FEATool Multiphysics
v1.11 Finite Element Analysis Toolbox |

Fluid-Structure Interaction - Elastic Beam

Fluid-structure interaction benchmark problem for stationary, laminar, and incompressible flow around a cylinder with an attached elastic beam. Although it is not possible to derive an analytical solution to these test cases, numerical solutions to benchmark reference quantities have been established for the beam deformation, drag, and lift forces [1].

The test configurations consider a solid cylinder centered at (0.2, 0.2) with diameter *d = 0.1* in a *l = 2.2* by *h = 0.41* rectangular channel. The fluid is assumed to have a constant density and viscosity, and a fully developed parabolic velocity profile is prescribed at the inlet. A beam of length *0.4* and width *0.02* is fixed to the end of the cylinder. First a static solution with a Reynolds number *Re = 20* is considered, and then an instationary solution with *Re = 100*.

This model is available as an automated tutorial by selecting **Model Examples and Tutorials...** > **Multiphysics** > **Fluid-Structure Interaction - Elastic Beam** from the **File** menu. Or alternatively, follow the step-by-step instructions below.

In the

*New Model*dialog box, select**2D**for the*Space Dimensions*, and select**Fluid-Structure Interaction**from the*Select Physics*drop-down menu. Leave the space dimension and dependent variable names to their defaults and press**OK**to finish the physics mode selection.

The geometry consists of two subdomains, an outer *0.41* by *2.5* rectangle with a circular hole centered at (0.2, 0.2), and a *0.4* by *0.02* thin rectangular beam.

Start with selecting **Rectangle** from the *Geometry* menu.

- Enter
`2.5`

into the*x*edit field._{max} - Enter
`0.41`

into the*y*edit field._{max} - Press
**OK**to finish and close the dialog box. - Select
**Circle**from the*Geometry*menu. - Enter
`0.2 0.2`

into the*center*edit field. - Enter
`0.05`

into the*radius*edit field. - Press
**OK**to finish and close the dialog box. - Select
**Rectangle**from the*Geometry*menu. - Enter
`0.2`

into the*x*edit field._{min} - Enter
`0.6`

into the*x*edit field._{max} - Enter
`0.2-0.01`

into the*y*edit field._{min} - Enter
`0.2+0.01`

into the*y*edit field._{max} - Press
**OK**to finish and close the dialog box.

The circle C1 and beam R2 must be subtracted from the outer rectangle, but first make copies of them.

- Select
**C1**in the geometry object*Selection*list box. - Select
**Copy/Transform Object...**from the*Geometry*menu. - Select the
**Make copy of geometry object**check box. - Press
**OK**to finish and close the dialog box. - Select
**R2**in the geometry object*Selection*list box. - Select
**Copy/Transform Object...**from the*Geometry*menu. - Select the
**Make copy of geometry object**check box. - Press
**OK**to finish and close the dialog box.

Use the *Combine Objects...* menu option to subtract the circles both rectangles and create the two subdomains, an outer domain for the fluid and inner for the solid beam.

- Select
**Combine Objects...**from the*Geometry*menu. - Enter
`R1-C1-R2`

into the*Geometry Formula*edit field. - Press
**OK**to finish and close the dialog box. - Select
**Combine Objects...**from the*Geometry*menu. - Enter
`R3-C2`

into the*Geometry Formula*edit field. Press

**OK**to finish and close the dialog box.- Switch to
**Grid**mode by clicking on the corresponding*Mode Toolbar*button. - Press the
**Settings***Toolbar*button to open the*Grid Settings*dialog box, and use the*Boundary Grid Size*edit field prescribe a grid size of`0.025`

on the outer boundaries,`0.01`

on the circle,`0.005`

on the beam. Enter

`0.025 0.025 0.025 0.025 0.01 0.01 0.01 0.01 0.005 0.005 0.005 0.005 0.005`

into the*Boundary Grid Size*edit field.Press the

**Generate**button to call the grid generation algorithm and press**OK**to finish and close the dialog box.- Switch to
**Equation**mode by clicking on the corresponding*Mode Toolbar*button. In the

