Required field
Required field
Required field
Required field

# Thermal Management Tutorial: CHT Analysis of an Electronics Box

This advanced thermal management tutorial describes the setup and analysis of electronics cooling on an electronics box containing different electronic components being cooled by the airflow of a fan.

All electronic devices generate heat during their operation. Components and materials, used in these devices, have individual maximum temperature limitations. Therefore, thermal management is extremely crucial for system reliability and preventing failure.

Simulation is a cost-efficient method to test different cooling strategies and optimize your solution. This is a great advantage to prevent time-consuming and expensive prototyping and physical testing procedure.

This tutorial teaches you how to:

• Select suitable boundary conditions for thermal management/electronics cooling.
• Assign materials for different components.
• Define individual contact properties.
• Judge the calculation stability.

We are following the SimScale workflow:

1. Preparing the CAD model for the simulation.
2. Setting up the simulation.
3. Creating the mesh.
4. Run the simulation and analyze the results.

## 1. Prepare the CAD Model and Select the Analysis Type

Import the tutorial project into your Workbench, by clicking the button below:

The simulation project contains two geometry parts, one is the original CAD Geometry, the other contains the fluid region and prepared topological entity sets. For this tutorial, use the prepared flow region geometry. Nevertheless, we will have a short explanation of how to generate the internal fluid volume.

Generate Internal Fluid Volume

If you wish to learn how to prepare your model for any type of simulation, take a look at the CAD preparation section. For every internal fluid simulation, we need the volume of the fluid. This can be directly created within the Cad Mode inside the SimScale platform. The steps to enter the CAD Mode can be seen in Figure 3.

1. Select the Geometry Part ‘Electronic Box’
2. Click on ‘Edit in CAD Mode‘.

The CAD mode interface looks as follows:

Next, create an internal flow volume. SimScale has a dedicated tool for this creation so that no extra boolean operations have to be performed. To create, extend the ‘Flow Volume’ icon and select ‘Internal’.

To create the internal fluid volume, select a face of the housing that will be adjacent to the boundary face. This will define a starting point (source) for the internal fluid volume creation and is referred to as a seed face.

Since the housing of the electronic box has two open faces, we have to define two boundaries, which will limit the creation of the internal fluid volume. For the electronic box, select the front and the backside of the housing, as the boundaries.

1. Select a seed face inside adjacent to the boundary face.
2. Select the boundary faces for the internal fluid volume.
3. Hit ‘Apply’.

Exit the Cad mode by clicking the Export button (top right). You should see a new part created named ‘Copy of Electronic Box’. For a faster simulation setup, it is recommended to assign Topological Entity Sets, which can group multiple parts under a name. We will then use these sets to assign simulation properties at once to a simulation setup.

For this simulation, use the ‘Electronics Box Flow Region Prepared’ geometry, where only the topological entity set for the boards is missing.

### 1.2 Topological Entity Set for the Boards

To continue with the simulation setup select the geometry ‘Electronics Box Flow Region Prepared’. To create the sets for the boards, switch to the volume selection mode, expand the geometry parts list, and select the following parts: ‘Board 4’, ‘Board 3’, ‘Board 2’, ‘Board 1’, and ‘Main Board’. After selecting the Parts click on the plus icon next to Topological Entity Sets and name the set ‘Boards’.

## 2. Simulation Setup

### 2.1 Create a Simulation

Select the CAD model ‘Electronics Box Flow Region Prepared’ and click the ‘Create Simulation’ button as presented in the following picture:

Now the SimScale simulation library will pop up:

Within this simulation library, all analysis types available in SimScale are listed. Selecting one of them shows a description of them. For this thermal management simulation, we select the ‘Conjugate Heat Transfer (CHT)’ option and hit the ‘Create Simulation’ button to confirm our selection.

Did you know?

The analysis type you choose within the simulation library depends on what results you are interested in and what given parameters you have.

• In this simulation we want to see the heat transfer both within the solid parts as well as from the solids to a fluid. Hence we need to select the Conjugate Heat Transfer (CHT) analysis type. This is the most common analysis type for electronics cooling. Note that SimScale also offers CHT v2.0 which is faster, more accurate but at a reduced feature set.
• If you are only interested in the heat transfer within solids, you can simplify the simulation process by performing a Heat Transfer analysis.
• On the other hand assuming you are only interested in the heat transfer within a fluid, you would go for Convective Heat Transfer.

