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.
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.
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:
Prepare the CAD model for the simulation.
Set up the simulation.
Create the mesh.
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 own workbench.
The following picture demonstrates what should be visible after importing the tutorial project.
Figure 2: Imported CAD model of the heat exchanger in the SimScale workbench
1.2. Use Geometry Operations on the CAD
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:
Figure 3: CAD components necessary for the simulation
Finally, we need to tell the program where the interfaces between those parts are. In order to do this, we need to create an imprint.
a. Open Inner Region for Modelling the Inner Region
Figure 4: Adding a new geometry operation for an open inner region creation
The first step for this simulation is the creation of two ‘Open Inner Region‘ features. For the first one, click on the ‘Add geometry operation‘ option, then select the ‘Open Inner region’:
Figure 5: Assigning the boundary and seed faces of the first open inner region
Make sure to toggle on ‘Keep existing parts‘. Otherwise, the housing of the heat exchanger will be gone. Always keep that on for CHT simulations.
Now select the faces at the border for the low-temperature fluid (displayed in blue),
and a seed face (displayed in pink) which can be any face later touching the fluid region.
Pressing ‘Start‘ will create the first flow volume.
b. Open Inner Region for Modelling the Outer Region
Now do the same for the other fluid, but this time select the following faces:
Figure 6: Assigning the boundary and seed faces of the second open inner region
c. Imprint
The last step of the CAD preparation is the use of the ‘Imprint‘ feature on the whole heat exchanger CAD model:
Figure 7: Imprinting the model
This will help the recognition of interfaces. The interfaces will later be assigned as contacts. On the panel that will appear, just click ‘Start‘ and wait until the final version of the CAD model is generated.
We have some knowledge base articles which can help understanding the CAD requirements for CHT simulations:
After the fluid regions are created and the imprint is ready, click on the original geometry, then a panel opens where you have the option to click ‘Create Simulation‘.
Figure 8: Create a simulation
Doing so opens the SimScale Simulation Library:
Figure 9: Choosing the conjugate heat transfer analysis
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:
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:
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
In order 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:
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.
Figure 13: Properties of water for the flow regions material assignment
Solids
Click on the ‘+’ icon next to the Solids’ under the Materials tab. The material chosen for the shell is ‘Steel‘.
Figure 14: Solids material list for the conjugate heat transfer analysis
The same procedure is followed in order to assign it to the respective part:
Figure 15: Properties of steel for the solid region material assignment
2.3. Assign the Initial Conditions
Now we initialize the temperatures for the simulation. This helps to make the simulation more stable. In order to add an initial value, click on the ‘+’ next to the Subdomains:
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.
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 this for the inner flow region (Tube region). Set the initial condition to 80 °C.
Figure 18: Initial temperature of the inner flow region
Finally, set the initial temperature to 15 °C for the shell.
Figure 19: Initial temperature of the shell
2.4. Assign the Boundary Conditions
In order 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.
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.
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:
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.
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:
Figure 24: Pressure assignment for the outlet of the outer flow region
2.5. Simulation Control & Numerics
Fill in the SimulationControl settings as following:
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:
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.
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:
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:
Figure 29: Convergence plot of the simulation
In order 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.
Figure 30: Cutting plane with 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‘.
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.
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!
This website uses cookies so that we can provide you with the best user experience possible. Cookie information is stored in your browser and performs functions such as recognising you when you return to our website and helping our team to understand which sections of the website you find most interesting and useful.
Strictly Necessary Cookies
Strictly Necessary Cookie should be enabled at all times so that we can save your preferences for cookie settings.
If you disable this cookie, we will not be able to save your preferences. This means that every time you visit this website you will need to enable or disable cookies again.
