Tutorial: Conjugate Heat Transfer in a U-Tube Heat Exchanger

This tutorial shows how a conjugate heat transfer simulation in a U-tube heat exchanger can be done.

This kind of heat exchanger is named after the U-shaped tube and is a simple, low price structure with less sealing surface. It has a tube configuration that can expand or contract freely, without producing thermal stress due to the temperature difference between the tube and shell, leading to a good thermal compensation performance. SimScale can simulate and visualize this thermal conduction between the solid shell and the two streams that flow within.

Overview

This tutorial teaches users how to:

• Set up and run a conjugate heat transfer simulation.
• Assign initial and boundary conditions, material assignments, and other properties to the simulation.
• Mesh with the SimScale standard meshing algorithm.
• Post-process the results in SimScale.

We are following the typical SimScale workflow:

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.

1. Prepare the CAD Model and Select the Analysis Type

1.1. Import the CAD into Your Workbench

First of all, click the button below. This action will copy the tutorial project containing the geometry into your Workbench.

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

1.2. CAD Mode

Before we start setting up the simulation we need to do some CAD pre-processing. As we simulate a conjugate heat transfer, we want to know the heat transfer between solids and fluids. Natively we already have the solid shell CAD part, now we need to create the flow regions.
The following picture illustrates the parts we need for setting up the simulation:

Finally, we need to run an Imprint operation to enhance the automatic contact detection. All of these steps are possible within SimScale’s CAD Mode:

a. Open Inner Region for Modelling the Inner Region

In CAD Mode, the first step is the creation of an Internal Flow Volume operation. In this step, we will assign a Seed face, as well as the boundary faces of the flow region.

1. Create an ‘Internal Flow Volume’ operation
2. Define a Seed face, which is a face that will be in contact with the flow region. In figure 5, the seed face is highlighted in blue
3. Select the Boundary faces, where the openings are. In this case, we have two boundary faces, highlighted in white in figure 5
4. Hit ‘Apply’

At this point, the tube side flow region will be created. Using the same logic, we have to create one more flow region, using another internal flow volume operation:

In the image above, please note that you will need to rotate the model around to select the second boundary face.

Now we have both fluid regions ready. Only the Imprint operation is missing before the model is ready to simulate:

1. Select an ‘Imprint’ operation
2. Click ‘Apply’
3. Hit ‘Finish’ to export the finalized model into your Workbench

1.3. Create the Simulation

When a model the exported from CAD Mode, it will be named Copy of Heat_Exchanger. This is the model that we will use to run the simulation. Before ‘Creating a Simulation’, you can also rename the CAD model appropriately, and save the changes by clicking on the check icon.

At this point, the analysis type widget opens in the viewer:

Choose the ‘Conjugate Heat Transfer‘, then click on the ‘Create Simulation‘ option to get started. If you want to learn more about this analysis type, click here.

2. Setting Up the Simulation

Now you can define the global settings of your simulation. The following setup should pop up automatically, if not you get there by clicking on the name of the simulation:

Here, you can define global settings for your simulation. In this case, the flow is turbulent, so the ‘k-omega SST’ turbulence model is chosen.

2.1. Assign the Model

Click on ‘Model‘ in the simulation tree to define the gravity force acting on the domain according to the coordinate system of the CAD. In this case, gravity is defined in the negative y-direction:

2.2. Assign the Materials

In this simulation, we want to analyze the heat transfer between a fluid through a solid into another fluid. Therefore, we need to assign properties to the two-fluid regions and the solid shell.

a. Fluids

To apply a new material, click on the ‘+’ icon next to the Fluids under the Materials tab. For this project, the two flow regions consist of ‘Water‘, so choose it from the option that is listed on the panel that appears:

After you click ‘Apply‘, assign the material to the flow regions by picking them on the geometry tree at the top right of the screen.

Solids

Click on the ‘+’ icon next to the Solids under the Materials tab. The material chosen for the shell is ‘Steel‘.

