Static Mixer

1. Create Case

After opening SimFlow, we will create a new case named static_mixer

1. Go to New panel
2. Provide name static_mixer
3. Click Create Case

2. Import Geometry

Firstly we need to Download Geometry: staticMixer.stl

1. Click Import Geometry
2. Select geometry file staticMixer.stl
3. Click Open

3. Geometry - Static Mixer

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

1. Click Fit View to zoom in on the geometry.

4. Meshing Parameters - Static Mixer

In order to create the mesh, we need to enable meshing for the imported geometry.

1. Go to Hex Meshing panel
2. Select staticMixer geometry
3. Enable Mesh Geometry

5. Base Mesh - Domain

The imported geometry represents only the mixer blades. By using a cylinder base mesh we will define the pipe housing.

1. Switch to Base tab
2. Select the Cylinder as a Base Mesh Type
3. Set the cylinder axis along Z axis
4. Set the size of the cylinder base mesh:
Length [m] 0.12
Radius [m] 0.0154
5, 6, 7. Set the following parameters accordingly
Radial Division 12
Axial Division 90
Central Division 22

6. Base Mesh - Boundaries

We need to assign individual names to each side of the base mesh. This will allow us to apply different conditions to each side.

1. Choose boundary names accordingly

First Disk inlet
Second Disk outlet
Cylinder wall (double click on the name to type)

2. Choose boundary types accordingly

First Disk patch
Second Disk patch
Cylinder wall

7. Material Point

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are considering flow inside the cylinder we need to place the material point outside of the blades.

1. Switch to Point tab
2. Specify the location of the material point inside staticMixer geometry

Material Point 0 0 0.1

You can specify the point location from the 3D view. Hold the Ctrl key and drag the arrows to the destination.

8. Start Meshing

1. Go to Mesh tab
2. Start the meshing process with Mesh button

9. Mesh

After the meshing process is finished the mesh should appear in the graphics window.

1. Click Fit View to zoom in the mesh

10. Check Mesh

Check the mesh quality and cells statistics.

1. Expand the Options list next to default region
2. Select Check option
3. Checks summary will be displayed on the command window. It also shows checking criteria.

11. Create Geometry - Box

To provide two different fluids into the mixer, we need to split the inlet boundary into two separate ones. We will use additional geometry to mark the selection for the extraction.

1. Go to Geometrypanel
2. Select Create Box
3. Set the origin and box dimensions

Origin[m] -0.02 0 -5e-03
Dimensions [m] 0.05 0.02 1e-02

12. Inlet Boundary (I)

Now, using the new geometry we will extract a new boundary from the original inlet.

1. Go to MESHpanel
2. Expand the Options list next to inlet boundary
3. Select Extract From option

13. Inlet Boundary (II)

1. Check box_1
2. Click Extract

14. Inlet Boundary (III)

1. Change the names accordingly

inlet to inlet_scalar0
inlet_in_box_1 to inlet_scalar1

(double click on the name to change it)

15. Inlet Boundary (IV)

As the results of the extraction, we should receive two separate inlet boundaries. Both boundaries can be distinguished by the different colors.

1. Expand Graphics Objects List
2. Uncheck the icon next to the Geometries to hide all geometry and press the Esc key
3. Check if the inlet boundaries are colored differently

16. Domain Modification (I)

With SimFlow, the user can also modify the existing mesh domain. We can extend the volume by extruding a specific boundary. For the purpose of this tutorial, we will extend the mixer tube by extruding the outflow face.

1. Select outlet boundary
2. Expand the Options list
3. Select Extrude option

17. Domain Modification (II)

The outlet boundary will be extended by 5 cm and additional mesh will be split into 37 cells in the extrusion direction.

1. Set the number of layers to 37
2. Set the thickness to 0.05
3. Click Extrude

18. Select Solver

We want to analyze the incompressible turbulent flow. For this purpose, we will use the PIMPLE (pimpleFoam) solver.

1. Go to SETUP panel
2. Filter the solvers by Incompressible flow
3. Pick PIMPLE (pimpleFoam) solver from the list
4. Select solver

19. Turbulence

In this tutorial, we will consider a laminar flow.

1. Go to Turbulence panel
2. Make sure the Laminar model is selected

20. Transport Properties

In order to define water properties, we go to the transport properties panel. We will use predefined fluid properties from the material database.

1. Go to Transport Properties panel
2. Click on Material Database
3. Select the water
4. Click Apply

21. Passive Scalar

We will use passive scalar to simulate the mixing of two different fluids. Passive scalar adds an additional transport equation to the system of governing equations. Note, the passive scalar does not influence the flow itself but only introduces a marker for tracing fluid transport. The scalar takes a value between 0 and 1 (0 represents clear water, and 1 represents water with air dissolved in it). To control scalar properties we can define either the Schmidt number or custom diffusivity. In our case, we will define custom diffusivity equal 2.0e-09 which corresponds to the water-air mixture.

