FEATool Multiphysics  v1.14
Finite Element Analysis Toolbox
Multi-Simulation Heat Exchanger

This model simulates how the flow of cool airflow is heated while moving through a tube-fin heat exchanger. Due to several symmetry planes only a small section of the heat exchanger geometry actually needs to be simulated, as illustrated in the following image.

multi_simulation1_00_50.jpg

The model illustrates the multi-solver simulation process by first solving for the flow field using the OpenFOAM CFD solver. After which the temperature field is solved for with the built-in FEATool Multiphysics solver, using the pre-computed flow field as a constant input to the heat equation. (Make sure the OpenFOAM solver is installed before running the model.)

This two step solution process for a one-way coupled model allows significant savings in computational time and resources, by separating the equations and physics problems, and use the best and most efficient solver for each individual sub-problem.

multi_simulation1_01_50.jpg

Tutorial

This model is available as an automated tutorial by selecting Model Examples and Tutorials... > Multiphysics > Multi-Simulation Heat Exchanger from the File menu. Or alternatively, follow the step-by-step instructions below.

  1. To start a new model click the New Model toolbar button, or select New Model... from the File menu.
  2. Select the 3D radio button.
  3. Select the Navier-Stokes Equations physics mode from the Select Physics drop-down menu.
  4. Press OK to finish the physics mode selection.

    multi_simulation1_04_50.png

By utilizing the symmetry in the y and z directions the computational domain of the airflow can be reduced significantly to a slice between two fins and one tube. This geometry can be constructed by subtracting the fins and a cylinder from a block.

First create the main block for the domain interior.

  1. Press the Create cube/block Toolbar button.
  2. Enter 20 into the xmax edit field.
  3. Enter 5 into the ymax edit field.
  4. Press OK to finish and close the dialog box.

Then create a cylinder and subtract it from the block.

  1. Press the Create cylinder/cone Toolbar button.
  2. Enter 2.5 into the radius1 edit field.
  3. Enter 2.5 into the radius2 edit field.
  4. Enter 10 0 0 into the center edit field.
  5. Enter 0 0 1 into the axis edit field.
  6. Press OK to finish and close the dialog box.
  7. Select B1 and C1 in the geometry object Selection list box.
  8. Press the - / Subtract geometry objects Toolbar button.

Create the lower fin, and then make a copy with a z-translation to move it to the upper side.

  1. Press the Create cube/block Toolbar button.
  2. Enter 5 into the xmin edit field.
  3. Enter 15 into the xmax edit field.
  4. Enter 5 into the ymax edit field.
  5. Enter 0.0625 into the zmax edit field.
  6. Press OK to finish and close the dialog box.
  7. Select B2 in the geometry object Selection list box.
  8. Press the Copy/transform selected geometry object Toolbar button.
  9. Enter 1 into the Number of copies to make edit field.
  10. Enter 0 0 1-0.0625 into the Displacement vector (x, y, and z-components) edit field.
  11. Press OK to finish and close the dialog box.

Finally remove the two fins using the geometry formula CS1 - B2 - TF1.

  1. Select Combine Objects... from the Geometry menu.
  2. Enter CS1-B2-TF1 into the Geometry Formula edit field.
  3. Press OK to finish and close the dialog box. The completed geometry should then look like the following.

    multi_simulation1_30_50.png
  4. Switch to Grid mode by clicking on the corresponding Mode Toolbar button.

Create a grid with the maximum target mesh size set to 0.2. Although this is a rather coarse mesh, it saves computational time and is good enough for demonstration purposes and an initial study.

  1. Enter 0.2 into the Grid Size edit field.
  2. Press the Generate button to call the grid generation algorithm.

    multi_simulation1_33_50.png
  3. Switch to Equation mode by clicking on the corresponding Mode Toolbar button.

Enter a non-dimensionalized unit density of 1 and viscosity of 0.00526. This is equivalent to a Reynolds number of 190.

  1. Enter 1 into the Density edit field.
  2. Enter 0.00526 into the Viscosity edit field.

    multi_simulation1_36_50.png
  3. Press OK to finish the equation and subdomain settings specification.
  4. Switch to Boundary mode by clicking on the corresponding Mode Toolbar button.

First set the velocity in the x-direction to 1.

  1. Select 5 in the Boundaries list box.
  2. Select Inlet/velocity from the Navier-Stokes Equations drop-down menu.
  3. Enter 1 into the Velocity in x-direction edit field.

Then select the Outflow/pressure condition for the outlet boundary.

  1. Select 11 in the Boundaries list box.
  2. Select Outflow/pressure from the Navier-Stokes Equations drop-down menu.
  3. Select 3, 7-10, 13, 14, and 16 in the Boundaries list box.

    multi_simulation1_44_50.png
  4. Select the Wall/no-slip condition from the Navier-Stokes Equations drop-down menu for the boundaries representing the fins and the cylinder.

Finally, select the Symmetry/slip condition for the rest of the boundaries.

  1. Select 1, 2, 4, 6, 12, 15, and 17 in the Boundaries list box.
  2. Select Symmetry/slip from the Navier-Stokes Equations drop-down menu.

    multi_simulation1_47_50.png
  3. Press OK to finish the boundary condition specification.
  4. Switch to Solve mode by clicking on the corresponding Mode Toolbar button.

