# Cylinder Cooling - CFD Simulation

Source: https://help.sim-flow.com/tutorials/cylinder-cooling
Last updated: 2026-10-14

[Video](https://help.sim-flow.com/tutorials/images/cylinder-cooling.mp4)

## 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) problem. As a result, we will track the temperature fields for both the cylinder and the fluid over time.

## 2. Download SimFlow

SimFlow is a general-purpose [CFD Software](https://sim-flow.com/download/cfd-simulation-software/)

To follow this tutorial, you will need the SimFlow free version. You may download it via the following link:
[Download SimFlow](https://sim-flow.com/download-simflow/)

## 3. Create Case

Open SimFlow and create a new case named *cylinder cooling*

1. Click **New**
2. Provide name `cylinder cooling`
3. Click **Create** to open a new case

![simflow-launcher](https://help.sim-flow.com/tutorials/images/launcher-cylinder_cooling.png)

## 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 \({\sf [m]}\)*`0``0``-0.25`
   *Length \({\sf [m]}\)*`0.5`
   *Radius \({\sf [m]}\)*`0.05`

![cc 2 geometry](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-2-geometry.png)

## 5. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-3-geometry.png)

## 6. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-4-meshing-properties-cylinder.png)

## 7. Base Mesh - Geometry and Mesh

We will define the base mesh now.

1. Go to the *Base* tab
2. Choose *Plate* Mesh Type
3. Define base mesh minimum and maximum extent
   *Min \({\sf [m]}\)*`-1``-0.4`
   *Max \({\sf [m]}\)*`1``0.4`
4. Define division along each axis
   *Division*`200 80`

![cc 5 base mesh geometry and mesh](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-5-base-mesh-geometry-and-mesh.png)

## 8. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-6-base-mesh-boudaries.png)

## 9. Material Point - Fluid

Now we will define a material point outside the cylinder geometry.

1. Go to *Point* tab
2. Set location of the material point
   *Material Point*`0``0.2``0`

![cc 7 material point fluid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-7-material-point-fluid.png)

## 10. Meshing - Fluid Region

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

![cc 8 meshing fluid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-8-meshing-fluid.png)

## 11. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-9-mesh-fluid.png)

## 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 **OK** button

![cc 10 create subregion fluid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-10-create-subregion-fluid.png)

## 13. Material Point - Solid

Now we will define a 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 Point*`0``0``0`

![cc 11 material point solid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-11-material-point-solid.png)

## 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 **Mesh** button

![cc 12 meshing solid region](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-12-meshing-solid-region.png)

## 15. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-13-mesh-solid-region.png)

## 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 **OK** button

![cc 14 create subregion solid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-14-create-subregion-solid.png)

## 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

![cc 15 create region interface](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-15-create-region-interface.png)

## 18. Check Mesh Boundaries

Verify the mesh by reviewing the boundary names and types.

1. Ensure that each boundary is correctly named and assigned the appropriate type

![cc 14 mesh boundaries](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-14-mesh-boundaries.png)

## 19. Simulation Type

We want to analyze a 2D simulation of a cooling cylinder. For this purpose, we will use a transient conjugate heat transfer simulation.

![Simulation Panel](https://help.sim-flow.com/assets/images/go-to-simulation-panel@2x.png)

![Step 1](https://help.sim-flow.com/assets/images/solvers-selection/chtMultiRegionFoam/01_heat_transfer@2x.png)

![Step 2](https://help.sim-flow.com/assets/images/solvers-selection/chtMultiRegionFoam/02_cht@2x.png)

![Step 3](https://help.sim-flow.com/assets/images/solvers-selection/chtMultiRegionFoam/03_transient@2x.png)

![Step 4](https://help.sim-flow.com/assets/images/solvers-selection/chtMultiRegionFoam/04_apply@2x.png)

## 20. Thermophysical Properties - Fluid (I)

We will now define the thermodynamic properties of the fluid material.

1. Go to *Thermo* panel
2. Select *fluid* region
3. Select *Constant Density*
4. Click **Material Database** button

![cc 15 thermo fluid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-15-thermo-fluid.png)

## 21. Thermophysical Properties - Fluid (II)

1. Select *water* material
2. Click **Apply**

![cc 16 material database water](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-16-material-database-water.png)

## 22. Thermophysical Properties - Solid (I)

We will now define the thermodynamic properties of the solid material.

1. Select *solid* region
2. Select *Constant Density*
3. Click **Material Database** button

![cc 17 thermo solid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-17-thermo-solid.png)

## 23. Thermophysical Properties - Solid (II)

1. Select *steel* material
2. Click **Apply**

![cc 18 material database steel](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-18-material-database-steel.png)

## 24. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-19-solution-pimple.png)

## 25. Operating Conditions

1. Go to *Operating Conditions* panel
2. Define gravitational acceleration
   *g \({\sf [m/s^2]}\)*`0``-9.81``0`

![cc 20 operating conditon gravitational acceleration](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-20-operating-conditon-gravitational-acceleration.png)

## 26. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-21-boundary-conditions-refe-velocity-inlet.png)

## 27. Boundary Conditions - Inlet (Thermal)

1. Go to *Thermal* boundary conditions tab
2. Set the following parameters accordingly
   *Type*`Fixed Value`
   *Value \({\sf [K]}\)*`300`

![cc 22 boundary thermal fixed value](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-22-boundary-thermal-fixed-value.png)

## 28. Initial Conditions

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

![cc 23 initial condition solid](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-23-initial-condition-solid.png)

## 29. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-24-time-controls.png)

## 30. Run - Output

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

![cc 25 write control run](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-25-write-control-run.png)

## 31. 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](https://license.sim-flow.com/trial)

Estimated computation time for serial mode: 5 minutes

1. Switch to *CPU* tab
2. Click **Run Simulation** button

![run cpu serial](https://help.sim-flow.com/tutorials/images/run-cpu-serial.png)

## 32. Residuals

![cc 26 residuals](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-26-residuals.png)

## 33. Start Postprocessing with ParaView

1. Go to *Postprocessing* panel
2. Run *ParaView*

![cc 27 postptrocessing](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-27-postptrocessing.png)

## 34. ParaView - Load Results

Now we are loading results into 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-28-paraview-load-results.png)

## 35. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-29.png)

## 36. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-pv.png)

## 37. ParaView - Choose Preset (II)

1. Select *Choose Preset* from the Color Map Editor placed by default on the right side of 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/kolorowanka.png)

## 38. 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](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-33-paraview-temerature-run.png)

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

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

![cc 34](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-34.png)

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

1. Click *First Frame*
2. Click *Rescale to Custom Data Range*
3. Set maximum value
   *Max*`305`
4. Click **Rescale**
5. Click *Play*

![cc 35 paraview run](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-35-paraview-run.png)

## 41. ParaView - Results

![cc 36 tourbulence](https://help.sim-flow.com/tutorials/images/cylinder-cooling/cc-36-tourbulence.png)

## 42. 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, calculate 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 postprocessing techniques.

[Paraview CFD Tutorial - Advanced Postprocessing in ParaView](https://www.youtube.com/watch?v=5M6VgXyHB60&list=PLy7xPqn9xXckoD2gZgPpv8mrxillJ9PWU&index=21)