1. Go to Passive Scalars panel
2. Press Add new passive scalar Equations button
3. Click on scalar1 to expand options list
4. Check the Custom Diffusivity
5. Set the Diffusivity [m2/s] equal to 2e-09

22. Boundary Conditions – Inlet Scalar 0 (Flow)

We will define the constant inlet velocity for both inlets.

1. Go to Boundary Conditions panel
2. Select inlet_scalar0 boundary
3. Set the Velocity Inlet character
4. Change the type and value of the velocity
U Type Fixed Value
U Value [m/s] 0 0 0.15

23. Boundary Conditions – Inlet Scalar 1 (Flow)

Repeat these steps for the second inlet.

1. Select inlet_scalar1 boundary
2. Set the Velocity Inlet character
3. Change the type and value of the velocity
U Type Fixed Value
U Value [m/s] 0 0 0.15

24. Boundary Conditions – Inlet Scalar 1 (Scalars)

For the inlet_scalar1 boundary set the inflow phase value.

1. Switch to Scalars tab
2. Set the value of scalar1 to:
scalar1 Inlet Value [-] 1

The rest of the boundary conditions leave as default.

25. Initial Conditions

Before we start simulation we need to define the initial conditions. We will specify a constant velocity equal to 0.15 m/s which corresponds to the inlet velocity.

1. Go to Initial Conditions panel
2. Set the velocity U to 0 0 0.15

26. Monitors – Create Slice (I)

During calculation, we can observe intermediate results on a section plane. To add sampling data on a plane we need to define plane properties and also select variables that will be sampled. Note that runtime post-processing can only be defined before starting calculations and can not be changed later on.

1. Go to Monitors panel
2. Switch to Sampling tab
3. Select Create Slice
4. ExpandFields list
5. Select all available options: p, U and scalar1
6. Normal is defined along Z axis. Set the point to:
Point [m] 0 0 0.05

27. Monitors – Create Slice (II)

Create the next slice above the mixer.

1. ExpandOptions list next to the slice_1
2. Click Duplicate
3. Click on slice_2 to expand options list
4. Change the point Z coordinate to 0.1

28. Monitors – Create Slice (III)

Duplicate the slice once again and move it to the vicinity of the outlet.

1. ExpandOptions list next to the slice_2
2. Click Duplicate
3. Click on slice_3 to expand options list
4. Change the point Z coordinate to 0.15

29. Run - Time Controls

Before running computations adjust the time controls in order to capture appropriate time scales of the flow features.

1. Go to RUN panel
2. Set the Simulation Time [s] to 3
3. Set the Time Stepping Δt[s] to 1e-03

30. Run - Output

We can control how often results should be saved on the hard drive. We will write the results at the interval of 0.1 seconds. Note, that only saved data will be available during postprocessing.

1. Switch to Output tab
2. Set the Interval [s] to 0.1
3. Click Run Simulation button

31. Results – Slice

Slices tab appears next to Residuals. Under this tab, we can preview results on the defined slice planes. The results preview is available during the calculation and we can track it on a regular basis. The newly calculated time step will be actualized automatically as long as the time selector points to the latest time step.
We want to check if the fluids are mixed at the end of the mixer. We will display scalar1 contribution at each slice in the mixer.

1. Change tab to Slice
2. Choose αmud field to display the mud phase
3. Click Adjust range to data to adjust color range to actually displayed data
4. Play with animation buttons to view the results of the analysis.

32. Postprocessing – ParaView

After computations are finished we can do complex visualization of our results with ParaView.

2. Click on Run ParaView

33. ParaView - Load Results

Load the results into the program.

1. Select static_mixer.foam
2. Click Apply to load results into ParaView
3. After loading results they will be shown in the 3D graphic window
4. Click on a Load a colour palette from the top menu and select White Background

34. ParaView – Streamline (I)

We can visualize the flow by displaying the streamlines.

1. Select Stream Tracer from top menu
2. Set the maximum streamline length to 0.3
3. Change Seed Type to Point Source
4. Type the center coordinate and radius of the sphere:
Center 0 0 0
Radius 0.016
5. Uncheck the Show Sphere
6. Increase the number of points to 200
7. Click Apply
8. Select the scalar1 from the list
9. Play with animation buttons to track the results of the analysis.

35. ParaView – Streamline (II)

To show the geometry together with the streamlines we will follow below steps:

1. Click on the eye next to static_mixer.foam
2. Select Solid Color from the list
3. Change the opacity to 0.3

This website uses cookies to offer you the best experience online. By continuing to use our website, you agree to the use of cookies.