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
Postprocessing for multi-region simulations require a newer version of the ParaView. For purpose of this tutorial we used ParaView 5.9.0. You can download the newest version of ParaView Download ParaView 5.9.0 .
To upgrade ParaView and use it with SimFlow follow these instructions .
Open SimFlow and create a new case named heat_exchanger
Go to New panel
Provide name heat_exchanger
Click Create Case button

3. Import Geometry - Heat Exchanger
4. 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 imported geometries. The size is displayed next to Geometry size label. In our case, the default unit meter is correct.
To confirm default unit meter, press OK

5. Geometry - Heat Exchanger
After importing geometry, it will appear in the 3D window. We will make the exchanger geometry transparent to see the interior of the heat exchanger.
Click Fit View to zoom the geometry
Hold the CTRL key and click exchanger wall
Select Display Properties

6. Change Opacity - Heat Exchanger
Select Opacity tab
Adjust opacity to 40%
Click OK to apply

7. Extract Geometry – Exchanger(I)
To reveal edges, we will use Extract Features operation. These edges will indicate additional mesh refinement regions.
Extend Options list next to the exchanger geometry
Select Extract Features

8. Extract Geometry – Exchanger(II)
Select Extract

9. Extract Geometry – Pipes (I)
Repeat extract operation for the pipes
Extend Options list next to the pipes geometry
Select Extract Features

10. Extract Geometry – Pipes (II)
Select Extract

11. Create Face Groups (I)
We need to distinguish surfaces that will be used as the mesh boundaries (both external and internal). We will do it in the 3D graphical panel.
Select first inlet face
(hold Ctrl and left-click on the geometry face)Click Geometry Faces next to exchanger
Click Create New Face Group
Click Create Group From 3D Selection
Rename group_1 to hot_inlet
(double click on the group to rename, press Enter to confirm)Click Clear Selection to deselect faces
(use before creating new selection within the same geometry)

12. Create Face Groups (II)
We will repeat the previous operations for the remaining inlets and outlets. The final face groups list for exchanger should look like below:
hot_inlet (darak red)
hot_outlet (light red)
cold_inlet (dark blue)
cold_outlet (light blue)
To create face groups for pipes geometry, hide the exchanger geometry first. Then create two face groups like below:inlet_baffle (yellow)
outlet_baffle (green)
Tip #1 To select a single face, first exit selection by clicking Esc |
Tip #2 To hide exchanger geometry, click the STL icon to the left of its name |

13. CHT Mesh
Since we are going to perform CHT (Conjugate Heat Transfer) simulation, we need to create the mesh per each fluid and solid sub-domain.
In the typical heat exchanger, we would have three regions: hot fluid region, cold fluid region, and solid region representing pipes and baffles.
In this tutorial, we will use the alternative approach, in which we will skip the solid region and represent it by infinitely thin walls. The influence of walls on heat transfer between fluids will be modeled using Thermal Resistance . Therefore, we will need to mesh only two fluid regions: hot and cold fluid regions.
14. Hot Fluid Mesh - Meshing Parameter - Exchanger
Hot fluid region
We will start meshing from the hot fluid region.
Go to Hex Meshing panel
Make sure that all geometries are visible
(you can unhide the geometry by clicking the icon next to the geometry name)Select exchanger geometry
Enable Mesh Geometry
Set Refinement to Min 0 Max 1

15. Hot Fluid Mesh - Meshing Parameter - Pipes
Select pipes geometry
Enable Mesh Geometry
Set Refinement to Min 1 Max 1

16. Base Mesh
We need to define the base mesh. The box geometry determines the background mesh domain. It encloses both fluid regions – hot and cold.
Go to Base tab
Press Autosize button
(make sure that all geometries are visible – autosize option adjust the base mesh only to the visible geometry)Define the number of divisions
Division372591

17. Hot Fluid Mesh - Material Point
In order to create the mesh in the hot fluid region, we will place the material point inside the hot fluid sub-domain. The resulting mesh will remain only in this region.
Go to Point tab
Specify location inside the hot fluid region
Material Point00-0.1
You can specify the point location from the 3D view. Hold the Ctrl key and drag the arrows to the destination.

