The starting project contains a heat sink, a chip, and the flow region. The following picture demonstrates what should be visible after importing the project.
1.1 Create the Simulation
Since we have a flow region and solid parts in the geometry, there will be interfaces between these volumes. In these cases, to enhance the detection of contacts, it’s recommended to run an imprint operation.
In this tutorial, the Imprint operation has already been performed. Therefore, we can directly proceed to ‘Create the Simulation’:
Now, the analysis type widget opens. From the list, select ‘Conjugate Heat Transfer’, and click once more on ‘Create Simulation’:
After creating a simulation, the simulation tree loads in the left-hand side panel. The global simulation settings will remain as default.
2. Simulation Setup
In section 2 of the tutorial, we set up a simple simulation to make use of the physics-based meshing option. If you do not interested in the physics-based meshing option, you can directly jump to section 3 Meshing.
Specify gravity under Model. It will be -9.81 m/s² in the y-direction:
In the simulation tree, please expand the Materials tab. Click on the ‘+ button’ next to Fluids and choose ‘Air’ from the fluid materials library.
Afterward, assign it to the Air domain.
Now repeat the process for the two Solids. Assign Aluminium to the Heat sink and Silicon to the Chip:
For the Chip volume, the material will be Silicon:
2.3 Boundary Conditions
Click on the ‘+ button’ next to Boundary conditions. Select ‘Natural convection inlet/outlet‘ and assign it to the 6 outer faces of the air domain.
3. Standard Mesh
The standard meshing tool will be used to mesh the heat sink. A total of six different meshes will be created, to show how the configuration parameters affect the resulting mesh. Make sure to check this documentation page for the standard mesh settings.
To create a mesh, please navigate to Mesh in the simulation tree. A tab with options will open.
Let’s give a brief overview of the basic settings:
Cell Sizing can be either manual or automatic. With Manual sizing, it’s possible to specify a maximum edge length for cells in the entire domain;
In the Fineness sliding bar, users can specify global levels of fineness to their meshes;
Automatic boundary layers generates layers automatically, based on the boundary conditions set by the user;
With Physics-based meshing, the regions near inlets and outlets are automatically refined. This option is useful to capture high gradients in these regions. Furthermore, if any advanced concepts are defined (such as porous medium and power sources), the algorithm automatically assigns cell zones to these volumes. To use physics-based meshing, users have to fully set up their simulation before creating a mesh.
When the Hex element core is enabled, the standard mesh becomes hybrid, generating tetrahedral cells close to the walls and hexahedral cells distant from walls.
3.1 Mesh One: Default Settings
Now it’s possible to use the default settings. Please head back to Mesh and hit ‘Generate‘.
After clicking to generate the mesh, the following warning message will appear:
The warning message states that the current setup will be used for the physics-based meshing automatic refinements. If the boundary conditions change, the mesh won’t be automatically updated. Since our setup won’t change, we can ignore the warning message and generate the mesh.
The standard mesh takes about 5 minutes to complete. When it finishes running, you can hide the Air domain to inspect the solid parts:
The default mesh is too coarse. For heat sinks, it’s recommended to generate a minimum of 2 or 3 elements across the fin thickness. Let’s generate a new mesh with a Fineness level of 7.
3.2 Mesh Two: Changing Global Fineness
The settings for the second mesh will be the same, except for the global level of Fineness.
Follow the steps below to create a new mesh:
Now simply adjust the Fineness slide bar to 7 and ‘Generate’ the second mesh.
The second mesh takes roughly 10 minutes to run. Let’s now compare the heat sink discretization using the first and second meshes:
The fineness level changes the mesh size globally. Comparing the new and previous meshes, there is almost no obvious change in the element size on the heat sink. This shows that a large portion of refinement is performed in the air domain. Local refinement on heat sink and chip would be a more cost-effective way to generate a mesh.
3.3 Mesh Three: Local Element Size Refinement
Using the steps from figure 16, please create another mesh. To enhance the discretization of the fins, we will use a Local element size refinement. The other settings remain default.