The same procedure is followed to assign it to the respective part:

2.3. Assign the Initial Conditions

Now we initialize the temperatures for the simulation. This helps to make the simulation more stable. To add an initial value, click on the ‘+’ next to the Subdomains:

In this case, we know the inlet temperatures of the fluids, so we define the global fluid temperatures to the inlet temperatures for the first calculation step.

• Start by clicking the ‘+’ icon next to the Subdomains tab.
• Name your subdomain as the ‘Outer flow region‘ to avoid confusion with the other flow region.
• Change the subdomain value to ‘100’ °C.
• Assign this to the Outer flow region by picking it from the Geometry tree at the top right of the screen, as you can see below.
• Click on the checkmark when you are finished.

Repeat these steps for the inner flow region (tube side). However, this time, set the initial condition to ’80’ °C.

Finally, set the initial temperature of the Shell to ’15’ °C.

2.4. Assign the Boundary Conditions

To assign boundary conditions on the heat exchanger, click on the ‘+‘ icon next to the Boundary conditions, and click on the types described in this section.

Inner Flow Region (Low-Temperature Fluid Region)

Initially, apply the inlet velocity of the cold stream, by clicking on the ‘Velocity Inlet‘ option at the drop-down menu that appears as seen in Figure 19, and set the velocity in the x-direction to –0.8 m/s. Add a temperature of 80°C.

A Pressure Outlet condition with the value of the atmospheric pressure (101325 Pa) is then applied to the outlet face of the inner flow region:

Outer Flow Region (High-Temperature Fluid Region)

Apply the same procedure for the hot stream, aka the outer flow region as well, starting with a Velocity Inlet of -0.5 m/s and a temperature of 100°C.

Finally, set the Pressure Outlet condition for the outlet with a value of 101325 Pa:

2.5. Simulation Control & Numerics

Fill in the Simulation Control settings as following:

Leave the numerics panel at its default state.

2.6. Mesh

Click on ‘Mesh‘ to access the global mesh settings, shown in the following picture. Choose the ‘Standard‘ algorithm, and set the Fineness to Level 5.5:

If you are interested to see how to use the standard meshing tool, take a look at this tutorial.

3. Run the Simulation

After all the settings are completed, proceed by clicking the ‘+‘ icon next to the Simulation Runs, so you start with the analysis. The mesh will be generated automatically before the run.

While the results are being calculated, you can already have a look at the intermediate results in the post-processor. They are being updated in real-time!

4. Post-Processing

When the simulation is complete, you can check the Convergence and the Results of the simulation. You can access either of them in the Simulation tree by clicking on them, as you can see below:

The convergence plot indicates whether or not the solution is reliable, or whether some changes should be made in the settings, such as making the mesh finer or increasing the simulation time. In the following picture, you can see how the residuals of your simulations will appear in the plot:

To view the results of your heat exchanger simulation, click on the ‘Solution Fields‘ tab under your finished run. This will redirect you to the post-processor.

Create a new cutting plane to view the temperature distribution across the center plane:

• Click on the ‘+’ icon next to the ‘Cutting Planes.
• Choose the ‘Z‘ axis. It will automatically generate a plane normal to this axis, coincident with the origin of the model.
• Choose the ‘Temperature‘ as the Scalar parameter.

Apply the continuous legend to add smoothing to the results:

• Go to the Results and click on the ‘Temperature‘.
• Apply the ‘Continuous Legend‘ feature by checking the empty square next to it.
• Repeat the above instruction for the ‘Node averaged values‘.

If you wish to see the temperature distribution on a whole part of your heat exchanger:

• Hide all the parts except for the chosen one.
• Go to the Results and apply the ‘Temperature‘ by clicking the icon next to it.
• Add the ‘Continuous Legend‘ and ‘Node averaged values‘ like before.

For more information, have a look at our post-processing guide to learn how to use the post-processor.
Congratulations! You finished the tutorial!

References

• http://www.ansonindustry.com/pressure-vessel/u-tube-heat-exchanger.html

Last updated: April 13th, 2021

What's Next

Thermal Management of an Electronics Box using CHT Analysis