Fill out the form to download

Required field
Required field
Not a valid email address
Required field

Documentation

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 performed using SimScale’s CHT v2 solver.

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.

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.

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

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

Finally, you 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, you 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, you 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, you 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 you 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:

create simulation in simscale
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, you want to analyze the heat transfer between a fluid through a solid into another fluid. Therefore, you 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 inner flow region by picking it on the geometry tree at the top right of the screen.

assigning the coolant as water
Figure 13: Properties of water for the flow regions material assignment

Now you will assign ‘Air’ as material of the hot flow region:

fluid material list air
Figure 14: The hot fluid will be modelled as gas.

Pick the flow region that corresponds to the outer fluid part:

flow region that corresponds to outer fluid simscale simulation tutorial
Figure 15: As both of the fluid parts are modelled as ‘Flow regions’

Solids

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 16: 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 17: 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 you 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 18: Adding subdomains

In this case, you know the inlet temperatures of the fluids, so you 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 ‘Hot Gas’ 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.
high temperature flow region initial condition subdomain
Figure 19: Initial temperature of the outer flow region

Repeat these steps for the coolant (tube side). However, this time, set the initial condition to ’10’ \(°C\).

low temperature flow region initial condition subdomain
Figure 20: Initial temperature of the inner flow region

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

shell initial condition subdomain
Figure 21: 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 22: 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 22, and set the velocity in the x-direction to ‘0.01’ \(kg \over \s\) . Add a temperature of ’10’ \(°C\).

velocity inlet low temperature flow region for heat exchanger simulation
Figure 23: Velocity for the inlet of the inner flow region

A Pressure Outlet condition with the mean 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 24: 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 Flow rate of ‘0.02’ \( kg/ over /s\) and a temperature of ‘100’ \(°C\).

velocity inlet high temperature flow region flow rate
Figure 25: Velocity for the inlet of the outer flow region

Finally, set the Pressure Outlet condition for the outlet with a mean value of ‘101325’ \(Pa\):

pressure outlet atmospheric pressure high temperature outer flow
Figure 26: 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 27: Simulation control panel

Leave the Numerics panel at its default state, except from the Absolute tolerance of the (ω) Specific dissipation rate. Set this to ‘1e-9’:

Numerics panel absolute tolerance
Figure 28: The solver reaches the default value for the dissipation’s rate absolute tolerance prior to the finish of the run.

3. 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 ‘6’:

mesh panel standard mesher
Figure 29: 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.

4. Start 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 30: 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!

5. 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 31: Results of the simulation

5.1. Convergence Plot

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 32: Convergence plot of the simulation. Oscillations around small values can be ignored.

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.

5.2 Surface Visualization

You can check the distribution of a parameter across a whole part. For example. if you wish to view the temperature values of the hot gas, do the following:

  • Hide the flow region that corresponds to the coolant, as well as the shell using the tree at the top right;
  • Set the Coloring input to ‘Temperature’;
  • Change the unit to ‘\(°C\)’;
  • Right-click on the legend at the bottom and choose the ‘Use continuous legend’ option.
hot gas temperature distribution from surface visualization feature
Figure 33: The visualization of each parameter can be applied to every part of the model separately, or combined.

The drop of the high-temperature inlet to the low-temperature outlet can be seen due to the transition of warm colors at the bottom to cold shades at the upper side of the fluid domain.

continuous legend provides smooth visualization of temperature on fluid region
Figure 34: This is how the surface visualization will appear after the continuous legend filter is added.

5.2. Cutting Planes

Create a new cutting plane to view the temperature distribution across the center plane. To add this feature:

  • Click on the ‘Add filter’ option;
  • Select the ‘Cutting Plane’ from the drop down menu that will appear.
adding a new feature in the post processor interface
Figure 35: When adding a new filter, all the available options will appear in a drop down menu.
  • Choose the ‘Z’ axis. It will automatically generate a plane normal to this axis, coincident with the origin of the model;
  • Choose ‘Temperature’ as the Coloring option.
cutting plane showing temperature distribution
Figure 36: Cutting plane with the temperature distribution

Now the contribution of the coolant in the temperature drop of the hot gas can also be visualized. The areas that are close to the hot gas inlet appear warmer than the upper part which is located near the cooler side. Also, the left part of the cutting plane, which is the farthest away from the coolant, has some warm-colored contours as well.

Apart from the internal temperature, the velocity magnitude can be really insightful too, especially when the vectors are visualized:

  • Change the Coloring to ‘Velocity Magnitude’;
  • Activate the ‘Vectors’;
  • Change the Scale factor to ‘0.08’ and the Grid Spacing to ‘0.01’;
  • Finally, activate the ‘Project vectors onto plane’.
velocity vectors shown in simscale post processing analysis
Figure 37: The longer the arrows that represent the vectors, the higher the velocity in that area. This can be observed mostly near the inlets and outlets, as well as inside the tubes.

5.3. Streamlines

Create a Particle Trace set, and select the face of the inlet’s coolant as the seed face in order to generate the visualization of flow as streamlines:

pick position for streamline generation of the coolant in heat exchanger
Figure 38: The streamlines enter the heat exchanger from the inlet, flow through the pipes, and exit from the model from the bottom after cooling down the hot gas.
  • Set the number of streamlines that are going to be generated horizontally to ’20’;
  • Repeat for the number of streamlines that are going to be generated vertically, but this time set it to ’30’;
  • Add a Spacing input of ‘3e-3’;
  • Switch the Coloring to ‘Temperature’;
  • Set the Size to ‘5e-4’. This is the diameter of the streamlines’ circular cross-section;
  • For this case, the Trace both directions option can be deactivated.
streamlines of the coolant in a heat exchanger
Figure 39: The beginning of the streamlines is far from the hot gas’s inlet, so the temperature is the lowest there.

This can be repeated for the hot gas too. Create a new ‘Particle Trace’ set. Select the face of the inlet as the seed face too:

pick position for streamline generation of the hit gas in heat exchanger
Figure 40: The seed face coincides with the inlet of the fluid medium here too.

Then apply the following:

  • Set the # Seeds horizontally and # Seeds vertically to ’20’;
  • Add a Spacing input of ‘3e-3’;
  • Switch the Coloring to ‘Temperature’;
  • Set the Size to ‘3e-4’;
  • Deactivate the Trace both directions option.
streamlines of the hot gas in a heat exchanger
Figure 41: The streamlines of the hot gas cover the whole volume inside between the cells and coolant’s tube.

Finally, keep in mind that if you wish to visualize the streamlines and the shell at the same time, so you produce an image as you can see in Figure 1, then you can go ahead and reduce the opacity of the latter, after setting the Coloring to ‘Solid Color’:

reducing the opacity so all sets are visible
Figure 42: After the two fluid regions are hidden using the tree at the top right of the interface, the visibility of the shell can be reduced so both streamlines sets are visualized too.

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

Note

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

Last updated: June 14th, 2021

What's Next

Contents
Data Privacy