18. Hot Fluid Mesh - Start Meshing
Now, it’s time to create the mesh of the hot fluid region.
Go to Mesh tab
Start the meshing process with Mesh button

19. Hot Fluid Mesh
When the meshing process is finished, the hot fluid region mesh appears on the screen.

20. Hot Fluid Mesh - Create Sub-region
For the CHT simulations, we need to mark each of the mesh regions as sub-domains. The sub-domains represent a partial mesh that will not be overwritten by meshing operations that use the default region as a target.
Expand the Options list next to the default region
Select Make sub-region
Enter Region Name to hot
Press OK

21. Cold Fluid Mesh - Meshing Parameter - Baffles
Cold fluid region
Now we can mesh the second region – the cold fluid region. We will use already defined geometry parameters for exchanger and pipes. We just need to add baffles to be included in the mesh.
Go to the Hex Meshing panel
Go to the Geometry tab
Select baffles
Enable Mesh Geometry
Set Refinement to Min 0 Max 1
Turn on Create Baffle

22. Cold Fluid Mesh - Material Point
We need to move the material point to be positioned inside the cold fluid region.
Go to Point tab
Specify location inside the hot fluid region
Material Point000.1

23. Cold Fluid Mesh - Start Meshing
Now, it’s time to create the mesh of the cold fluid region. Please note, that the resulting mesh will be automatically assigned to the default region and will exist next to the previously created hot fluid mesh.
Go to Mesh tab
Start the meshing process with Mesh button

24. Mesh
The complete mesh should look like in the picture below.

25. Cold Fluid Mesh - Create Sub-region
Move the default region into the cold fluid region. The CHT simulation can only use the sub-region meshes.
Go to MESH panel
Expand the Options list next to the default region
Select Make sub-region
Enter Region Name to cold
Press OK

26. Create Mesh Interface (I)
In the previous steps we have created the mesh for hot and cold fluid regions. At the moment they are treated separately, so the information on the flow cannot be exchanged between them. It’s time to create the interface (coupling) between both fluid regions. Later we will define boundary conditions which will describe the way we want to exchange information between hot and cold fluid region.
Select the pipes in cold fluid region and the pipes in hot fluid region
(hold CTRL key and select both boundaries)Press Create Region Interface

27. Create Mesh Interface (II)
Repeat previous steps for pipes_inlet_baffle and pipes_outlet_baffle couple. Check the interfaces list
_pipes _in cold \(\leftrightarrow\) _pipes _in hot
_pipes_inlet_baffle _in cold \(\leftrightarrow\) _pipes_inlet_baffle _in hot
_pipes_outlet_baffle _in cold \(\leftrightarrow\) _pipes_outlet_baffle _in hot
+Adjust the remaining boundaries types
baffles wall
baffles_slave wall
exchanger _in cold _wall
exchanger_cold_inlet patch
exchanger_cold_outlet patch
exchanger _in hot _wall
exchanger_hot_inlet patch
exchanger_hot_outlet patch

28. Select Solver
For the calculations, we will use a steady-state conjugate heat transfer solver. The family of CHT solvers will activate only if sub-region meshes exist.
Go to SETUP panel
Pick CHT Multi Region SIMPLE solver
Select solver

29. Radiation
We will disable radiation for our simulation.
Go to Radiation panel
Uncheck Enable Radiation option

30. Thermo - Fluid Properties - Hot Region
Now we need to define fluid properties. We will assume that working fluid for hot and cold regions is water.
Go to Thermo panel
Select hot region
Select Constant Density for Equation of State
Open Material Database
Scroll down to find Water
Click Apply

31. Thermo - Fluid Properties - Cold Region
Select cold region
Select Constant Density for Equation of State
Open Material Database
Scroll down to find Water
Click Apply

32. Operating Conditions
We will turn off the gravity acceleration and set the reference pressure.
Go to Operating Conditions panel
Set non Gravity Acceleration
g \({\sf [m/s^2]}\)000

33. Boundary Conditions - Exchanger Cold Inlet - Flow
We will leave the default conditions for the baffles and heat exchanger external surfaces – adiabatic (isolated) walls. Now, we will define the inlets and outlets parameters for hot and cold regions.
Go to Boundary Conditions panel
Select exchanger_cold_inlet boundary
Set the Velocity Inlet character
Set the inlet velocity
U Reference Value \({\sf [m/s]}\)0.01

