You will now create the structural model for the tube.
In the Model Tree, double-click Models. In the Edit Model Attributes dialog box, enter solid as the name and select Standard & Explicit as the model type. Click OK.
The structural part will be based on the existing part used to define the fluid. You will modify the structural part to represent the U-shaped tube by deleting the existing features of the part and creating a shell from the solid.
To define the part:
From the main menu bar, select Model
Copy Objects. In the Copy Objects dialog box, select fluid as the From model and solid as To model.
Expand the Parts container, and select the fluid part.
Click OK.
Abaqus/CAE copies the fluid part from the fluid model into the solid model.
Rename the part. In the Model Tree, expand the Parts container underneath the solid model. Click mouse button 3 on the fluid part, and select Rename from the menu that appears.
In the Rename Part dialog box, enter solid as the new name and click OK.
To delete the existing features of the solid part:
In the Model Tree, expand the Section Assignments container under the solid part.
Click mouse button 3 on the section fluid (which is no longer relevant), and select Delete from the menu that appears. Click Yes to confirm the operation.
Expand the Sets container under the solid part.
Select all the sets, click mouse button 3 on the selections, and select Delete from the menu that appears. Click Yes to confirm the operation.
Repeat this process to delete all the surfaces and all the face and cell partitions.
To create a shell from the solid:
From the main menu bar in the Part module, select ToolsGeometry Edit. In the Geometry Edit dialog box, select Face as the category and Remove as the method.
Select the faces representing the inlet and the outlet.
Click Done in the prompt area.
Click OK when prompted to delete faces.
Close the Geometry Edit dialog box.
Click mouse button 3 on the solid part, and select Update Validity from the menu that appears. Abaqus/CAE updates the features of the part.
To assign biased meshing to the part, we will first partition it.
To partition the part:
In the Model Tree, expand the solid item under the Parts container and double-click Mesh in the menu that appears.
Create a datum plane by clicking the Create Datum Plane: Offset From Principal Plane tool 
.
Click XY Plane in the prompt area. Accept the default offset of 0.0, and press [Enter].
Click the Partition Face: Use Datum Plane 
tool to create a partition running along the length of the tube.
Select all the faces of the tube in the viewport, and click Done in the prompt area.
Select the datum plane created in the previous step, and click Create Partition in the prompt area.
You will now create sets and surfaces that will be utilized to define section properties and boundary conditions.
To define sets:
In the Model Tree, expand the container for the solid part.
Double-click Sets. In the Create Set dialog box, name the set all and click Continue.
Select the entire geometry in the viewport, and click Done in the prompt area.
Abaqus/CAE creates a set containing the entire part.
Repeat this procedure to create a set named ends containing the edges at the inlet and outlet regions of the tube.
To define surfaces:
In the Model Tree, expand the container for the solid part.
Double-click Surfaces. In the Create Surface dialog box, name the surface inner and click Continue.
In the prompt area, select by angle as the selection technique. Select the surface of the tube.
In the prompt area, select the color associated with the inner surface of the tube (purple).
Repeat the previous steps to create a surface named outer by selecting the outer surface (brown) of the shell.
The next step in creating the model involves defining and assigning material and section properties to the structural part. Each region of the model must refer to a section property. In this model we are modeling a flexible rubber material using a linear elastic material model. The material properties include a density of 1100 kg/m3, an elastic modulus of 1 MPa, and a Poisson’s ratio of 0.45. The tube thickness is assumed to be 2 mm.
To define material properties:
In the Model Tree, double-click Materials to create a new material named elastic.
From the General menu of the material editor, select Density and enter a value of 1100 kg/m3.
From the Mechanical menu of the material editor, select ElasticityElastic.
Enter a value of 1.e6 Pa as the Young’s Modulus and 0.45 as the Poisson’s Ratio.
Click OK.
To define a shell section:
In the Model Tree, double-click Sections to create a new section named shell.
Select Shell as the category and Homogeneous as the type. Click Continue.
In the Edit Section dialog box, enter 0.002 as the value of the constant shell thickness.
Select elastic as the material.
Click OK.
To assign the shell section:
In the Model Tree, expand the Parts container. Expand the container for the part named solid.
Double-click Section Assignments.