### 2.2 Global Settings

Now you have successfully created the thermal management simulation and you should see the simulation tree, named Conjugate heat transfer on the left side of the Workbench as shown in the picture below:

1. Open the global Settings for the Conjugate heat transfer setup.
2. Adjust the Turbulence model to ‘k-omega-SST’.

You can define the global settings by clicking on the simulation, in this case, named ‘Conjugate heat transfer‘. Here we can decide whether we want to take into account radiation, which turbulence model we want to apply, and whether we want time-dependent or averaged results. Makes sure the turbulence model to ‘k-omega-SST’ is selected and keeps the rest as defaults.

Did you know?

The k-omega SST turbulence model switches between the k-omega and k-epsilon model automatically, therefore it takes the advantage of both models and can be used for the majority of turbulence simulation.

### 2.3 Geometry

The Geometry is being selected automatically. In case you have multiple geometries uploaded, make sure to choose the right one.

### 2.4 Contacts

The thermal interface is a commonly used feature when it comes to electronics cooling and thermal management applications. Contacts are detected automatically, thanks to our earlier use of the SimScale internal fluid volume tool. It should be 646 standard interfaces at the beginning.

If you want to specify the physical quantities of contact you can change the type of the interface, therefore you need to select the interface. In this case, it is the interface between the large chip and the heat sink. To see them we need to hide the housing, the flow region, and the heat sink.

#### Changing The Thermal Conductivity Of The Large Chip and Conductor

For this analysis, we want to simulate a 0.001 $$m$$ thermal paste with 8 $$\frac{W}{mK}$$ thermal conductivity, between the large chip and heat sink. To achieve that we have to change the contact definition of the contact between the large chip and the capacitor. To hide the parts in view of the contact surface, select the topological entity sets, and hide them by clicking on the eye icon.

1. Expand the Topological Entity Sets
2. Select the Housing, Main Board Heat Sink, and Fluid Volume sets and hide them using the eye icon one by one.

Now you can select the interface and define a specific interface condition like presented in the following picture:

1. Select the interface highlighted in red.
2. Right-click on the Workbench and choose ‘Filter contacts by selection’.

Doing so leads to the menu where you can define the interface’s properties:

1. Chage the interface type to Thin layer restiance.
2. Assign a Thermal conductivity of 8 $$\frac{W}{m K}$$ and a Layer thickness of 0.001 $$m$$.

Watch Out!

1. If there are any partial interfaces () detected, there is a CAD issue on the corresponding contact face. To find the problematic face, select the interface and then right-click anywhere on the Workbench and select ‘Isolate all assignments’. This will visualize the problematic interface. Finally, go back to CAD mode or your CAD software and fix the corresponding face.
2. Avoid adding thin layered materials (thermal paste, insulator on winding, etc.). Including these materials in the model increases the mesh density and the computational expense. Instead, you can define them as a Contact interface as described earlier in this section.

### 2.5 Model

In the next step, define the simulation model, in this case, it means setting up gravity like in the figure below.

Define gravity based on its global coordinate system. Here, it is 9.81 $$m/s^2$$ in the positive y-direction. This condition gains more importance when dealing with natural convection.

### 2.6 Materials

The next step in the setup is the material assignment for the various components of the electronic box. Assign a fluid material to the fluid volume and a selection of solid materials to the individual components.

1. Fluid Materials (Air)

To define a new fluid, click on the ‘+’ next to the Fluids item. Doing so makes the fluid library pop up:

Choose Air and hit ‘Apply’ to confirm the selection. Accordingly, the material properties pop up:

Assign the Topological Entity ‘Fluid Volume’ to the air material. Next, we will assign the materials for the electronic components. The table shows the material selection for the individual components. For better visualization of the next steps, it’s recommended to hide the already assigned parts, therefore hide the ‘Fluid Volume’ by clicking on the eye icon in the list of ‘Topological Entity Sets’

Be careful when assigning the solid materials:

When creating and assigning materials beware of what parts of the geometry are highlighted, because this will be assigned to the new material automatically.
Also note that every part in the CAD model needs to be assigned to one and only one material.

#### 2. Solid Materials (Aluminium)

Next, we select the solid material for the housing. For this tutorial, we will use the aluminum material provided by SimScale. To select a new solid material select the ‘+’ icon next to Solids and select Aluminium.

1. Create a new material.
2. Select ‘Aluminium’ from the SimScale material libary
3. Confirm the material by clicking the ‘Apply’ button.

Next, we have to select the part which we want to assign to the Aluminium material. To do this either select the ‘Housing’ from the Topological Entity Sets or select the part directly in the user interface.

