E.6 Creating the fluid model for the fluid-structure interaction analysis

You will now create models to perform the fluid-structure interaction analysis of fluid flow inside a deformable tube. Two models must be created: one for the fluid flow and another for the structural response of the tube. You will first create the fluid model that is used in the fluid-structure interaction analysis.

E.6.1 Defining the fluid model

In this section you copy the previously created fluid model to a new model that will be used in the fluid-structure interaction analysis.

To create the fluid model:

In the Model Tree, click mouse button 3 on the model named fluid-cfd.
From the menu that appears, select Copy Model.
Name the new model fluid, and click OK.

Abaqus/CAE creates the fluid model. Make all subsequent changes to this model.

E.6.2 Modifying the analysis step and output requests

You will now modify the total analysis time for the fluid-structure interaction analysis.

To modify the analysis step and its output requests:

Modify the CFD analysis step in the model named fluid.
1. In the Model Tree, expand the Steps container and double-click Step-1.
  The step editor appears.
2. From the Basic tabbed page, do the following:
  1. Modify the description to read Flow in a deformable hose.
  2. Set the time period of the step to 0.2 sec.
Modify the output requests.
1. In the Model Tree, expand the Field Output Requests container.
2. Double-click F-Output-1.
3. Select Every x units of time as the frequency, and enter 0.02 as the time interval.
4. Click OK.
  Abaqus/CAE makes the specified changes to the analysis.

E.6.3 Modifying the boundary conditions

You will now modify the boundary conditions. The no-slip/no-penetration wall boundary condition on the tube wall surface is suppressed because the fluid velocities and mesh displacements are dictated by the coupled solution. Therefore, it is not necessary to specify this boundary condition.

In addition, since the Arbitrary Lagrangian-Eulerian (ALE) method is activated to accommodate the displacements of the tube, appropriate boundary conditions are required for the mesh deformation solution.

To modify the boundary conditions:

Suppress the no-slip/no-penetration wall boundary condition on the tube wall surface.
1. In the Model Tree, expand the container for the fluid model and expand its BCs container.
2. Click mouse button 3 on the boundary condition named noSlip, and select Suppress from the menu that appears.
  Abaqus/CAE suppresses the wall boundary condition on the fluid surface.
Create the mesh displacement boundary conditions by defining a fixed-mesh condition at the inlet and outlet boundaries.
1. In the Model Tree, double-click BCs to create a new boundary condition named fix-mesh.
2. Select Mechanical as the category and Displacement/Rotation as the type, and click Continue.
3. Select fluid-1.fixed as the set to which the boundary condition will be applied.
4. Set U1, U2, and U3 to 0.
5. Click OK to close the boundary condition editor.

E.6.4 Defining the fluid-structure interaction

The CFD model includes a surface definition representing the region of the fluid that interacts with the tube surface. This surface is used to define the co-simulation interaction with the structural model.

To define a fluid-structure interaction:

In the Model Tree, double-click Interactions.
Name the interaction fsi.
Select Step-1 as the step in which it will be defined, and accept Fluid-Structure Co-simulation boundary as the type.
Select fluid-1.wall as the surface to which the interaction will be applied.
Click OK to close the interaction editor.

E.6.5 Specifying CFD analysis controls for co-simulation

The recommended practice to improve convergence behavior is to specify the ratio of the solid-to-fluid density. This specification is particularly important when the ratio is close to one, as is the case in this analysis (as shown below, the density of the tube is 1100 kg/m³, implying a ratio of 1.1).

You can specify the ratio of solid-to-fluid density in Abaqus/CAE using the keywords editor.

To specify CFD analysis controls:

In the Model Tree, click mouse button 3 on the fluid model and select Edit Keywords from the menu that appears.
The keywords editor appears.
Scroll down and click in the option block just prior to the *Co-simulation option block, and click Add After.
Enter the following:
```
*Controls, type=FSI
 , , , 1.1
```
Click OK.
Abaqus/CAE saves your changes to the CFD analysis controls.