Back to all tutorials

# Static Mixer - CFD Simulation SimFlow Tutorial

## 1. Create Case

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

1. Go to panel

2. Provide name static_mixer

3. Click

## 2. Import Geometry

1. Click

2. Select geometry file staticMixer.stl

3. Click

## 3. Imported Geometry Units

The STL format does not contain the unit information which are defined during the geometry export. If we do not know the exported unit, we can estimate it based on the total size of the model. It is displayed next to Geometry size label. In our case, the default unit meter is correct.

1. To confirm default unit meter, press

## 4. Geometry - Static Mixer

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

1. Click to zoom in on the geometry.

## 5. Meshing Parameters - Static Mixer

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

1. Go to panel

2. Select geometry

3. Enable Mesh Geometry

## 6. 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 tab

2. Choose base mesh type
Base Mesh Type Cylinder

3. Set the cylinder axis
Axis Z

4. Set the size of the cylinder base mesh:
Length $${\sf [m]}$$0.12
Radius $${\sf [m]}$$0.0154

5. 67 Set the following parameters accordingly
Axial Division100
Central Division21

## 7. 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

## 8. 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 the blades.

1. Switch to tab

2. Specify the location of the material point inside staticMixer
Material Point000.1

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

## 9. Start Meshing

1. Go to tab

2. Start the meshing process with button

## 10. Mesh

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

1. Click to zoom in the mesh

## 11. Check Mesh

Check the mesh quality and cells statistics.

1. Expand the list next to default region

2. Select option

3. Checks summary will be displayed on the command window. It also shows checking criteria.

## 12. 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 panel

2. Select

3. Set the origin and box dimensions
Origin $${\sf [m]}$$-0.020-5e-03
Dimensions $${\sf [m]}$$0.050.021e-02

## 13. Inlet Boundary (I)

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

1. Go to panel

2. Expand the list next to inlet boundary

3. Select option

1. Check box_1

2. Click

## 15. Inlet Boundary (III)

1. Change the names accordingly
inletinlet_scalar0
inlet_in_box_1inlet_scalar1
(double click on the name to change it)

## 16. 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

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

## 17. 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 boundary

2. Expand the list

3. Select option

## 18. 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 layer’s number accordingly
Number of Layers37

2. Set the thickness accordingly
Thickness0.05

3. Click

## 19. Select Solver - PIMPLE

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

1. Go to panel

2. Filter the solvers by flow

3. Pick PIMPLE (pimpleFoam) solver from the list

4. solver

## 20. Turbulence

In this tutorial, we will consider a laminar flow.

1. Go to panel

2. Make sure the Laminar model is selected

## 21. 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 panel

2. Click on

3. Select the water

4. Click

## 22. 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 panel

2. Press button

3. Click on to expand options list

4. Check the Custom Diffusivity

5. Set the diffusivity
Diffusivity $${\sf [m^2/s]}$$2e-09

## 23. Boundary Conditions - Inlet Scalar 0 (Flow)

We will define the constant inlet velocity for both inlets.

1. Go to panel

2. Select boundary

3. Set the boundary character
inlet_scalar0 Velocity Inlet

4. Change the type and value of the velocity
UTypeFixed Value
UValue $${\sf [m/s]}$$000.15

## 24. Boundary Conditions - Inlet Scalar 1 (Flow)

Repeat these steps for the second inlet.

1. Select boundary

2. Set the boundary character
inlet_scalar1 Velocity Inlet

3. Change the type and value of the velocity
UTypeFixed Value
UValue $${\sf [m/s]}$$000.15

## 25. Boundary Conditions - Inlet Scalar 1 (Scalars)

For the inlet_scalar1 boundary set the inflow phase value.

1. Switch to tab

2. Set the value of scalar1 to:
scalar1Inlet Value $${\sf [-]}$$1

## 26. 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 panel

2. Set the velocity
U 000.15

## 27. 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 panel

2. Switch to tab

3. Select

4. Expand list

5. Select all available options
Fields p U scalar1

6. Normal is defined along Z axis. Set the point to:
Point $${\sf [m]}$$000.05

## 28. Monitors - Create Slice (II)

Create the next slice above the mixer.

1. Expand list next to the slice_1

2. Click

3. Click on to expand options list

4. Change the point coordinate
Point [m] 000.1

## 29. Monitors - Create Slice (III)

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

1. Expand list next to the slice_2

2. Click

3. Click on to expand options list

4. Change the point coordinate
Point [m] 000.15

## 30. Run - Time Controls

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

1. Go to panel

2. Set the simulation time
Simulation Time [s] 3

3. Set the time stepping
Time Stepping $$\Delta t[s]$$ 1e-03

## 31. 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 tab

2. Set the write control interval
Write Control Interval [s] 0.1

## 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: 20 minutes

1. Switch to tab

2. Use parallel mode

3. Increase number of CPUs for the computation
Number of processors 2

4. Click button

## 33. 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

2. Changed displayed results by selecting

3. To adjust color range to actually displayed data click

4. Play with animation buttons to view the results of the analysis.

## 34. Postprocessing - ParaView

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

1. Go to panel

2. Click on

## 35. ParaView - Load Results

Load the results into the program.

1. Select static_mixer.foam

2. Click to load results into ParaView

3. After loading results they will be shown in the 3D graphic window

4. Click on a from the top menu and select

## 36. ParaView - Streamline (I)

We can visualize the flow by displaying the streamlines.

2. Set the maximum streamline length
Maximum Streamline Length 0.3

3. Change a seed type
Seed Type Point Source

4. Type the center coordinate and radius of the sphere:
Center000

5. Uncheck the Show Sphere

6. Increase the number of points
Number of Points 200

7. Click

8. Select the scalar1 from the list

9. Play with animation buttons to track the results of the analysis.

## 37. 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
Opacity 0.3