Back to all tutorials

Cylinder Cooling - 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 cylinder_cooling

  1. Go to New panel

  2. Provide name cylinder_cooling

  3. Click Create Case

cc 1 create case

3. Create Geometry - Cylinder

We need to create a cylindrical boundary for the domain. For this purpose, we will create a cylindrical geometry for later use in the meshing process.

  1. Go to Geometry panel

  2. Select Create Cylinder

  3. 4 Define origin, length, and radius of the cylinder accordingly
    Origin \({\sf [m]}\)00-0.25
    Length \({\sf [m]}\)0.5
    Radius \({\sf [m]}\)0.05

cc 2 geometry

4. Geometry - Cylinder

After creating a cylindrical boundary, it will appear in the 3D panel.

  1. Click Fit View to zoom the geometry

cc 3 geometry

5. Meshing Properties - Cylinder

  1. Go to Hex Meshing panel

  2. Click cylinder_1

  3. Select Mesh Geometry

  4. Select Create Boundary Layer Mesh

cc 4 meshing properties cylinder

6. Base Mesh - Geometry and Mesh

We will define the base mesh now.

  1. Go to the Base tab

  2. Chose Plate Mesh Type

  3. Define base mesh minimum and maximum extend
    Min \({\sf [m]}\)-1-0.4
    Max \({\sf [m]}\)10.4

  4. Define division along each axis
    Division200 80

cc 5 base mesh geometry and mesh

7. Base Mesh - Boundaries

  1. Define boundary names accordingly
    X- inlet
    X+ outlet

  2. Define the following boundary types accordingly
    Y- wall
    Y+ wall

cc 6 base mesh boudaries

8. Material Point - Fluid

Now we will define material point outside the cylinder geometry.

  1. Go to Point tab

  2. Set location of the material point
    Material Point00.20

cc 7 material point fluid

9. Meshing - Fluid Region

  1. Go to Mesh tab

  2. Start the meshing process with Mesh button

cc 8 meshing fluid

10. Mesh - Fluid Region

After a few minutes of meshing the following mesh should appear.

  1. Click Fit View to zoom the geometry

  2. Click View XY to orient view plane

cc 9 mesh fluid

11. Create Sub-Region - Fluid

After creating the mesh, we have to make a sub-region - fluid.

  1. Go to Mesh panel

  2. Press Options button

  3. Select Make sub-region option

  4. Enter name fluid for the sub-region

  5. Click OK button

cc 10 create subregion fluid

12. Material Point - Solid

Now we will define material point for sub-region - solid.

  1. Go to Hex Meshing panel

  2. Go to Point tab

  3. Set location of the material point
    Material Point000

cc 11 material point solid

13. Meshing - Solid Region

Everything is set up now for the meshing of the solid region

  1. Go to Mesh tab

  2. Start the meshing process with Mesh button

cc 12 meshing solid region

14. Mesh - Solid Region

After a few minutes of meshing the following mesh should appear.

  1. Click Fit View to zoom the geometry

cc 13 mesh solid region

15. Create Sub-Region - Solid

After creating the mesh, we have to make a sub-region - solid.

  1. Go to Mesh panel

  2. Press Options button

  3. Select Make sub-region option

  4. Enter name solid for the sub-region

  5. Click OK button

cc 14 create subregion solid

16. Create Region Interface

Two mesh regions are not coupled until you create a region interface. It will be further used to define which information is exchanged between regions.

  1. Select Solid type for solid region

  2. Make sure you have selected wall type for cylinder_1

  3. Hold CTRL key and select cylinder_1 in fluid and cylinder_1 in solid

  4. Click Create Region Interface icon

cc 15 create region interface

17. Select Solver - CHT Multi Region

  1. Go to Setup panel

  2. Select Transient filter

  3. Select Heat Transfer model filter

  4. Pick CHT Multi Region

  5. Select solver

cc 14 solver section

18. Thermophysical Properties - Fluid (I)

We will define now the thermodynamic properties of fluid material.

  1. Go to Thermo panel

  2. Select fluid region

  3. Select Constant Density

  4. Click Material Database button

cc 15 thermo fluid

19. Thermophysical Properties - Fluid (II)

  1. Select water material

  2. Click Apply

cc 16 material database water

20. Thermophysical Properties - Solid (I)

We will define now the thermodynamic properties of solid material.

  1. Select solid region

  2. Select Constant Density

  3. Click Material Database button

cc 17 thermo solid

21. Thermophysical Properties - Solid (II)

  1. Select steel material

  2. Click Apply

cc 18 material database steel

22. Solution - Solvers

  1. Go to Solution panel

  2. Go to the Pimple tab

  3. Increase the number of Correctors to 2

cc 19 solution pimple

23. Operating Conditions

  1. Go to Operating Conditions panel

  2. Define gravitational acceleration
    g \({\sf [m/s^2]}\)0-9.810

cc 20 operating conditon gravitational acceleration

24. Boundary Conditions - Inlet (Flow)

  1. Go to Boundary Conditions panel

  2. Select inlet

  3. Change character to velocity inlet

  4. Define inlet velocity
    Reference Value \({\sf [m/s]}\)0.1

cc 21 boundary conditions refe velocity inlet

25. Boundary Conditions - Inlet (Thermal)

  1. Go to Thermal boundary conditions tab

  2. Set the following parameters accordingly
    TypeFixed Value
    Value \({\sf [K]}\)300

cc 22 boundary thermal fixed value

26. Initial Conditions

  1. Go to Initial Conditions panel

  2. Select solid region

  3. Set temperature T to 400

cc 23 initial condition solid

27. Run -Time Control

  1. Go to Run panel

  2. Set Simulation Time [s] to 200

  3. Change Time Stepping to Automatic

  4. Set initial and maximum time step accordingly
    Initial \(\Delta t\) \({\sf [s]}\)0.2
    Max \(\Delta t\) \({\sf [s]}\)0.2

cc 24 time controls

28. Run - Output

  1. Switch to Output panel

  2. Set Write Control Interval [s] to 5

cc 25 write control run

29. 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: 3 minutes

  1. Switch to CPU tab

  2. Use parallel mode

  3. Increase the Number of processors

  4. Click Run Simulation button

cc 25 run cpu

30. Residuals

cc 26 residuals

31. Start Postprocessing with ParaView

  1. Go to Postprocessing panel

  2. Run ParaView

cc 27 postptrocessing

32. ParaView - Load Results

Now we are loading results into the ParaView.

  1. Select cylinder_cooling.foam

  2. Click Apply to load results into ParaView

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

cc 28 paraview load results

33. ParaView - Change Background

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

  1. Click Load a Color Palette

  2. Select White Background

cc 29

34. ParaView - Choose Preset (I)

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

cc pv

35. ParaView - Choose Preset (II)

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

  2. Search rainbow

  3. Choose Blue to Red Rainbow preset.

  4. Apply changes

  5. Close Choose Preset window

  6. Set Number of Table Values to 20

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

kolorowanka

36. ParaView - Display Temperature Contour (I)

  1. Select contour coloring variable to T

  2. Click Last Frame

  3. Click Rescale to Data Range

  4. Click First Frame

  5. Click Play

cc 33 paraview temerature run

37. ParaView - Display Temperature Contour (II)

After applying changes the contour will be shown in the 3D window.

cc 34

38. ParaView - Display Temperature Contour (III)

  1. Click First Frame

  2. Click Rescale to Custom Data Range

  3. Set maximum value
    Max305

  4. Click Rescale

  5. Click Play

cc 35 paraview run

39. ParaView - Results

cc 36 tourbulence