Free Tetrahedral Meshing of a Piston Geometry

The free meshing algorithm using tetrahedral elements is the most general meshing technique, and does not pose any constraints on the structure of the geometry. Hence you can use it to mesh any object. There are nine predefined parameter sets for the mesher, ranging from “extremely fine” to “extremely coarse.” These settings result in a good mesh for most geometries and simulation problems. In addition you can tune the mesh parameters individually, as demonstrated in this tutorial.

Model Definition

Create a tetrahedral mesh for the geometry of an engine piston as shown in the following figure.

As you can see the geometry contains small details such as fillets and chamfers. To better resolve these details with the mesh you will work with the following mesh parameters:

•

Minimum element size

•

Curvature factor

•

Resolution of narrow regions

•

Maximum element growth rate

You will also learn how to use the tools for assessing the mesh quality.

COMSOL_Multiphysics/Meshing_Tutorials/piston_mesh

Modeling Instructions

From the menu, choose .

In the window, click

In the window, click

In the toolbar, click

In the window for , locate the section.

Click .

Browse to the model’s Application Libraries folder and double-click the file piston_quarter.mphbin.

Click .

Mesh 1

In the window, under click .

In the window for , click

The window indicates that there are roughly 22,000 tetrahedral elements in this mesh.

Assume that the current mesh does not resolve details such as fillets and chamfers sufficiently for your simulation needs and a finer parameter setting is required. This would be the case for a stress analysis of the part.

Locate the section. From the list, choose .

Click

This mesh consists of approximately 320,000 elements. Many of the finer details of the geometry are adequately resolved, but there is a significant increase in the total number of elements compared to the Normal mesh setting.

In the following you will test how to tune mesh parameters to refine the mesh only on selected boundaries.

Mesh Statistics

Continue with examining the quality of the mesh.

Right-click and choose .

The window contains details about the mesh, including the number and type of elements, and a histogram of element quality.

The default quality measure, Skewness, is suitable for most types of meshes, and it is based on the equiangular skew that penalizes elements with large or small angles as compared to the angles in an ideal element. This quality measure is also used when reporting bad element quality during mesh generation.

The element quality has a value between 0 and 1, where 1 describes a perfectly symmetric element and 0 describes a degenerated, or completely flat, element. For 3D meshes in general a minimum quality of about 0.1 means a satisfactory mesh.

However, this depends on the type of geometry and physics application. Note also that the quality number is calculated based on the linear elements.

Meshing with predefined parameter sets usually results in a mesh with quite good quality. According to the information under the section , the present mesh has an average quality of 0.65 with a minimum quality of 0.2.

The histogram reveals the element quality distribution. In this case, the elements with low quality, represented by the tail on the left of the distribution plot, represent a very small fraction of the mesh.

Before adjusting individual mesh parameters start by restoring the mesh with the normal size settings.

Right-click and choose .

In the window, under click .

In the window for , locate the section.

From the list, choose .

Click

Meshing Sequence

Size

Right-click and choose .

You can now access and modify the default meshing sequence that appears under the node.

The first feature node in the meshing sequence is a global attribute node, since it influences all subsequent operation nodes in the meshing sequence. This first node cannot be deleted from the sequence.

Instead of editing parameters of the global Size node add a Size node to the Free Tetrahedral 1 mesh operation.

Size 1

In the window, right-click and choose .

The node is a local attribute node because it only applies to its parent mesh node.

Resolution of Curvature

In the window for , locate the section.

From the list, choose .

In the window, click .

Select the boundary highlighted in the figure below (Boundary 39).

By selecting only one of the fillets you can save time generating the mesh while testing parameter values. You will be able to change the selection of the node to all boundaries after you have found the right set of parameters.

In the window for , locate the section.

Click the button.

Locate the section. Select the check box.

In the associated text field, type 0.2.

The parameter determines the size of boundary elements compared to the curvature of the geometric boundary. The curvature radius multiplied by the curvature factor gives the maximum allowed element size along the boundary. A lower value gives a finer mesh along curved boundaries.

Click

Zoom in on the selected boundary for a closer look at the mesh.

It seems that reducing the resolution of curvature had almost no effect on the number of mesh elements on the fillet. The reason is that another mesh parameter limits the minimum element size allowed in the mesh.

Minimum Element Size

In the window, under click .

In the settings window, locate the section.

Select the check box.

In the associated text field, type 0.0002.

The value in the field specifies the minimum allowed element size. You can use this value to, for example, prevent the generation of many elements around small curved parts of the geometry.

Click

This time the selected boundary has a much finer mesh. Adjust the mesh again by increasing the resolution of curvature.

In the window for Size, locate the section.

In the text field, type 0.45.

Click

Now assume that you also want a better resolution of narrow regions with no curvature such as chamfers.

Resolution of Narrow Regions

In the window, click .

Add the face highlighted below to the selection. The selection should now contain both boundaries 8 and 39.

In the window for , locate the section.

Select the check box.

In the associated text field, type 2.

The mesh parameter controls the number of element layers that are created in narrow regions (approximately). If the value of this parameter is less than one, the mesh generator might create elements that are anisotropic in size in narrow regions.

Click

Assume that you are happy with the parameter settings for curved and narrow regions. Now apply these for all boundaries of the geometry.

Locate the section. From the list, choose .

Click

Click the

button in the toolbar to get the view in the figure below.

The fine details of the geometry are resolved satisfactorily with this mesh of approximately 324,000 tetrahedral elements.

Continue with checking the mesh quality.

In the window, right-click and choose .

Compared to the mesh with the predefined mesh parameter set, the average quality is slightly less and the minimum quality is also lower. This is expected because the boundaries are finely meshed and the elements are growing toward the inner parts of the geometry according to the parameter set specified in the global node. Allowing even higher element growth will reduce the number of elements further and will result in even lower element quality.

Maximum Element Growth

Reduce the number of mesh elements further by specifying the rate of growth from the small elements on the surface to the larger elements inside.

Size

In the window, click .

In the window for , locate the section.

Click the button.

Locate the section. In the text field, type 1.8.

The parameter determines the maximum rate at which the element size can grow from a region with small elements to a region with larger elements.

In the window, click .

In the window for , click

The mesh now consists of approximately 173,000 elements while keeping the fine mesh on curved and narrow boundaries.

Right-click and choose .

As expected the increase of the growth rate parameter results in an even lower quality. The average quality is now 0.61, and the minimum quality is 0.16, which are both acceptable numbers.

A mesh plot can help with localizing the worst quality elements.

In the toolbar, click

Results

Mesh 1

The plot is added to the under the section of the window. The default mesh plot that appears in the window contains the surface elements colored according to quality.

In the window for , click to expand the section.

Select the check box.

From the list, choose .

In the text field, type 0.005.

Mesh Plot 1

In the window, click .

In the window for , locate the section.

Select the check box.

In the toolbar, click

You can now see 0.5% of the tetrahedral elements with the worst quality. These are mostly located in the regions where the elements are growing from the surfaces toward the inside of the geometry.