Fill out the form to download

Required field
Required field
Not a valid email address
Required field

Documentation

Creating a Standard Mesh on the Example of a Heat Sink

This tutorial demonstrates how to create meshes using the standard mesh tool. To showcase the effect of the setup parameters, a total of 6 meshes will be created, using a heat sink as the model.

heat sink discretization standard mesh
Figure 1: Heat sink mesh created with the standard algorithm.

Overview

This meshing tutorial teaches users how to:

  • Create meshes using the standard meshing algorithm;
  • Apply different types of mesh refinement;
  • Use all basic and advanced settings;
  • Inspect the mesh.

Note

The usual workflow in SimScale is the following:

  1. Prepare the CAD model for the simulation;
  2. Set up the simulation;
  3. Create the mesh;
  4. Run the simulation and analyze the results.

Since this is a meshing tutorial, it will focus on the third step.

1. Prepare the CAD Model and Select the Analysis Type

First of all, click the button below. It will copy the tutorial project containing the geometry into your workbench.

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.

heat sink geometry for standard mesh tutorial project
Figure 2: Imported CAD model of a heat sink, chip, and flow region in the workbench.

1.1 Getting Started

Since we have a flow domain and solid parts in the geometry, there will be interfaces between these phases. Before creating a simulation, run an ‘imprint‘ operation to detect these contacts automatically. Follow the steps below:

imprint operation to detect contacts
Figure 3: Running an imprint operation to automatically detect contacts between solid and fluid.
  1. Right-click on the geometry name;
  2. Select and ‘start‘ the ‘imprint‘ operation.

1.2 Create the Simulation

To create a simulation, click on the ‘imprint‘:

creating simulation after imprinting
Figure 4: Creating a new simulation for the geometry.

Hitting the ‘Create Simulation’ button leads to the following options:

library of analysis types available
Figure 5: Analysis types available in SimScale.

Choose ‘conjugate heat transfer‘ as the analysis type and ‘create the simulation’.

2. Simulation Setup

Note

We set up a simple simulation to make use of the physics based meshing option.
If you do not care about it, you can directly jump to section 3 Meshing.

2.1 Model

Specify gravity under ‘model‘. It will be -9.81 m/s² in the y-direction:

gravity natural convection
Figure 6: Specifying gravity in the model tab.

2.2 Materials

Click on the ‘+ button’ next to ‘fluids‘. From the materials library, choose ‘air‘.

materials library showing fluids
Figure 7: Fluid materials library.

Afterward, assign it to the ‘air domain‘.

assigning a material to the flow region
Figure 8: Assigning air to the air domain.

Now repeat the process for the two ‘solids‘. Assign ‘aluminium‘ to the ‘heat sink‘ and ‘silicon‘ to the ‘chip‘:

assigning material to a heat sink in a conjugate heat transfer analysis
Figure 9: The heat sink volume consists of aluminium.

Similarly, for the chip:

assigning material to a chip in a conjugate heat transfer analysis
Figure 10: Assigning silicon as material to the chip volume.

2.3 Boundary Conditions

Click on the ‘+ button’ next to ‘boundary conditions‘. Select ‘natural convection inlet/outlet‘. Assign it to the 6 outer faces of the ‘air domain‘.

heat sink natural convection simulation
Figure 11: Boundary condition to simulate natural convection for a heat sink geometry.

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 configuration parameters affect the resulting mesh.

Make sure to check this documentation page for the standard mesh settings.

To create a mesh, the first step is to click on ‘mesh‘ in the simulation tree. A tab with options will open.

default settings for the standard meshing tool
Figure 12: Default settings for the standard mesher.

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‘ generate 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. To use this option, users have to fully set up their simulation before creating a mesh.
  • When the ‘hex element core‘ is enabled, the standard mesh becomes hybrid, with 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‘.

standard mesh default settings generation
Figure 13: Generating a standard mesh with default settings.

The standard mesh takes about 5 minutes to complete. When it finishes running, hide the ‘air domain‘ to inspect the solid parts:

heat sink mesh default settings
Figure 14: Heat sink mesh using the standard algorithm with default settings.

This 1.2M cell 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 ‘fineness‘.