To create a refinement, click on the ‘+ button’ next to Refinements and select Local element size.
With local element size, you can specify a maximum element size for selected entities. It’s particularly useful to increase the resolution on small faces.
For the heat sink model, each fin is 0.002 meters thick. A Maximum element size of 0.001 meters will ensure at least 2 elements across the thickness.
Set up the refinement as below. To save time, assign it to a pre-saved topological entity set named Local element size refinement.
Now we can go back to the Mesh tab and hit ‘Generate’.
Now, with the controlled cell size, it’s possible to see a big difference in the fins’ discretization.
So far, we have learned how to visualize the mesh on surfaces. However, this does not give us any information regarding the interior elements. For such cases, a Mesh clip can be used to see the interior cells. Please follow the steps below:
Click on the Mesh clip icon;
Rotate or translate the cutting plane using the sliding bars;
‘Generate’ the mesh clip.
Now the interior is visible. We can see the hexahedral cells in the middle of the domain. By zooming in to the fins, the boundary layers can be seen:
3.4 Mesh Four: Region Refinement
From the image above, we can see that mesh size suddenly increases when it transitions from tetrahedral to hexahedral cells.
While this is not a big deal in thermal conductivity, it may cause inaccuracy or even create instability in flow simulations. Additionally, due to the natural convection, hot air is expected to rise along the vertical axis of the heat sink. Therefore, a region refinement is recommended.
For the fourth mesh, let’s copy the third mesh and add a region refinement. To copy a mesh, follow the steps below:
Click on the arrow to access the mesh menu
Click on Copy mesh settings from…
Select the third mesh to copy all of its settings
After these steps, the fourth mesh can be set up. Click on the ‘+ button’ next to Refinements and create a Region refinement. The Maximum edge length defines the maximum element size within a region. Please input 0.004 meters.
Afterward, click on the ‘+ button’ next to Geometry primitives and select a Cartesian box.
Next, define the coordinates of the cartesian box, keeping in mind that it should fully cover the heat sink and chip. Consider the possible flow motion while deciding where to place the refinement region.
Go ahead and ‘Generate‘ the fourth mesh. This one has an improved discretization around the heat sinks. To visualize it clearly, we can create another Mesh clip:
3.5 Standard Mesh Five: Inflate Boundary Layers
By default, the Automatic boundary layers option creates 3 layers. However, you can change all of the layer settings, giving you full control over the layer generation.
Please copy the settings from the previous mesh and configure the new mesh as below:
For this mesh, we will only adjust the Number of layers to ‘5’. It is also possible to easily control the Layer gradation by either specifying the Growth rate or the First layer thickness. After adjusting the number of layers, we are ready to ‘Generate’ the fifth mesh.
The extra layers can be seen with a mesh clip. With this configuration, the near-wall profiles are captured more accurately.
3.6 Mesh Six: Advanced Settings
By expanding Advanced settings, you will find two additional parameters:
Small feature suppression represents a threshold to ignore small entities. Only entities larger than the input value are meshed.
The Gap refinement factor represents the number of cells in small gaps. It doesn’t necessarily have to be an integer.
On one of the sides of the heat sink, a lot of small features are present. Their smallest edge has about 0.2 mm of length. Naturally, gaps are also present, between the fins.
To see how both advanced settings work, please copy the settings of the very first mesh from this tutorial. Change Small feature suppression to 0.0005 meters and the Gap refinement factor to 2.
Comparing the first mesh to the advanced settings mesh, the differences can be seen clearly:
The 2 gap elements improve the discretization of the gaps between the fins, while the small feature suppression prevents the small faces from being meshed.
The small feature suppression setting can be particularly helpful when the CAD models are not very clean.
Congratulations! You have finished the standard meshing tutorial!
Strictly Necessary Cookies
Strictly Necessary Cookie should be enabled at all times so that we can save your preferences for cookie settings.
If you disable this cookie, we will not be able to save your preferences. This means that every time you visit this website you will need to enable or disable cookies again.