#### 3. Soldi Materials (PLA (Polylactic acid) / Copper / Tin / Silicon)

Next, we will assign the rest of the solid materials. Therefore repeat the steps for the Aluminum material assignment and select the equivalent material from the material library. The results for each material should look like this:

#### Silicon

For the Silicon assigned volumes, not all topological entity sets are visible in Figure 26. The other assignments not visible are Small Chips, Transformer, and Board Large Chip. Please make sure that these are also selected.

Custom Material

If you want a different material for your thermal management simulation than the default materials in the library, you can create a custom material.

### 2.7 Initial Conditions

Initial conditions are the starting points for a thermal management simulation. Those are the values assumed at the beginning of a simulation. We will not touch the global initial values for this analysis as the defaults are sufficient, but define the initial temperature for the Main Board Large Chip and the Main Board Heat Sink. To achieve that, select a subdomain for the temperature and assign the temperature and the parts.

1. Create a new subdomain for the tempertature by clicking the ‘+’ icon.
2. Set the Subdomain value to 50 $$°C$$.
3. Assign the sets ‘Main Board Heat Sink’ and ‘Main Board Large Chip’.

Did you know?

You do not have to initialize anything. SimScale’s default values work for common use-cases.
Although if you estimate the individual initial conditions applying for your specific application correctly, you can stabilize the calculation and improve the convergence behavior.

### 2.8 Boundary Condition

Next, we have to assign the boundary conditions to the simulation. For this tutorial, we assume that the electronic box is equipped with external fans, which sucks the air through the electronics box.

#### 2.8.1 Boundary Conditions with Fans ON

The following picture shows an overview of the physical situation applied in this electronics cooling simulation:

We will assign boundary conditions to the fan outlets, openings (inlets), and the heat transfer surface of the casing, using boundary conditions (BCs).

In this example, air movement is forced by fans sucking the air out of the domain. The casing surface helps to lose heat to the exterior domain. In this example, we do not create an exterior domain to simulate the external heat transfer of the electronic box. We assume the device to be in a 20 $$°C$$ ambient environment and simulate the heat transfer to the ambient by applying an external wall boundary condition.

#### a. Fan outlet – Custom

To create a fan boundary condition a custom boundary condition is used. The setup of this boundary condition can be seen in Figure 28 below:

1. Create a custom boundary condition by hitting the ‘+’ button next to boundary conditions.
2. Select ‘Custom’.
3. Define the values according to Figure 28:
• (U) Velocity: ‘Pressure inlet-outlet velocity‘. This means that the velocity on the fan BC is dependent on the pressure difference.
• (P) Modified pressure: ‘P<fan> Fan pressure‘. This option enables to upload a fan curve.
• Flow direction: ‘Out‘. This is an exhaust fan, therefore flow should leave through the fan.
• (T) Temperature: ‘adiabatic’. Adiabatic means to take the surface value from the neighbor element. We want the solver to calculate the temperature on the outlet based on the heat it absorbed on its way through the electronics box, that’s why we do not specify an absolute value.
• (k) Turb. kinetic energy: ‘Zero gradient‘. Same like adiabatic for temperature.
• (ω) Specific dissipation rate: ‘Zero gradient‘. Same like adiabatic for temperature.
4. Select the outlet faces of the Flow region highlighted in the figure.
5. Define the fan curve by creating a table:

Create two new columns, one for the mass flow through the fan $$Q$$ $$kg/s$$ and one for the fan pressure $$P<fan>$$ $$Pa$$. Now you can define your own pressure curve, by typing in the value or simply uploading a CSV file. You can download the table used for this tutorial with the download link below.

Did you know?

You can also use a velocity outlet and specify a fixed flow rate or velocities for the outlet.

#### b. Inlet – Pressure Inlet

For the airflow into the electronic box define a pressure inlet boundary condition. Create a new boundary condition and select the ‘Pressure Inlet’ type. The setup and the assigned faces can be seen in Figure 30:

#### c. Thermal Wall – Housing

Last we have to define the influence of the ambient temperature on the electronic box. Since we don’t simulate the airflow around the electronic box, we will use a thermal wall model for the housing. With this model, we can also implement the effect of heat flux through the housing. Create a new boundary and select the wall model. The setup for the external wall heat flux model can be seen in the figure below:

1. Change the temperature model to ‘External Wall Heat Flux’.
2. Change the ambient temperature to 35 $$°C$$.
3. Change the initial boundary temperature to 20 $$°C$$.
4. Assign all of the outside faces of the housing as displayed above.