*Equation Settings*dialog box that automatically opens, select the fluid domain,**1**in the*Subdomains*list box, and set the density ρ to`1e3`

and viscosity µ to`1`

in the corresponding edit fields. The other coefficients can be left to their default values.- Select subdomain
**2**and press the**Solid**radio button to designate the beam as a structural domain (non-fluid). Set the density ρ to

`1e3`

, Poisson's ratio ν to`0.4`

, and modulus of elasticity*E*to`1.4e6`

. Then press**OK**to finish and close the dialog box.Press the

**Constants***Toolbar*button, or select the corresponding entry from the*Equation*menu, to open the*Model Constants and Expressions*dialog box. Enter a constant value of`0.2`

for the mean velocity`u_mean`

. Also enter the expression`1.5*u_mean*4/0.1608*y*(0.41-y)*(0.5*(1-cos(pi/2*t))*(t<2)+(t>=2))`

for the inlet velocity`u_in`

. This expression defines a parabolic inlet profile*1.5*u_mean*4/0.1608*y*(0.41-y)*which is successively applied between*t = 0-2*by using the scaling factor*(0.5*(1-cos(pi/2*t))*(t<2)+(t>=2))*.- Switch to
**Boundary**mode by clicking on the corresponding*Mode Toolbar*button. First select the left inflow boundary (number

**4**) and choose the**Inlet/velocity**boundary condition from the drop-down menu. Enter`u_inlet`

in the edit field for the velocity coefficient in the*x-direction*to use the pre-defined expression for the inlet velocity.Select the right outflow boundary (number

**2**) and select the**Neutral outflow/stress boundary**boundary condition from the drop-down menu.- Select the
**Interior Boundaries**check box to enable boundary conditions for internal and interior boundaries. Select the

*Fluid-Structure interface*condition for the boundaries shared between the fluid and solid (**11**,**12**, and**13**).Finally, select the

*Prescribed displacement*boundary condition with zero displacement to fix the right edge of the beam (boundaries**9**and**10**). Then press**OK**to finish the boundary condition specification- Now that the problem is fully specified, press the
**Solve***Mode Toolbar*button to switch to solve mode, and press the**FSI Solver**button to open the solver settings dialog box. Set the

*time step*to`0.2`

and*final time*to`10`

which should give enough time to develop a steady solution. Then press**Solve**to start the solution process.Press the

**Solve**button.

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

To calculate the drag and lift forces, first select

**Boundary Integration...**from the*Post*menu. In the*Boundary Integration*dialog box, select the boundaries which make up the circle and beam in the left hand side*Boundaries*selection list box (numbers**5-8**and**11-13**). Then select the corresponding**Total force, x-component**from the pre-defined integration expressions. Press the**OK**or the*Apply*button to show the result in the lower*Integration Result*frame as well as in the*Command Log*message window.

The computed drag force is about *14.4483* which is close to the reference value of *14.29426*. Now repair the process for the force in the y-direction.

Similarly, the computed lift force is about *0.81534* in the y-direction which should be compared to the reference value of *0.763746*. To get a closer result one could use a finer grid along the cylinder and beam boundaries, as well as higher order elements which yield higher accuracy for quantities involving derivatives (as the force terms here do)

To set an instationary test case, go back and increase the density of the beam to *1e4* and change the mean inlet velocity to *1*. Also decrease the time step of the solver to *0.01* and the final time to *15*. Note that, depending on your system configuration, the instationary simulation may take a long time to finish.

The *fluid-structure interaction - elastic beam* 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.

[1] Hron J. *A monolithic FEM/multigrid solver for ALE formulation of fluid structure interaction with application in biomechanics*. In H.-J. Bungartz and M. Schaefer, editors, Fluid-Structure Interaction: Modelling, Simulation, Optimisation, LLNCSE. Springer, 2006.