OS-T: 1600 Fluid-Structure Interaction Analysis of Piezoelectric Harvester
Assembly
The purpose of this tutorial is to demonstrate how to carry out Fluid-Structure
Interaction analysis that is, with OptiStruct nonlinear
transient analysis coupling within AcuSolve fluid dynamic
analysis.
Before you begin, copy the file(s) used in this tutorial to your
working directory.
In this tutorial, you will explore the possibility of using piezoelectric based fluid
flow energy harvesters. These harvesters are self-excited and self-sustained in the
sense that they can be used in steady uniform flows. The configuration consists of a
piezoelectric cantilever beam with a cylindrical tip body (which is the structure
model) which promotes sustainable, aero-elastic structural vibrations induced by
vortex shedding and galloping. The structural and aerodynamic properties of the
harvester alter the vibration amplitude and frequency of the piezoelectric beam and
the fluid flow. As you may know, the Piezoelectric energy harvesting using fluid
flow involves the mutual interaction of three distinct dynamic systems, namely the
fluid, the structure and the associated electrical circuit.
Note: This tutorial is
limited to study only fluid and the structure domain.
Figure 1. Schematic of the Problem
Figure 2 illustrates the fluid structural model
used for this tutorial: the dimensions of the beam are shown in Figure 1 and Figure 2.Figure 2. Various Layers of Beam
Launch HyperMesh and Set the OptiStruct User Profile
Launch HyperMesh.
The User Profile dialog opens.
Select OptiStruct and click
OK.
This loads the user profile. It includes the appropriate template, macro
menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for
OptiStruct.
Import the Model
Click File > Import > Solver Deck.
An Import tab is added to your tab menu.
For the File type, select OptiStruct.
Select the Files icon .
A Select OptiStruct file browser
opens.
Select the Slab.fem file you saved
to your working directory.
Click Open.
Click Import, then click Close to
close the Import tab.
Set Up the Model
Create Set Segment
In the Model Browser, right-click and select Create > Set Segment from the context menu.
For Name, enter FSI_Interaction_Surf.
Click Color and select a color from the color
palette.
For Card Image, select SURF from the drop-down
menu.
For Elements, click 0 elements > elements and pick all the faces of the beam.
Figure 3. All sides of the beam except in the front
Click add to add the faces to the set segments.
Click return to exit from this panel.
Define Nonlinear Parameters
In the Model Browser, right-click and select Create > Load Step Inputs.
For Name, enter NLPARM.
For Config type, select Nonlinear Parameters from the
drop-down menu.
See NLPARM Bulk Data Entry for more information.Figure 7.
Define Output Control Parameters
From the Analysis page, select control cards.
Click GLOBAL_OUTPUT_REQUEST.
For DISPLACEMENT, ELFORCE, OLOAD, STRESS, and STRAIN, set Option to
Yes and click return.
Click PARAM.
Select LGDISP, and for LGDISP_V1 enter
1.
Click return twice to go to the main menu.
Create Nonlinear Transient Analysis Subcase
In the Model Browser, right-click and select Create > Load Step from the context menu.
For Name, enter
FSI.
Click Color and
select a color from the color palette.
For Analysis type, select Non-linear transient.
Input/Select the Load Collector.
Figure 8.
Submit the Job
From the Analysis page, click the OptiStruct
panel.
Figure 9. Accessing the OptiStruct Panel
Click save as.
In the Save As dialog, specify location to write the
OptiStruct model file and enter
Slab for filename.
For OptiStruct input decks,
.fem is the recommended extension.
Click Save.
The input file field displays the filename and location specified in the
Save As dialog.
Set the export options toggle to all.
Set the run options toggle to analysis.
Set the memory options toggle to memory default.
Click OptiStruct to launch
the OptiStruct job.
If the job is successful, new results files
should be in the directory where the Slab.fem was written. The Slab.out file is a good place to look for error messages that could help
debug the input deck if any errors are present.
Submit the AcuSolve Job
Open the AcuSolve input file (slab_dcfsi.inp) in a
text editor.
Change the socket_host
parameter in the EXTERNAL_CODE block to your machines hostname and save the
file.
Figure 10.
Open the AcuSolve Cmd Prompt application.
Enter the command: acuRun-pb slab_dcfsi -np 8.
Figure 11.
If the job is successful, you will see new
results files in the directory where HyperMeshwas invoked. The
Slab.out file is where you will find
error messages that will help you debug your input
deck, if any errors are present.
The default
files that will be written to your directory
are:
cci.txt
Contains information pertaining to model
progression. Logs regarding connection
establishment, initial external code handshake and
subsequent time step data in conjunction with
exchange/stagger.
Slab.html
HTML report of
the analysis, giving a summary of the problem formulation and the analysis
results.
Slab.out
ASCII based
output file of the model check run before the simulation begins and gives some basic
information on the results of the run.
Slab.stat
Summary of analysis process, providing CPU
information for each step during the process.
Slab.h3d
HyperView
compressed binary results file.
View the Results
Using HyperView, plot the Displacement contour at 1.0 s.