FEATool Multiphysics
v1.14
Finite Element Analysis Toolbox

This model simulates how the flow of cool airflow is heated while moving through a tubefin 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.
The model illustrates the multisolver simulation process by first solving for the flow field using the OpenFOAM CFD solver. After which the temperature field is solved for with the builtin FEATool Multiphysics solver, using the precomputed 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 oneway 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 subproblem.
This model is available as an automated tutorial by selecting Model Examples and Tutorials... > Multiphysics > MultiSimulation Heat Exchanger from the File menu. Or alternatively, follow the stepbystep instructions below.
Press OK to finish the physics mode selection.
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.
20
into the x_{max} edit field.5
into the y_{max} edit field.Then create a cylinder and subtract it from the block.
2.5
into the radius_{1} edit field.2.5
into the radius_{2} edit field.10 0 0
into the center edit field.0 0 1
into the axis edit field.Create the lower fin, and then make a copy with a ztranslation to move it to the upper side.
5
into the x_{min} edit field.15
into the x_{max} edit field.5
into the y_{max} edit field.0.0625
into the z_{max} edit field.1
into the Number of copies to make edit field.0 0 10.0625
into the Displacement vector (x, y, and zcomponents) edit field.Finally remove the two fins using the geometry formula CS1  B2  TF1
.
CS1B2TF1
into the Geometry Formula edit field.Press OK to finish and close the dialog box. The completed geometry should then look like the following.
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.
0.2
into the Grid Size edit field.Press the Generate button to call the grid generation algorithm.
Enter a nondimensionalized unit density of 1
and viscosity of 0.00526
. This is equivalent to a Reynolds number of 190.
1
into the Density edit field.Enter 0.00526
into the Viscosity edit field.
First set the velocity in the xdirection to 1
.
1
into the Velocity in xdirection edit field.Then select the Outflow/pressure condition for the outlet boundary.
Select 3, 710, 13, 14, and 16 in the Boundaries list box.
Finally, select the Symmetry/slip condition for the rest of the boundaries.
Select Symmetry/slip from the NavierStokes Equations dropdown menu.
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 1e4
.
Enter 1e4
into the Stopping criteria/tolerance for initial residuals edit field.
Press the Solve button to start the OpenFOAM solver. The view will switch to show the convergence process for the solution variables.
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.
Press OK to plot and visualize the selected postprocessing options.
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.
First deactivate the equation for the flow field by deselecting 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 oneway coupled multiphysics problems. If the flow field and properties also depend on the temperature, both physics modes must be solved fully coupled together.)
Set the nondimensionalized thermal conductivity to 3.76e3
, while leaving the density and heat capacity at their default unit values. This is equivalent to a Prandtl and Peclet numbers of 266.
3.76e3
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.
u
into the Convection velocity in xdirection edit field.v
into the Convection velocity in ydirection edit field.Enter w
into the Convection velocity in zdirection edit field.
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.
Enter 1
into the Streamline diffusion tuning parameter edit field.
For the temperature boundary conditions set the inlet temperature to 0
and the surfaces of the surrounding fins and cylinder to 1
.
0
into the Temperature edit field.1
into the Temperature edit field.For the outflow boundary select Convective flux/outflow.
Select 1, 2, 4, 6, 12, 15, and 17 in the Boundaries list box.
And finally select Thermal insulation/symmetry for the symmetry boundaries..
Select Thermal insulation/symmetry from the Heat Transfer dropdown menu.
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 recompute the initial conditions as initial guess.)
After the solution process is done the temperature field can now be plotted and visualized.
Press OK to plot and visualize the selected postprocessing options.
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 multisimulation heat exchanger multiphysics model has now been completed and can be saved as a binary (.fea) model file, or exported as a programmable MATLAB mscript text file, or GUI script (.fes) file.