Unassigned Surfaces

Surfaces which are not assigned to either of the boundary conditions or a contact will be treated as an adiabatic wall. Therefore, the wall will be calculated as a perfect thermal insulator, with no heat flux across the wall.

### 2.9 Advanced Concepts – Defining Power Sources

Components in electronics devices receive electrical current and generate heat. Heat dissipation from any component can be defined by assigning an absolute power source $$W$$ or a specific power source $$W/m^3$$ to the corresponding part. In this tutorial, we only assign a power source to the main CPU and the other small chips.

The following table describes the power source and the topological set.

The setup of the individual power sources are described in the images below:

#### a. Main Board Large Chip

1. Hit the ‘+’ button next to Power sources under Advanced concepts.
2. Select the option ‘Absolute power source’.
3. Define the amount of heat, in this case, we choose ’60 $$W$$’.
4. Select the Topological Entity Set ‘Main Board Large Chip’

Did you know?

You can assign as many different heat sources as you like. You also have the option to assign the power sources to a geometry primitive you define during the simulation setup, in case you do not have the electronic component generating heat represented in your model.

The following figures show the heat sources applied in this tutorial, please follow the same workflow as just described:

#### c. Board Flat Chips

These advanced concepts might also be helpful for an electronics cooling application:

• Rotating zones: If your CAD model contains the rotor blades, you can set up their rotational properties here
• Power sources: Here you can define additional heat sources
• Momentum sources: This serves as a simplification for modelling the fans, in case you do not have the fan’s geometry

### 2.10 Simulation Control

The default settings for numerics are usually suitable. Experienced users can use manual settings for smoother or faster convergence.

The Simulation Control settings define the general controls over the simulation. We will use the following controls for this simulation:

• End time: 1300 $$s$$
• Write interval: 1300 time step
• The number of processors: Automatic
• Maximum runtime: 30000 $$s$$

### 2.11 Result Control

As a default setting, velocity, pressure, density, temperature, and radiation variables will be saved for every cell in the fluid domain. The changes of those between the timesteps are displayed in the convergence plot.

You can use result control to observe the development of the values at any point or surface in your domain during the calculation. For this tutorial, we will create two result control items to analyze the airflow through the electronic box.

#### 2.11.1 Outlet Temperature

To access the outlet air temperature create an area average on the fan outlet faces. With that, the physical data for these surfaces such as pressure, temperature, velocity, and more will be saved every 20 iterations and written into a plot during the calculation. Follow the steps presented in the figure below:

1. Hit the ‘+’ button next to Surface data under Result control.
2. Select the option ‘Area Average’.
3. Define a Write interval as ’20’.
4. Select the six outlet faces highlighted in the Figure 35.

#### 2.11.2 Volumetric Flow Rate

To see the flow rate generated by the fan, duplicate the above result control item.

1. Rightclick on the Area Average result control item and select ‘Duplicate’.
2. Change the Surface data to ‘Area integral’.
3. Change the Write interval to ’20’.

Did you know?

Adding result control items help to see the convergence, but they also increase the computational time. Therefore it is recommended to add only the necessary items and keep the write interval high. As an example, if you perform 2000 iterations, assigning the write interval as 50 means that every selected result control item will be saved 40 times.

We recommend adding result control items to the inlets, outlets, and components with expected critical temperatures. Repeat the same setup procedure as for the control items before and assign the faces of the CPU.

#### 2.11.3 CPU Temprature

In the figure below you can see the setup for the CPU result control item.

## 3. Mesh

Default mesh settings usually create a good mesh. For conjugate heat transfer, we recommend the following settings:

Keep everything as default, except the following items:

1. Select the ‘Mesh’ item to generate a new mesh.
2. Sizing‘Automatic’, Fineness: ‘2’.
3. Expand the Advanced settings set small feature suppression of ‘1.e-5 $$m$$‘ This makes the algorithm neglect anything that is smaller than 1e-5 $$m$$. Do not generate the mesh yet.

## 4. Start the Simulation

After all the settings are completed, proceed by clicking the ‘+‘ icon next to the Simulation Runs, to start with the analysis. The mesh will be generated automatically before the run. Right after the mesh generation, the simulation run will start.

While the results are being calculated, you can already have a look at the intermediate results in the post-processor. They are being updated in real-time!

