Fill out the form to download

Required field
Required field
Not a valid email address
Required field


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.

streamlines in a utype heat exchanger simulation
Figure 1: Visualization of the temperature distribution on the streams in the heat exchanger

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.


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.

heat exchanger CAD import workbench
Figure 2: Imported CAD model of the heat exchanger in the SimScale workbench

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:

cad parts for cht simulation of heat exchanger
Figure 3: CAD components necessary for 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:

entering cad mode environment simscale heat exchanger
Figure 4: To enter the CAD Mode environment, simply click on the highlighted icon.

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.

flow volume creation cht simulation cad mode
Figure 5: After clicking on Apply, the tube side flow region will be created.
  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:

flow volume creation shell side heat exchanger cad mode
Figure 6: In the image, the seed face is highlighted in blue, whereas the boundary faces are highlighted in white.

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:

imprint operation cht cad mode
Figure 7: The imprint operation enhances the automatic contact detection. In CHT analysis, it’s always run after the flow volume creation.
  1. Select an ‘Imprint’ operation
  2. Click ‘Apply’
  3. Hit ‘Finish’ to export the finalized model into your Workbench

We have some knowledge base articles which can help to understand the CAD requirements for CHT simulations:

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.

create simulation button heat exchanger
Figure 8: After saving the name change, you can create a new simulation

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

analysis type conjugate heat transfer
Figure 9: SimScale has a wide range of analysis types available, covering CFD and FEA.

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:

turbulence model k-omega sst steady state conjugate heat transfer
Figure 10: Choosing the k-omega SST turbulence model for the compressible CFD analysis

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:

gravity direction assignment model
Figure 11: The gravity that is applied to the simulation

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:

fluid material list water
Figure 12: Fluids material list for the conjugate heat transfer analysis

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.

water properties flow regions
Figure 13: Properties of water for the flow regions material assignment


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

solid material list steel
Figure 14: Solids material list for a conjugate heat transfer analysis

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

steel properties shell
Figure 15: Properties of steel for the solid region material assignment

Did you know?

If you have a custom material that is not available in the materials list, you can easily define it in SimScale. This article shows the necessary steps.

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:

subdomain initial temperature value
Figure 16: Adding 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.

high temperature flow region initial condition subdomain
Figure 17: Initial temperature of the outer flow region
  • 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.

low temperature flow region initial condition subdomain
Figure 18: Initial temperature of the inner flow region

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

shell initial condition subdomain
Figure 19: Initial temperature of the shell volume

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.

add boundary conditions simulation tree
Figure 20: Boundary conditions

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.

velocity inlet low temperature flow region for heat exchanger simulation
Figure 21: Velocity for the inlet of the inner flow region

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:

pressure outlet atmospheric pressure inlet low temperature flow region heat exchanger CAD
Figure 22: Pressure assignment for the outlet 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.

velocity inlet high temperature flow region
Figure 23: Velocity for the inlet of the outer flow region

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

pressure outlet atmospheric pressure high temperature outer flow
Figure 24: Pressure assignment for the outlet of the outer flow region

2.5. Simulation Control & Numerics

Fill in the Simulation Control settings as following:

simulation properties run time
Figure 25: Simulation control panel

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:

mesh panel standard mesher
Figure 26: Mesh panel for the Standard mesher with automatic sizing

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.

create a new simulation run icon
Figure 27: Create a new simulation 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:

solution fields convergence plot results simulation run
Figure 28: Results of the simulation

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:

convergence plot
Figure 29: Convergence plot of the simulation

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.
post processor cutting plane results temperature distribution
Figure 30: Cutting plane with the temperature distribution

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‘.
continuous legend temperature distribution heat exchanger cutting plane
Figure 31: Applying the continuous legend feature on the temperature results

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.
temperature distribution inner stream heat exchanger
Figure 32: Visualizing the temperature distribution on the inner flow region (low-temperature region)

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


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


Last updated: April 13th, 2021

What's Next

Data Privacy