As a first step, we need to create a new simulation. To create a simulation, left-click on the CAD model and then on the ‘Create Simulation’.
This dialog box allows the user to select the simulation model. Click on the ‘Conjugate Heat Transfer‘ simulation, and then click ‘Create Simulation’.
The default settings for the simulation are kept the same. Save the simulation model by clicking on the tick mark.
2.1 Default Settings
The following figure shows the standard meshing setup:
Click on the Mesh icon to create a new mesh.
Choose the ‘Standard’ Algorithm.
For the first mesh we keep the default settings:
Keep Automatic boundary layers activated. If the Boundary Conditions (BC) are set and a simulation run is performed, this option will help mesher to generate boundary layers (BL) automatically.
Physics based meshing refines the mesh automatically according to the assigned boundary conditions
Hex element core generates hexahedral elements inside the interior domain.
Specify the Number of processors for the meshing operation (16 in this tutorial). In general the automatic option is a good choice. The more cores does not necessarily mean faster calculation.
Give a name to your mesh by double-clicking on the mesh title.
Once the mesh generation is finished, check the mesh info. You can see how many cellsand nodesare generated, how much timedid it take and how many core hours consumed. You can also expand the Event log to see additional information regarding the mesh.
From the current view, we only see the mesh on the surfaces of the flow domain. You can hide the flow domain to see the mesh on the Heat sink and Chip parts. Under the Mesh tree, left-click on the eye icon next to the Air domain to hide it.
If you had multiple volumes to hide, the following workflow would be more useful:
Use theSelect Volume feature.
Using right-click, select multiple mesh regions.
Left-click on the workbench and select Hide selection option.
The current mesh looks too coarse. For simulating heat sinks, it is 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.
2.2 Global Refinement
You can simply increase the fineness level, but once you start a new mesh operation, the old one will be deleted. To keep the old one, right-click on the mesh and select create a new mesh option. In new mesh settings, select finenesslevel ‘7’ by using the slideror double-clicking on fineness value and assigning 7. Name the new mesh and generate it.
The new mesh contains 1.5M elements, which is double the previous one. Generated number of elements is correlated with many geometrical properties, therefore it is hard to predict how large/coarse an updated mesh will become.
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.
2.3 Local Refinement
Create a new mesh refinement, using fineness level 5. Measure the fin thickness, using the ruler in the workbench. The thickness of the fins is approximately 2mm. Click on the ‘+’ icon next to ‘Refinements‘ under the ‘Mesh‘. Select Local element size. This is a refinement option to limit the cell sizes on surface elements.
Assign maximum edge length and select small surfaces. The maximum element size will ensure that there isn’t any element with a larger size than what we assign. To keep the mesh density low as possible, avoid selecting large surfaces of the heat sink. The maximum edge length of 0.001m will ensure to create a minimum of 2 elements across the thickness.
Surface refinement increased the mesh density on fins significantly. So far, we learned how to visualize the mesh on surfaces. This does not give any information regarding the interior elements. A Mesh clip is recommended to see the interior elements.
Depending on the mesh size, generating a mesh clip will take some time.
As can be seen, while surface elements are tetrahedral, interior elements are hexahedral. from the heat sink region to the air domain, mesh size suddenly increases. 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.
2.4 Region Refinement
Is it possible to keep the previous mesh setting and updating it with region refinement? To do that, click on the current mesh and Duplicate the mesh.
Click on the ‘+’ icon next to Refinements under the Mesh. Select Region refinement. This is a refinement option to limit the cell sizes within a volume.
The maximum edge length defines the maximum element size within the defined region. Assign it as 0.004m. Next, we need to define the region. If there was a region that was created earlier, you could simply activate it. Here, we need to create a new region by clicking the ‘+’ icon next to Refinement regions. Select the cartesian box to define the region as a box:
Next, define the coordinates of the cartesian box. It should fully cover the heat sink and chip. Consider the possible flow motion while deciding where the refinement region.
Go back to the region refinement and assign the new cartesian box.
Generate the mesh, and use cutting planes to visualize the mesh.
The mesh resolution looks better now.
To correctly model the flow through the fins, the boundary layer has to be resolved accurately. This can be achieved by refining the mesh in the regions close to the walls. A practical and cost-effective approach is to create layers on the walls. As a default, Automatic BL option adds 3 layers:
BL’s can be also generated manually. This will let you have full control over the BL generation.
2.5 Inflate Boundary Layers
Duplicate the previous mesh and rename it.
To add a BL refinement, click on the ‘+’ icon next to Refinements under the Mesh.
Select the Inflate boundary layer setting.
Assign 5 to Number of layers. This will ensure that 5 layers will be generated on selected surfaces. First, hide the solid parts, then use box select to select the air surfaces around the solid parts.
You can control the BL thickness by specifying the growth rate or the first layer thickness.
Never create BL’s on inlet and outlet surfaces, they should only be applied to surfaces representing physical walls.
Generate this mesh and see the layers by mesh clip.
Up to now, we’ve learned how to use automatic and manual mesh refinements. There are a few other settings you can consider. Let’s turn back to the initial mesh (Default mesh) we created. You can select an old mesh by simply clicking the current mesh and navigate to the one you would like to select.
Check your CAD model again by hiding the air domain. You will see that there are some small faces printed on the heat sink. These faces are obviously not relevant for this study, on the other hand, they will increase the mesh density or might even cause mesh failure. Now view the mesh to confirm that they cause undesirable mesh density.
Next we will learn how to control the global mesh size, adding gap refinements, and solve small feature issue.
2.6 Manual Sizing
Create a new mesh and assign switch the Sizing to Manual. You will see the Manual edge length option. This will let you limit the largest cell size in the whole domain.
2.7 Advanced Settings
Expand the Advanced settings feature. You will see the following settings:
Small feature suppression: This will help to suppress small faces
Number of Gap elements: This will help to automatically generate up to 4 elements in gaps
In many cases, the mesher can suppress small features. In this example, the smallest edge of the printed faces is 0.2mm. To be able to suppress them, we should use a bigger size limit.
Assign 0.0005m to the small feature suppression.
The number of Gap elements feature sets automatic sizing to the elements inside gaps. In this view, we cannot see the elements inside the air domain, but usually, element size on a domain surface is identical to the neighbor element. Therefore element sizes on the heat sink can give an idea regarding the air element sizes in the gaps.
You do not have to assign an integer to the number of gap elements option, but you can also use integers. Here is how sizing works:
Assign 2 to the number of Gap elements option
Once the mesh is completed, you will see that:
The maximum element size created the elements with defined sizing limitations.
Small features on the side of the heat sink are neglected from mesh refinement.
There are 2 elements in every gap.
Congratulations! This concludes the standard meshing tutorial.
Last updated: April 29th, 2020
Did you find this article helpful?
How can we do better?
We appreciate and value your feedback.
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.