Back to all tutorials

# Cylinder Cooling - CFD Simulation CFD Software Tutorial

## 1. Introduction

In this tutorial, we will explore the process of cooling a steel cylinder using a stream of water. You will learn how to create a multi-region mesh, using a 2D mesh for simplification. This problem involves solving the interaction between a solid and a fluid as a conjugate heat transfer (CHT). As a result, we will track the temperature fields for both the cylinder and the fluid over time.

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:

## 3. Create Case

Open SimFlow and create a new case named cylinder cooling

1. Click
2. Provide name cylinder cooling
3. Click to open a new case

## 4. 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

## 5. Geometry - Cylinder

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

1. Click to zoom the geometry

## 6. Meshing Properties - Cylinder

1. Go to Hex Meshing panel
2. Click cylinder_1
3. Select Mesh Geometry
4. Select Create Boundary Layer Mesh

## 7. 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

## 8. Base Mesh - Boundaries

1. Define boundary names accordingly
X- inlet
X+ outlet
2. Define the following boundary types accordingly
Y- wall
Y+ wall

## 9. 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

## 10. Meshing - Fluid Region

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

## 11. Mesh - Fluid Region

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

1. Click to zoom the geometry
2. Click to orient view plane

## 12. 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 button

## 13. 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

## 14. 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 button

## 15. Mesh - Solid Region

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

1. Click to zoom the geometry

## 16. 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 button

## 17. 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

## 18. Select Solver - CHT Multi Region

1. Go to Setup panel
2. Select filter
3. Select Heat Transfer model filter
4. Pick CHT Multi Region (chtMultiRegionFoam)
5. solver

## 19. 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 button

## 20. Thermophysical Properties - Fluid (II)

1. Select water material
2. Click

## 21. Thermophysical Properties - Solid (I)

We will define now the thermodynamic properties of solid material.

1. Select solid region
2. Select Constant Density
3. Click button

## 22. Thermophysical Properties - Solid (II)

1. Select steel material
2. Click

## 23. Solution - Solvers

1. Go to Solution panel
2. Go to the Pimple tab
3. Increase the number of Correctors to 2

## 24. Operating Conditions

1. Go to Operating Conditions panel
2. Define gravitational acceleration
g $${\sf [m/s^2]}$$0-9.810

## 25. 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

## 26. Boundary Conditions - Inlet (Thermal)

1. Go to Thermal boundary conditions tab
2. Set the following parameters accordingly
TypeFixed Value
Value $${\sf [K]}$$300

## 27. Initial Conditions

1. Go to Initial Conditions panel
2. Select solid region
3. Set temperature T to 400

## 28. 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

## 29. Run - Output

1. Switch to Output panel
2. Set Write Control Interval [s] to 5

## 30. 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: 5 minutes

1. Switch to CPU tab
2. Click button

## 32. Start Postprocessing with ParaView

1. Go to Postprocessing panel
2. Run ParaView

## 33. ParaView - Load Results

Now we are loading results into the ParaView.

1. Select cylinder_cooling.foam
2. Click to load results into ParaView
3. After loading results they will be shown in the 3D graphic window

## 34. 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

## 35. ParaView - Choose Preset (I)

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

## 36. 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. changes
5. Choose Preset window
6. Set Number of Table Values to 20
7. Click Save current color map settings values as default for all arrays

## 37. 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

## 38. ParaView - Display Temperature Contour (II)

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

## 39. ParaView - Display Temperature Contour (III)

1. Click First Frame
2. Click Rescale to Custom Data Range
3. Set maximum value
Max305
4. Click
5. Click Play

## 41. 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.