Advanced Tutorial: Thermomechanical Analysis of an Engine Piston

This article provides a step-by-step tutorial for a thermomechanical analysis of an engine piston under maximum pressure and temperatures.

Overview

This tutorial teaches how to:

• Set up and run a thermomechanical analysis.
• Assign topological entity sets in SimScale.
• Assign boundary conditions, material and other properties to the simulation.
• Mesh with the SimScale standard meshing algorithm.

We are following the typical SimScale workflow:

1. Preparing the CAD model for the simulation.
2. Setting up the simulation.
3. Creating the mesh.
4. Run the simulation and analyze the results.

1. Prepare the CAD model and select the analysis type

Firstly, you can click the button below and it will copy the tutorial project containing the geometry into your own workbench.

The following picture shows what should be visible after importing the tutorial project.

1.1 Create the Simulation

The first step you will do is to create the simulation.

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

Choose Thermomechanical as analysis type and click the ‘Create Simulation’ button to confirm. After that, a simulation tree showing you all the necessary steps to set up all your simulation will show in your workbench.

1.2 Create Topological Entity Sets

Prior to setting up the simulation, we recommend creating topological entity sets. You can do this at any point of the simulation setup, however, it is easier to do it in the beginning.

The sets for the top, the rings and the ring grooves have already been created for you according to the following picture:

Now, you will only need to create the set for the interior and the skirt of the piston, which is everything other than what is already assigned to sets. Here are the steps that you can follow:

1. Hide all the existing topological entity sets.
2. Activate the box selection.
3. Select all remaining parts.
4. Hit the ‘+’ next to Topological Entity Set and give it a name.

2. Assigning the Material and Boundary Conditions

In this section we will define the physics of our model.

2.1 Model (Gravity)

In the first step, we define the magnitude and direction of the gravity by assigning the values below:

The magnitude of the gravity that we use is 9.81 \(m^2/s\) in the direction -1 in \(e_y\).

2.2 Define a Material

Afterwards, we will define the material of our piston and we will use Aluminium as the material.

2.3 Assign the Boundary Conditions

A thermomechanical analysis will need two boundary conditions which are the thermal boundary conditions and the mechanical boundary conditions we will set up both in this section.

a. Thermal Boundary Conditions

We will use a Convective heat flux boundary condition as our thermal boundary conditions. You can therefore add a boundary condition by hitting the ‘+’ and select ‘Convective heat flux boundary’ condition:

Following the above instructions open the setup options for convective heat flux. We will define them according to the picture below:

1. Firstly, you can set the \(T_0\) Reference temperature as 741 \(°C\) and the Heat transfer coefficient as 450 \(W/(K.m^2)\).
2. Next, you will need to define the surface where the boundary condition is applied. For example, this is the boundary condition for the top of the piston.

Follow this procedure for each row within the table below:

Entity Set	Reference temperature [°C]	Heat transfer coefficient [W/(K*m^2)]
Top	741	450
Ring 1	180	150
Groove – Ring 1	180	1000
Ring 2	160	150
Groove – Ring 2	160	400
Ring 3	140	150
Groove – Ring 3	140	400
Interior and skirt	120	650

b. Mechanical Boundary Conditions

Now it is time for the mechanical conditions, which are three pressure definitions (top and the first two rings) and two remote displacements. For example, we will assign a pressure boundary condition to the top of the piston.

By following the same process as before, you can select the pressure boundary condition in the lists of boundary conditions. After that, we will use a pressure value of 2e7 \(Pa\) at the top face of the piston. The pressure boundary conditions for the other parts can be seen in the table below:

Entity	Pressure [Pa]
Ring 1	14e7
Ring 2	4e6

Now, you can create the two remote displacements and give them the following properties:

For the first remote displacement, we will apply it at the top pin of the piston with coordinate of the external points:

• x: 0 \(m\)
• y: -0.042 \(m\)
• z: 0.02028 \(m\)

For the second remote displacement at the opposite side of the piston, the remote point will have the coordinates:

• x: 0 \(m\)
• y: 0.042 \(m\)
• z: -0.01992 \(m\)

Now all boundary conditions are assigned and we can proceed to creating the mesh.

3. Mesh

We will use the standard algorithm for our mesh, which is a good choice in general as it is quite automated and delivers good results for the most geometries. For this tutorial, we will generate a second order mesh.

You will only need to change the Sizing to Manual and set our maximum edge length as 1.8e-3 m and enable the 2nd order elements toggle. Make sure your setting look like the picture below:

When the mesh has been generated, you can observe your mesh. The mesh will look like this:

If we create a first order mesh, it will visually look exactly like the second order mesh, because the cell count is the same for both. However the second order mesh has additional nodes inbetween two connecting nodes, which helps to model deformations more accurate.

4. Start the Simulation

Finally, you can run your thermomechanical analysis for the engine piston and you can do this by clicking the ‘+’ button to start a simulation run.

Moreover, you can change the name of your simulation to your liking and start the simulation by clicking ‘Start’

5. Post-Processing

After the simulation has finished, you can access the simulation results by one from two options:

1. Click Solution fields under the simulation run.
2. Click the ‘Post-process results’ button form the run dialog.

You can choose what results to visualize by going to the Filters panel:

1. Expand the Parts Color section,
2. Select the desired field for Coloring.

5.1 Temperature

For example, we will plot the Temperature field:

To achieve this visualization we performed a couple of changes from the default state:

1. Changed the temperature units to \(°C\).
2. Selected ‘Use continuous scale’ in the context menu, opened by right-clicking on the color bar:

5.2 Von Mises Stress

We can also visualize the von Mises stress distribution with this same method:

1. Change the units to \(MPa\).
2. Use continuous scale.
3. Change the maximum value of the legend to ‘400’.

By lowering the maximum value of the color scale, we can create a threshold and find all the regions in the part where the stress exceeds this value. Those regions are colored in red in Figure 23, and are found in the support holes and the top face, where applied and reaction forces appear.

5.3 Deformation

Finally, we want to visualize the deformation of the piston head. For this, we first use the Add Filter button in the Filters panel to create the Displacement plot:

You might notice that the deformation is not apparent. This happens because the magnitude of the deformations is relatively small. In order to fix this, we changed the Scaling factor to 20:

Also, to be able to find the magnitude of the deformations, we switched the Coloring to Displacement > Magnitude:

Finally we come up with the following plot:

We can see how the piston head deforms due to the applied loads, boundary, and thermal conditions. The top face sinks down, while the ring portion bulks out. We can also see the expansion at the bottom portion, which can be important for design purposes.

Congratulations! You finished the thermomechanical analysis of an engine piston tutorial!

Last updated: February 17th, 2021