In the prompt area, click Sets. In the Region Selection dialog box, choose all and click Continue.
Click Done in the prompt area.
In the section assignment editor, choose the shell section created earlier and click OK.
You will now create a mesh for the tube structure.
To create the mesh:
In the Model Tree, expand the solid item under the Parts container and double-click Mesh in the menu that appears.
Note that the entire tube is colored pink, which means that the part can be meshed with the default free meshing technique.
Change the meshing technique to sweep.
From the main menu bar, select MeshControls.
Select the entire part in the viewport to assign new controls, and click Done in the prompt area.
In the Mesh Controls dialog box, select Sweep as the technique and click OK.
Abaqus/CAE changes the part's color to yellow in the current viewport.
Assign mesh seeds. You create biased seeds for the inlet and outlet regions of the tube. This seeding method creates a mesh that is coarser axially at the inlet and outlet and finer in the middle sections of the tube.
Click the Seed Edges tool 
, and click Select in Viewport in the prompt area (if necessary).
In the viewport, select the straight edges in the inlet and outlet regions running along the midplane and click Done.
In the Local Seeds dialog box, select By size as the method, Single as the bias type, and enter 0.0045 as the minimum size and 0.01 as the maximum size.
Ensure that the seeding bias is such that seeds are concentrated away from inlet and outlet regions of the tube (i.e., each arrow should point axially inward). Flip the direction of any arrow that violates this condition.
Set the global seed size.
Click the Seed Part tool 
.
In the Global Seeds dialog box, enter 0.004 as the approximate global size.
Accept all the other default values, and click OK.
Abaqus/CAE sets the global seed size for the part.
Mesh the part.
Click the Mesh Part tool 
.
Click Yes in the prompt area.
Abaqus/CAE creates a mesh for the part with approximately 950 shell elements.
You will now create an instance of the part in the assembly to include it in your model.
To instance a part:
In the Model Tree, expand the Assembly container and double-click Instances in the list that appears to create an instance of the part.
In the Create Instance dialog box, select solid from the Parts list and click OK.
You will now define the analysis step. An implicit dynamic procedure is used to model the structural response of the tube.
To define an implicit dynamic analysis step:
In the Model Tree, double-click Steps.
In the Create Step dialog box, accept the default procedure type (General) and the default name (Step–1). From the list of available procedures, select Dynamic, Implicit and click Continue.
From the Basic tabbed page of the step editor, do the following:
Enter deformation of the tube as the description.
Enter 0.2 sec as the time period.
Toggle on Nlgeom.
Select Transient fidelity as the application type.
From the Incrementation tabbed page of the step editor, do the following:
Enter 1000 as the maximum number of increments.
Enter 0.001 as the initial increment size.
Enter 2.e-6 as the minimum increment size.
Toggle on Suppress calculation for the Half-increment Residual.
Click OK to create the step.
To define output requests:
In the Model Tree, expand the Field Output Requests container.
Double-click F-Output-1.
Select Every x units of time as the output frequency, and enter 0.02 as the time interval.
Accept the default output variables, and click OK.
The tube is secured at each end, so you need to define an encastre boundary condition for the set definition that includes the ends of the tube.
To define the boundary conditions:
In the Model Tree, double-click BCs underneath the solid model.
In the Create Boundary Condition dialog box, name the boundary condition fixed-ends and select Initial as the step.
Accept Mechanical as the category, and select Symmetry/Antisymmetry/Encastre as the type.
Click Sets in the prompt area.
In the Region Selection dialog box, select the set named solid-1.ends and click Continue.
In the Edit Boundary Condition dialog box, select Encastre and click OK.
Abaqus/CAE creates the boundary condition.
The structural model includes a surface definition representing the regions of the tube that interact with the fluid. This surface is used to define the co-simulation interaction with the Abaqus/CFD model.
To create a fluid-structure interaction:
In the Model Tree, double-click Interactions.
Name the interaction fsi.
In the Create Interaction dialog box, select Step-1 as the step and Fluid-Structure Co-simulation boundary as the type. Click Continue.
In the Region Selection dialog box, select solid-1.inner as the surface to which the interaction will be applied and click Continue.
In the interaction editor, click OK.
Abaqus/CAE creates the fluid-structure interaction.