Cooling Channel - CFD Simulation SimFlow Tutorial

In this tutorial, you’ll take on the challenge of solving the conjugate heat transfer problem. We will explore a scenario in which a plate is exposed to heat from equipment located on the top surface. This topic has numerous applications where analyzing the circulation of fluids is essential for efficient heat dissipation.

Throughout this tutorial, you will acquire expertise in the following areas:

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

Open SimFlow and create a new case named cooling channel

In the following tutorial, we will use the geometry that has been already created and consits of multiple parts. We will import all parts to the SimFlow.

Download GeometriesPlatePipeHeater

The STL format does not contain the unit information which is 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.

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

In this simulation, we are dealing with an internal flow problem. The imported geometry determines the bounds of the domains. To inform the program where the boundaries of the inlet and outlet mesh should be created, we will use the Face Groups. Face Group is a set of faces that should be distinguished within a geometry. When the geometry containing the face group is used for meshing, an additional boundary is created. The boundary represents the respective face group and inherits its name.

Now, rotate the view in a way you will be able to see the second end of the pipe.

In the Geometry Panel we can find four Face Groups under the pipe geometry. The first group, named default, contains all non-selected surfaces. These surfaces will become the walls of the pipe. The two additional groups represent the inlet and the outlet of the fluid domain. We will rename these groups to make the resulting boundary names more readable.

The geometry is ready to be meshed. Set the transparency of the plate geometry to see the pipe inside.

Once the geometry is prepared, we can move to the geometry surface mesh properties. To better resolve the heat transfer from the heater, we will increase mesh resolution in this area.

Near the pipe surface, also we will refine the mesh to better resolve the coolant flow. We will apply the same settings as before.

We will also enable meshing for the plate geometry in this step.

Now, we need to define the base mesh. The box geometry determines the domain’s background mesh. The base mesh encompasses both fluid and solid regions.

Typically, we use only the default material point to create a mesh inside defined fluid volume. In this tutorial, we will take advantage of the Multi-Zone Mesh option instead. Using two material points, we will identify two separate regions in which the mesh will be created. Solid region will be used for the heat transfer in plate geometry, while in the fluid region we will simulate the fluid flow inside the pipe.

In this step, we will initiate the meshing process.

The meshing process can be executed in parallel, offering a substantial reduction in mesh generation time. When running in parallel, you have the flexibility to choose the number of CPUs utilized, depending on your PC’s capabilities. Please be aware that if you are using the free version of SimFlow, you are limited to employing only 2 CPUs, and meshes exceeding 200'000 nodes cannot be created.

If you would like to test full version Request 30-day Trial

After the meshing process is finished, the mesh should appear on the screen. At the begging you will see the mesh in light blue color. All the cell zones overlap the mesh, and thus we only see the cell zones. To hide cell zones and display mesh boundaries, follow these steps:

The result of multi-zone meshing is a single mesh region with multiple cell zones. At this stage, the plate and fluid volumes are connected. The boundaries separating the fluid and solid volumes are no longer present in the mesh. We can recreate them by converting the cell zones into separate mesh sub-regions. After this operation, new boundaries will appear in place where two cell zones are connected.

Please, note, when we use the Cell Zones to Regions option, the new boundaries between cell zones will be automatically coupled to each other. The coupling between boundaries localized in two different regions represents the interface that allows the heat transfer between them.

To convert cell zones to regions, you need to:

New regions appeared under the default mesh region - fluid and plate. Currently, the mesh is duplicated, and we can see both original mesh and the new regions. Now, we need to remove the old mesh (default region).

Now we will assign proper region types to indicate which region denotes fluid and solid. The default type is set as fluid which is accurate for the fluid region. However, in the case of the plate region, it is necessary to set it to solid.

Also, we need to make sure that all boundaries have the proper type. The final mesh should consist of patch types for inlet/outlet, walls for outer boundaries and the inner pipe walls interface.

We will perform a steady state simulation of the Conjugate Heat Transfer (CHT) problem. The family of CHT solvers will activate only if sub-region meshes exist. We will use CHT Multi Region SIMPLE (chtMultiRegionSimpleFoam) solver.

For the sake of simplicity, we will not take into account the radiation heat transfer.

To assign specific materials for regions, we will use the built-in database of material properties. We assume that water, incompressible fluid is flowing in the pipe.

Selecting material from the Material Database will fill all the inputs in the Transport Properties panel. We are still able to overwrite these values at any time.

Similarly, we will now define the thermodynamic properties of a solid material. We assume that the plate is made of aluminium.

We will now define the boundary conditions of our model. First, define the inlet velocity of the water in the pipe.

The interface between the pipe and the plate is coupled enabling the transfer of heat between these two regions. It is possible to take into account the thermal resistance of the pipe, even though the pipe thickness is not represented in the mesh. To accomplish this, you only need to specify a constant thickness of the pipe and provide its thermal conductivity.

To provide heat to the aluminium plate, we will use the heater boundary and assume constant heating power 'Q'.

To simulate the heat transfer from the plate to the environment, we will use the Wall Heat Flux boundary condition, which implements convective heat transfer. We will make the assumption that the ambient temperature is 300K, and for passive cooling, we’ll specify a heat transfer coefficient equal 5.

Finally, we can start calculations. It’s important to be aware that for the CHT solver, the maximum iteration count is the sole criterion for ending the computation. Even if the residual levels reach the desired values, the solver will continue running until the maximum iteration limit is reached.

To speed up the calculation process, increase the number of CPUs depending 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: 6 minutes

When the calculation is finished, we should see a similar residual plot.

Start ParaView software to display results.

Load results into the ParaView.

We will display the temperature map for the model.

To see the temperature distribution inside the model, we will use the clip filter.

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.

Paraview CFD Tutorial - Advanced Postprocessing in ParaView