The OpenFOAM CFD solver will first be used to solve for the flow field. Open the OpenFOAM solver settings dialog box and reduce the tolerance for convergence to 1e-4.

  1. Press the OpenFOAM Toolbar button.
  2. Enter 1e-4 into the Stopping criteria/tolerance for initial residuals edit field.

    multi_simulation1_51_50.png
  3. Press the Solve button to start the OpenFOAM solver. The view will switch to show the convergence process for the solution variables.

    multi_simulation1_52_50.png

After the problem has been solved FEATool will automatically switch to postprocessing mode and display the resulting velocity field.

Open the Postprocessing settings dialog box and change from surface to slice plot to help see the interior of the flow field.

  1. Press the Plot Options Toolbar button.
  2. Clear the Enable/disable surface plot check box.
  3. Select the Enable/disable slice plot check box.
  4. Press OK to plot and visualize the selected postprocessing options.

    multi_simulation1_56_50.png

One can now clearly see how there is a large wake behind the cylinder, and how the fins create a very thin low velocity boundary layer.

To couple and study the temperature field, switch back to Equation mode to add a Heat Transfer physics mode to the model.

  1. Switch to Equation mode by clicking on the corresponding Mode Toolbar button.
  2. First deactivate the equation for the flow field by de-selecting the active button. This means that the flow variables will not be solved for and held constant, which saves computational effort. (Note that this decoupling is only possible for one-way coupled multiphysics problems. If the flow field and properties also depend on the temperature, both physics modes must be solved fully coupled together.)

    multi_simulation1_58_50.png
  3. Next switch to the + tab and add the Heat Transfer physics mode.
  4. Select the Heat Transfer physics mode from the Select Physics drop-down menu.
  5. Press the Add Physics >>> button.

Set the non-dimensionalized thermal conductivity to 3.76e-3, while leaving the density and heat capacity at their default unit values. This is equivalent to a Prandtl and Peclet numbers of 266.

  1. Enter 3.76e-3 into the Thermal conductivity edit field.

To couple the flow field to the convective terms for the temperature, enter the dependent variable names u, v, and w in the corresponding edit fields.

  1. Enter u into the Convection velocity in x-direction edit field.
  2. Enter v into the Convection velocity in y-direction edit field.
  3. Enter w into the Convection velocity in z-direction edit field.

    multi_simulation1_65_50.png

As this is a convective flow dominated model some degree of artificial and numerical stabilization is appropriate to add in order to ease convergence and smooth out oscillations.

  1. Press the Artificial Stabilization button.
  2. Select the Check to enable streamline diffusion check box.
  3. Enter 1 into the Streamline diffusion tuning parameter edit field.

    multi_simulation1_68_50.png
  4. Press OK to finish and close the dialog box.
  5. Press OK to finish the equation and subdomain settings specification.
  6. Switch to Boundary mode by clicking on the corresponding Mode Toolbar button.

For the temperature boundary conditions set the inlet temperature to 0 and the surfaces of the surrounding fins and cylinder to 1.

  1. Switch to the ht tab.
  2. Select 5 in the Boundaries list box.
  3. Select Temperature from the Heat Transfer drop-down menu.
  4. Enter 0 into the Temperature edit field.
  5. Select 3, 7-10, 13, 14, and 16 in the Boundaries list box.
  6. Select Temperature from the Heat Transfer drop-down menu.
  7. Enter 1 into the Temperature edit field.
  8. Select 11 in the Boundaries list box.

For the outflow boundary select Convective flux/outflow.

  1. Select Convective flux/outflow from the Heat Transfer drop-down menu.
  2. Select 1, 2, 4, 6, 12, 15, and 17 in the Boundaries list box.

    multi_simulation1_81_50.png

And finally select Thermal insulation/symmetry for the symmetry boundaries..

  1. Select Thermal insulation/symmetry from the Heat Transfer drop-down menu.

    multi_simulation1_82_50.png
  2. Press OK to finish the boundary condition specification.
  3. Switch to Solve mode by clicking on the corresponding Mode Toolbar button.

Press the Restart button to solve the problem for the temperature field with the existing flow field constant (as the fluid flow physics mode was deactivated earlier). (Do not use the usual = solve button, as this would clear the already computed flow field and instead re-compute the initial conditions as initial guess.)

  1. Press the Restart/Solve with last computed solution as initial condition Toolbar button to start the solution process for the temperature.

After the solution process is done the temperature field can now be plotted and visualized.

  1. Press the Plot Options Toolbar button.
  2. Select Temperature, T from the Predefined slice plot expressions drop-down menu.
  3. Press OK to plot and visualize the selected postprocessing options.

    multi_simulation1_88_50.png

One can clearly see how the fluid is heated by both the cylinder and walls, and transported straight away in the direction of the flow.

The multi-simulation heat exchanger multiphysics model has now been completed and can be saved as a binary (.fea) model file, or exported as a programmable MATLAB m-script text file, or GUI script (.fes) file.