Electronics Cooling - CFD Simulation SimFlow Tutorial

This tutorial will demonstrate a simulation of electronic cooling. We will model a Joule heat source within a solid part (CPU) and a cooling domain filled with flowing air. The steady-state simulation will calculate conjugate heat transfer (CHT) on the interface between the CPU and air. In the second part of the simulation, we will enable the Surface-to-Surface radiation model and observe its impact on the results in ParaView.

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 electronics_cooling

Firstly we need to Download GeometriesBoardCpuPins

The imported geometry is in STL format, which does not store unit information. We need to confirm the unit in which the model was created. In the selection of unit, we can use the Geometry size label, which displays overall size of the model in each direction. In our case, the default unit meter is correct.

After loading geometry, it will appear in the graphics window

Add fan geometry to the model. It will be placed above the CPU.

Now rotate the geometry of the model so that we can see the bottom side of the newly created fan. We will now select a face that will be subdivided from the fan as a separate boundary patch by the meshing tool.

The last primitive geometry to create is a box that will be used as a tool to extract outlet patch from outer boundaries

Since we are going to perform CHT (Conjugate Heat Transfer) simulation, we need to create the mesh for fluid and solid sub-domains. We will specify the mesh parameters for all geometries and using the material point we will choose the subdomain that will be meshed.

Now, we will define the base mesh. The box geometry determines the background mesh domain.

In order to create the mesh in the solid region, we will place the material point inside the fan geometry. The resulting mesh will remain only in this region.

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

When the meshing process is finished, the solid region mesh appears on the screen.

Before generating a mesh for the fluid region, you must convert the current mesh into a sub-region. Otherwise, it would be overwritten by the new mesh.

Once the solid region is created, we can move the material point to anywhere inside the base mesh, but outside the solid region.

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

The mesh will be displayed in the graphics window

In the geometry setup, you created outlet_tool . You will now use this box to extract patch from boundary patch

The new patch will appear on the list of boundaries

Now we have to rename the newly created boundary

Now, after you used the Extract tool on the default mesh, you can convert it into a sub-region. It’s important to note that extract operations are no longer available once the mesh is converted.

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.

We will use CHT Multi Region SIMPLE (chtMultiRegionSimpleFoam) solver. This is a steady state solver that allows modeling of conjugate heat transfer and radiation.

We will first run a simulation without taking radiative heat transfer into account. However, it is important to set up all radiation model parameters now (these parameters cannot be changed later without resetting simulation).

Now we need to define solid and fluid properties. We will assume that the working fluid is air and the solid is made of aluminum.

For turbulence modeling, we will use \(Realizable \; k{-} \varepsilon\) model

We will now adjust the solver tolerance threshold of the enthalpy equation in the solid region in order to achieve better convergence

To achieve better convergence we will adjust SIMPLE algorithm settings.

Now, we will adjust the limits of temperature fields in order to narrow the convergence space of the solution

Now set heat source term in the CPU volume. In this tutorial, we assume that only the CPU produces the heat of power of 0.25 W and its volume is about 200 mm ³ :

Now, we will define the inlets and outlet boundary conditions. On the inlet, we will set constant air inflow.

We will now enable radiation coupling on the fluid side of the interface

Next, enable radiation coupling on the solid side of the interface

Estimated computation time: 10 minutes

Start ParaView software to display results

We will now plot the temperature contour on the circuit board again. We will use the same scale, so the differences in results are more evident

Results are displayed in the graphics window. Note that the maximum temperature in the domain is 360 K.

We will now enable the radiation equation in our simulation. To do this, close Paraview and go back to SimFlow

The case is set up. We will increase the number of iterations and run the simulation

Estimated computation time: 20 minutes

Start ParaView software to display results

You will now plot the temperature contour on the circuit board again. You will use the same scale, so the differences in results are more evident

Results are displayed in the graphics window. Note that in this case, the maximum temperature in the domain is 343 K, which is 17 K lower than in the previous simulation.

Radiation plays an important role in this scenario. Therefore, our last task will be to display radiative heat flux mapped on the geometry

Results are displayed in the graphics window.

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