ADINA-FSI Analysis with Nastran Input

Description of Simple FSI Example The FSI example is an analysis of flow over a flexible structure. The FSI boundary indicates where the structure is located. We will first describe the fluid model and then the structural model. The Nastran file for the fluid model consists of 3D elements coated with shell elements on the external boundary. When imported into the AUI (ADINA CFD program module), the 3D elements with four different PIDs become four 3D fluid element groups and the each set of shell elements with the same PID becomes one element face set and node set where loads and boundary conditions may be applied. It is intentional to create four different 3D fluid element groups in this model even though the fluid properties in all four groups are the same. For fluid regions that involve moving boundaries (in this case FSI), it is important that the fluid boundary does not have regions which are concave. This allows the fluid mesh to undergo relatively large deformation without the need for adaptive remeshing. The Nastran file for the structural model also consists of 3D elements and shell elements coated on boundaries where boundary conditions are to be applied. Observe that at the two ends of the 3D elements (thin triangular surfaces), no shell elements need to be coated as there are no boundary conditions to be applied on those surfaces. Procedure for Creating the Example FSI Model Right-click on the links to save the two Nastran files (fsi01_a.nas and fsi01_f.nas) containing the nodes and elements for the structural and fluid models to your working directory. Start the AUI and select ADINA Structures program module. We will first create the structural model. Since this is going to be an FSI analysis, we will also select the FSI option. Click menu: File > Import NASTRAN... In the Import NASTRAN File dialog box, select fsi01_a.nas and set the option to create element face sets and node sets. Then click Open. The Log Window will pop up and show some warning messages. Click Close to close the window. We will set the global degrees of freedom for the model to allow only Y-translation and Z-translation. Click on menu: Control > Degrees of Freedom... and toggle off X-translation and all rotations. Click OK to apply these settings. Click on the Mesh Plot icon and the Node Symbols icon to display the elements and nodes. You can then examine the node sets and element sets created based on the shell elements coated on the 3D elements (menu: Meshing > Nodes > Node Set... and Meshing > Elements > Element Face Set...). The node set or element face set that is shown in the dialog box will be highlighted on the mesh plot (white highlight below). We will now use node set 3 to apply fixed boundary conditions. Click on the Apply Fixity icon . Make sure that Apply to: Node Sets is selected. Specify Node Set 3 in the table. Since the default fixity "ALL" is to be applied, it is not necessary to specify it in the table. Click OK to apply and close the dialog box. Next, we apply the FSI Boundary on element face set 2. Click on menu: Model > Boundary Conditions > FSI Boundary... Now, click Add, select Type: Element-Face Sets, and specify element-face set 2 in the table. Then, click OK to apply and close the dialog box. This completes the definition of the structural model. We will create the data file for the model. Click on the Data File/Solution icon . Specify File Name: fsi01_a and make sure the Run ADINA check box is off. We will proceed with the fluid model. Click on the New icon and click Yes when prompted whether to discard all changes and continue. In the module bar, select ADINA CFD and FSI option. Turn on the option to define special boundary conditions on element-face sets. Click on menu: Control > Miscellaneous Options... and select the Element option. Import Nastran fsi01_f.nas with the option to create element face sets and node sets. After importing the file, click on the Mesh Plot icon and you can examine the element face sets and nodes sets that has been created. We will apply normal traction load on element face set 5. Click on the Apply Load icon . In the Apply Usual Boundary Conditions/Loads dialog box, select Load Type: Normal Traction and click on the Define button. In the Define Normal Traction dialog box, click on Add and specify 3 for Magnitude. Then click OK. Back in the Apply Load dialog box, specify 5 for Site # in the table and click OK. Next, we apply wall boundary conditions on element face sets 7, 8 and 9 and FSI boundary condition on element face set 12. Click on the Special Boundary Condition icon . In the dialog box, click Add to define special boundary condition 1. Make sure that Type: Wall is selected. Then, specify element-face set 7 in the table. Click Add to define special boundary condition 2, Type: Wall on element-face set 8 and then special boundary condition 3, Type: Wall on element-face set 9. Finally, click Add to define special boundary condition 4, Type: Fluid Structure Interface on element-face set 12. Note that an FSI boundary condition defined in the structural model must be referenced by this boundary condition. Click OK to close the dialog box. Now, we will impose zero velocity in the X direction on node sets 10 and 11. Click on the Apply Fixity icon . Make sure that Apply to: Node Sets is selected. Click on the Define button. In the Define Zero Values dialog box, click on Add button. Specify New Name: ZEROU, toggle on X-Velocity and click OK. Back in the Apply Zero Values dialog box, select ZEROU as Default Zero Values. Then, specify node sets 10 and 11 in the table and click OK. As the structure deforms, we want the fluid mesh to move in a uniform manner with minimal local element distortion. This is done using the leader follower feature. Click on menu: Meshing > ALE Mesh Constraints > Leader Follower... In the dialog box, specify two pairs of leader follower as illustrated below. As the structure deforms, node 661 will follow the horizontal movement of node 782 and node 1 will follow node 122. Finally, we turn off the heat transfer option for this model and define the fluid material properties. Click on menu: Model > Flow Assumptions... and toggle off the Heat Transfer option and click OK. Click on menu: Model > Materials > Constant... In the Define Material dialog box, specify 1 for Viscosity and Density and click OK. The fluid model definition is now complete and we can create the data file. Click on the Data File/Solution icon . Specify File Name: fsi01_f and make sure the Run ADINA-F check box is off. Running the FSI Analysis We will use the structural and fluid model data files created above to run the ADINA-FSI analysis. You can start the ADINA-FSI program from within the AUI. Click on menu: Solution > Run ADINA-FSI... In the ADINA-FSI window, click on Start. Specify the fsi01_a.dat and fsi01_f.dat files and click Start to run the analysis. When the analysis is completed, click on Close to exit the ADINA-FSI program. You can then load the porthole (result) files in the AUI for post-processing. Shown below is a particle trace plot for the CFD results.