Follow the steps below to create a new mesh:

creating a new mesh in simscale
Figure 15: Steps to create a brand new mesh.

Simply adjust the ‘fineness‘ slide bar to 7 and ‘generate‘ the second mesh.

heat sink mesh changing global fineness
Figure 16: Settings for the second heat sink mesh, using fineness 7.

The second mesh takes about 8 minutes to run and consists of 1.8M cells. Let’s now compare the heat sink discretization using the first and second meshes:

comparing discretization heat sink different fineness
Figure 17: Mesh using global fineness 7 (left) and mesh created with default settings (right).

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

Create another mesh. To enhance the capture 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‘. Select local element size.

creating a local element size refinement
Figure 18: Creating a new refinement for a standard mesh.

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‘.

assigning a refinement to a set of faces
Figure 19: Assigning a local element size refinement to a previously created topological entity set.

Now go back to ‘mesh‘ and ‘generate‘ it.

using region refinement standard mesh
Figure 20: Overview of the configuration for the third mesh.

Now, with the limited cell size, it’s possible to see a big difference in the fins. The number of cells is now at 2.8M.

local element size refinements to get more cell density
Figure 21: Effects of the local element size refinement on cell density.

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 cells. Follow these steps:

creating a mesh clip
Figure 22: Steps to create a mesh clip.
  1. Click on the ‘mesh clip‘ icon;
  2. Rotate or translate the cutting plane using the sliding bars;
  3. ‘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:

standard hybrid mesh clip showing internal faces
Figure 23: Mesh clip of a heat sink geometry, highlighting layer generation on the walls.

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 refinement.

To copy a mesh, follow the steps below:

copying an existing mesh
Figure 24: When you copy a mesh, all mesh settings, including refinements, are copied to the new one.
  1. Click on the arrow access the mesh menu;
  2. Click on ‘copy mesh settings from…‘;
  3. Select the third mesh.

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‘. Select a ‘cartesian box‘.

creating a geometry primitive for a region refinement
Figure 25: Setting up a region refinement.

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.

region refinement cartesian box dimensions
Figure 26: Specifying dimensions for a cartesian box. Assign this box to the region refinement.

Go ahead and ‘generate‘ the mesh. This one consists of 3.5M elements and takes roughly 13 minutes to finish. Create a ‘mesh clip‘ for it:

region refinement standard mesher
Figure 27: Effect of a region refinement. This mesh is better suited to capture natural convection.

3.5 Standard Mesh Five: Inflate Boundary Layers

By default, the ‘automatic boundary layers‘ option creates 3 layers. You can also specify boundary layers manually, giving you full control over its generation.

Copy the settings from the previous mesh and follow the steps below:

inflate boundary layer refinement
Figure 28: The boundary layer refinement should only be assigned to solid walls and never to inlets and outlets.
  1. Click on the ‘+ button’ and create an ‘inflate boundary layer‘ refinement;
  2. Change the number of layers to 5;
  3. To quickly assign all heat sink and chip walls, hide the ‘air domain‘ by clicking on the eye next to it;
  4. Right-click in the viewer and ‘assign all visible‘ parts.

It’s easy to control the boundary layer thickness by either specifying the growth rate or the ‘first layer thickness‘.

Before generating the mesh, remember to disable ‘automatic boundary layers‘.

generating a standard mesh with manual boundary layer addition
Figure 29: Standard mesh with manual boundary layers.

The extra layers can be seen with a mesh clip. With this configuration, the near-wall profiles are captured more accurately.

boundary layers created with manual refinement on a standard mesh
Figure 30: Manually created boundary layers on the fin.

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.

small features and gap elements in a heat sink
Figure 31: Highlighting small features (left) and one gap element (right) within the heat sink.

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.

standard meshing tool advanced settings
Figure 32: Advanced standard mesh settings.

Comparing the first mesh to the advanced settings mesh, differences can be seen clearly:

standard mesh small feature suppression
Figure 33: Mesh with feature suppression and gap elements (top) versus default settings mesh (bottom).

The small features are no longer captured. As a result, the cell count dropped from 1.2M cells to 743k.

Congratulations! You have finished the standard meshing tutorial!

Note

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

Contents
Data Privacy