Conjugate Heat Transfer: Cooling of electronic sink¶
Please note that the interfaces are now automatically defined, and “Thermal coupled no-slip wall” boundary condition is automatically assigned to these interfaces, hence the interface assignment is not required.
The conjugate heat transfer method show processes that have temperature variations because of thermal interactions between solids and fluids. This tutorial provides a step-by-step guide on how to set up a conjugate heat transfer simulation for an electronic cooling sink used for removing the heat from a PCB.
The material library provides pre-defined Solid and Fluid materials with the required properties at standard conditions. It will be shown, how these can be easily added and used. The user may modify these properties based on the requirements.
The tutorial project is a sample Electronic cooling sink which consists of 3 solid regions and 1 fluid region. The solid regions are two FB-4 chips, which have a higher initial temperature, and a heat sink over one of the chips. The air flows over the solid regions to remove the heat from it.
The mesh for the project needs to be created using the guidance provided in this tutorial to create multi-region mesh using the SimScale platform.
Import tutorial project¶
- To start this tutorial, you have to import the tutorial project into your ‘Dashboard’ via the link above.
Create a CHT simulation¶
- To create a new simulation, switch to the Simulation Designer tab and click on “New simulation”. Enter a name for the simulation e.g. ‘Electronic cooling sink - CHT’ and click OK.
- From the analysis type choose: ‘Fluid Dynamics’ section of the analysis types, then ‘Conjugate heat transfer’ and setup the properties as shown in the figure below and click on ‘save’. After saving a new tree will be automatically generated in the left panel with all the parameters and settings that are necessary to completely specify such an analysis.
- All parts that are completed are highlighted with a green check. Parts that need to be specified have a red circle. While, the blue circle indicates an optional settings that does not need to be filled out
Selecting a domain¶
- Now, click on the “Domain” node from the tree and select the mesh which was created following the mesh tutorial, to assign it to this simulation from the options panel. Clicking on ‘save’ will automatically load the selected mesh in the viewer.
Setting up the Model:¶
Adding materials to the domain¶
- Gravity needs to be enabled to account for buoyancy effects. Select “Model” node from the subtree and change the values as shown in the figure
- Then we will add the materials from the ‘Material Library’ for fluid and the solid phases. First, we start with clicking on sub-tree “Materials”. Select “Fluid” from the tree and click on “New” from the options panel as shown. For better visualization you can also render the the domain to “surfaces”.
- We do not need to enter the material properties as we will import predefined ones by clicking on “Import from material library” at the top.
- This pops-up a ‘Material Library’ from which we select “Air” and click on save. This will then automatically load the standard properties for air.
Assign this material to the fluid volume called ‘solid_0’ and click ‘Save’.
- Similarly select the “Solid” node from the sub-tree and click “New”. Import the material properties by clicking “Import from material library”, select ‘Aluminium’ and assign this material to the volume “solid_1”, which is the heat sink. Click the ‘Save’ button.
- Add another solid material to represent the FB-4 chips by selecting ‘Solid’ from the sub-tree and then clicking “New”. Import the material property of ‘Copper’, but change the properties as shown in the following figure to satisfy the material requirement. Assign this to volumes “solid_2” and “solid_3”
Initial Conditions (Defining initial flow variables and temperatures of different regions):¶
- The next tree item “Initial conditions” allows to define the initial velocity, pressure and temperature for the regions. For pressure and velocity we keep the default values. Then click on ‘Temperature’, change type to ‘Subdomain-based’ and click ‘save’ by keeping “Default Temperature value” of 293 K. This means for now all the regions are maintained at 293 K. Now click on “New” under ‘Subdomains’ to add different domain.
- Rename the subdomain, enter the settings as shown in the figure below (363 K for the FB-4 chips) and assign it to the volumes “solid_2” and “solid_3”, then click on ‘save’.
- Similarly click on ‘Temperature’ node of sub-tree add the other two sub-domains of ‘Heat_Sink’ and ‘Fluid’ one-by-one, with properties as shown in the following figure and assign it to the volumes “Zone_solid_3” and “Zone_fluid” respectively.
Now, we come to define the boundary conditions.
- Click on “Boundary conditions” in the tree and click “New” button to create a new entry as shown below.
- Rename the entry as “Inlet” and specify the values shown in the figure below, assign inlet faces for this boundary condition and click on save.
- Add another boundary condition (as before), rename it as “Outlet” and specify the settings as shown in figure below, assign the outlet faces for this boundary condition and save it. Faces can be added by selecting them in the viewer, and then clicking “Add selection from viewer”.
- Then add the boundary representing the fluid walls, named “FluidWalls”, by following the settings from the following image. Assign walls of the fluid domain for this boundary condition. Faces can be added by selecting them in the viewer, and then clicking “Add selection from viewer”.
- The settings of bottom face of the PCB FB-4 needs assignment. This is done as shown below, with the name “ChipBottom”.
- Lastly, add the bottom face of heat sink, rename it to “HeatSinkBottom” and specify the settings as shown in the following figure.
Please make sure no interface is assigned to a boundary condition.
- Based on the type of problem, we modify some of the numerics for better stability and convergence on the simulation. For this problem we can keep the default numerics, therefore, no change is required for numerics.
- Next, in simulation control we define some main control settings such as start and end times, time step size, auto time-stepping and number of processors for this simulation run. Follow the figure below to set up as shown and click ‘save’.
- Finally click on “Simulation Runs” and click on “New” from the options panel. Then click “Start” to start the simulation run. That’s it ...!
- Once the run finishes, the results can be post-processed by clicking on “Post-processor” tab and loading the results by clicking on “Solution fields” as shown below.
- Select the fluid domain and click ‘Add Filter’ to create a ‘Slice’ with the following settings
- The parameters need to be changed to view the temperature changes across the domain.