results, you may take advantage of the more advanced features.

In ParaView, you can display streamlines, contour plots, vector fields, line or time plots, calculating volume or surface integrals and create animations.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, Paraview CFD Tutorial - Advanced Postprocessing in ParaView, in which we demonstrate some of the most commonly used post-processing techniques.