34. Boundary Conditions - Exchanger Cold Inlet - Thermal
Go to Thermal tab
Set the type and value
T Type Fixed Value
T \(T_0\) \({\sf [K]}\)283

35. Boundary Conditions - Exchanger Cold Outlet
Select exchanger_cold_outlet
Switch to Thermal tab
Set the Type to Zero Gradient

36. Boundary Conditions - Exchanger Hot Inlet - Flow
Select exchanger_hot_inlet boundary
Set the Velocity Inlet character
Switch to Flow tab
Set the inlet velocity
U Reference Value \({\sf [m/s]}\)0.02

37. Boundary Conditions - Exchanger Hot Inlet - Thermal
Go to Thermal tab
Set the type and value
T Type Fixed Value
T \(T_0\) \({\sf [K]}\)383

38. Boundary Conditions - Exchanger Hot Outlet
Select exchanger_hot_outlet
Switch to Thermal tab
Set the Type to Zero Gradient

39. Boundary Conditions - Interfaces (I)
Now we need to define how hot and cold fluid exchange information between each other. At the beginning of this tutorial, we mentioned we will not model solid walls between two fluid regions. Instead, we will use thermal resistance to replicate heat conduction through the solid.
In the Boundaries list pipes , pipes_inlet_baffle , pipes_outlet_baffle occur twice, as boundaries with the same names exists in both hot and cold regions. Thermal resistance parameters will be displayed only on one from the pair.
image:[image]
40. Boundary Conditions - Pipes - Thermal
We will apply the same settings for other interfaces under hot region: pipe , pipes_inlet_baffle and pipes_outlet_baffle boundaries.
Select pipes (hot region)
Go to Thermal tab
Check the Resistance
Set the thickness of the wall and thermal conductivity
T \(\sigma\) \({\sf [m]}\)5e-03
T \(\kappa\) \({\sf [W/m \cdot K]}\)385

41. Boundary Conditions - Pipes Inlet Baffle - Thermal
Select pipes_inlet_baffle (hot region)
Go to Thermal tab
Check the Resistance
Set the thickness of the wall and thermal conductivity
T \(\sigma\) \({\sf [m]}\)5e-03
T \(\kappa\) \({\sf [W/m \cdot K]}\)385

42. Boundary Conditions - Pipes Outlet Baffle - Thermal
Select pipes_outlet_baffle (hot region)
Go to Thermal tab
Check the Resistance
Set the thickness of the wall and thermal conductivity
T \(\sigma\) \({\sf [m]}\)5e-03
T \(\kappa\) \({\sf [W/m \cdot K]}\)385

43. Initial Conditions - Cold Region
Before we start simulation we need to define the initial conditions. We will adjust the initial velocity and temperature to the inlet conditions of each region.
Go to Initial Conditions panel
Select hot fluid region
Define initial velocity and temperature
U000.02
T383

44. Initial Conditions - Hot Region
Select cold fluid region
efine initial velocity and temperature
U0.0100
T283

45. Run Simulation
Finally, we can start our computation.
Go to Run panel
Set Number of Iterations to 700
Click Run Simulation

46. Residuals
Monitor convergence process under Residuals tab

47. Postprocessing - ParaView
After computations are finished we can do a complex visualization of our results with ParaView.
Go to Postprocessing panel
Click Run ParaView
If you do not plug in the new ParaView to SimFlow, you can just run the ParaView and open the case file:
` …/heat_exchanger/heat_exchanger/heat_exchanger.foam `

48. ParaView - Load Results
Load the results of the simulation from SimFlow
Select heat_exchanger.foam
Click Apply button to load results into ParaView
Select Temperature from the drop-down list
After loading results they will be shown in the 3D graphic window

49. ParaView - Clip
We will create the cross-section through the computational domain to display the temperature distribution.
Select Clip button
Set the plane origin and normal
Origin000
Normal010Untick Show Plane
Untick Invert
Press Apply
From the drop-down menu select Temperature

50. ParaView - Results
Orient the view parallel the XZ plane and rotate 90 degrees clockwise