## 5. Post-Processing

When the simulation is complete, you can check the Convergence plot and the Solution fields from the simulation. You can access either of them in the simulation tree by clicking on them, as you can see below:

### 5.1 Convergence And Outlet Flow / Temprature

When the run is finished, or even while the results are being calculated, we can observe the convergence behavior. For a steady-state analysis, the result should converge to a point where the flow field characteristics do not change anymore, which can be seen that the residuals are approaching a horizontal line.

a. Convergence Plot

Each timestep, the solver calculates solutions for each cell in the mesh. The residuals are the differences between those results. Hence the lower the residuals, the more stable the solutions are. We also call that “convergence”. The following picture shows the convergence plot for the tutorial’s calculation.

1. Select the finished Simulation run
2. Open convergence plots and residuals.

The residuals are presented dimensionless and you can convert them into a percentage: In the tutorial, all graphs are beneath 1e-2 and some even lower than 1e-3, which is a good sign for convergence.

b. Result Control

With the result control items created we can analyze the results for special faces of interest. Let’s have a look at the outlet temperature. Since the inlet temperature is constant, with this result, we can calculate the temperature difference of the airflow for the complete electronics box. For the same power input into the components and inlet temperature, the higher the air temperature is the better is the cooling of the electronic parts. The result for the temperature of each outlet face can be seen in Figure 40 below.

Having a look at this plot, most of the temperatures approaches a horizontal line, which means, that the result is approaching a steady-state result, where the flow field characteristics are constant. The maximum temperature is 296$$K$$ ( 43$$°C$$). Averaging the temperature for all faces we get an average outlet temperature of 294$$K$$ ( 41$$°C$$), which means we have an increase of 21 $$K$$ between the inlet and the outlet.

### 5.2 Surface Visualization

Let’s have a look at the different temperatures and the flow field visually. The following figure shows how to access the SimScale post-processor. This can either be done by selecting ‘Solution Fields’ in the simulation tree or ‘Post-process results’ from the run panel.

#### 5.2.1 Main Board Temprature

At first, we will have a look at the temperature of the Main Board. Therefore hide the cutting plane and choose ‘Temperature’ to display on your part as the Coloring option. Change the units to $$°C$$, and in order to improve the quality of your visualization by making the color transition smoother, right-click on the legend bar at the bottom, and select the ‘Use continuous scale‘ option as shown in step 3 below:

1. Toggle off the visibilty of the cutting plane.
2. Switch the coloring unit to ‘$$°C$$’
3. Rightclick on the temprature scale and select continuous scale.

To have a look at the temperature distribution on specific parts of your model, you can hide them so that only the chosen parts are displayed. For example, to visualize the internal parts, hide the ‘Housing‘ on the geometry tree list, or activate the parts selection, select the housing and right-click to hide the selection.

We can see how the temperature not only affects the parts but also the mainboard PCB.

We can see that the temperature of the chips at the outlets is quite high. This makes sense because they are not exposed to the middle of the flow. Furthermore, some heat has already been transferred to the air at the beginning of the domain, so its capacity to lower the temperature has decreased.

### 5.3 Cutting Plane

Next, we want to take a look at a section of the electronics box.

1. Toggle off the Parts color to hide all the parts.
2. Toggle on the Cutting plane to make it visible
3. Choose the ‘X‘ axis. It will automatically generate a plane normal to this axis, coincident with the origin of the model.
4. Choose ‘Temperature’ as the Coloring parameter.
5. Toggle on Vectors;
6. Switch the Coloring to ‘Solid color’ and choose a white color.
7. Set the Scaling factor to ‘0.08’ and the Grid Spacing to ‘0.0093’.

After the setup of the cutting plane, the result should look similar to this:

### 5.4 Streamlines

Finally, to view the streamlines, add the Particle Trace filter. Keep in mind that you need to activate the visibility of the parts coloring in order to use the openings as seed faces. You can also toggle off the cutting plane.

1. Create a new ‘Particle trace’ by selecting the icon from the filter section
2. Toggle on Parts color and toggle off the section plane.
3. Select the seed point and select the inlet faces of the electronic boxs.
4. The # Seeds horizontally represents the number of streamline coloums along the x-axis. Make sure it is big enough that it covers the whole y dimension of the domain. An input of ‘10′ should be fine for this case. The # Seeds vertically represents the number of rows along the z-axis. Set it to ‘6’. Set the Spacing to ‘0.0073’;

After finishing the setup, and hiding the housing and flow field, the result should look similar as presented in the figure below.

For a general overview of SimScale’s online post-processing capabilities, this documentation can be used.

Congratulations! You finished the tutorial!

Note

If you have questions or suggestions, please reach out either via the forum or contact us directly.

Last updated: April 8th, 2022