The following topics are available for this example simulation:
In a micro-pump, a flexible membrane is moved back and forth to obtain the driving pressure for the fluid flow. Electro-thermal, electrostatic, or piezoelectric actuators are most commonly used to move the membrane.
This example, based on a benchmark from A. Klein, analyzes such a micro-pump, shown in Figure 4.6: Piezoelectric Micropump Description. This device consists of a fluid chamber with a deformable membrane at the top. The membrane is actuated by a piezoelectric layer during pump operation.
This example shows an approach that can be beneficial in any complicated analysis: a simplified study is done in preparation for a more rigorous one. Some reasons for doing a simplified analysis first are to investigate the basic responses of the model, to verify that the appropriate steps, loads, settings, etc., have been included in the analysis, or to determine the relative importance of modeling certain aspects of the system. Specifically, in this example, a static analysis is done on the mechanical portion of the analysis, thereby ignoring the damping and inertial effects of the membrane movement. The membrane movement is also simplified: with the diaphragm in the neutral position and the chamber filled with the working fluid, the PZT layer is actuated at t = 0 with an electric field and then held in that position for the duration of the analysis.
The coupled field element SOLID5 with displacement and voltage DOFs is used for the piezoelectric material and SOLID186 is used for the silicon membrane. Air at 25 degrees Celsius is used as the working fluid for the CFX solver.
The following material properties were used for the silicon:
| Young's Modulus: 1.689e11 Pa |
| Poisson's ratio: 0.3 |
| Density: 2329 kg/m3 |
The following material properties were used for the piezoelectric material (PZT4):
| Density: 7500 kg/m3 |
| X and Z Permittivity: 804.6 (Polar axis along Y axis) |
| Y Permittivity: 659.7 |
The elasticity stiffness matrix is shown here (N/m2 units):
The piezoelectric stress matrix is shown here (C/m2 units):
This model has a 0.1 mm thickness in the z direction, and both side surfaces have a Uz = 0 boundary condition for the structural part, and a symmetry condition for the fluid part.
Perform the following setup tasks for this example simulation:
The first step in this example is to create two .cdb files, one to set up the piezoelectric analysis and one to set up the fluid analysis. These files will be imported into the MFX solver. You will create these files with two batch runs using the input files piezo.inp and CFX_fluid.inp, respectively. This example provides the models (under /ansys_inc/v182/ansys/data/models); you must be familiar with setting up a piezoelectric analysis and familiar with creating a CFX fluid mesh.
You will then set up the CFX model in CFX-Pre and create the CFX definition file. Finally, step by step instructions are provided for interactively setting the MFX input and creating the MFX input file. This will then be executed through the MFX launcher.
It is important that you enter all names exactly as shown in this example, including spaces and underscores. Mechanical APDL and CFX use these names in their communication during the solution.
To create the two .cdb files, perform these steps:
Open the Mechanical APDL Product Launcher.
| Windows: Select menu path . |
Linux: Type
launcher182. |
Select the Simulation Environment .
Select an appropriate license (one that supports multiphysics capabilities).
The File Management tab is activated by default. In the File Management tab:
Enter the working directory where the piezo.inp and CFX_fluid.inp files are located. You can type this directory in or select it via browsing.
Enter a unique jobname.
Enter piezo.inp for the input file.
Enter piezo.out for the output file.
Click . This input file will create the pfsi-solid.cdb file to be used later.
Repeat this process for the CFX_fluid.inp file, using CFX_fluid.inp as the input file name, and CFX_fluid.out as the output file name. This input file will create the fluid.cdb file that will be used later.
Perform the steps below to set up the MFX controls. The first step reads in the pfsi-solid.cdb input file, which includes the preliminary model and preprocessing information.
Open the Mechanical APDL Product Launcher.
| Windows: Select menu path: |
Linux: Type
launcher182. |
Select a license.
Set your working directory or any other settings as necessary. See The Mechanical APDL Product Launcher in the Operations Guide for details on using the Mechanical APDL Product Launcher.
Click .
After the program has opened, select menu path and navigate to the file pfsi-solid.cdb. Click .
Select menu path .
For the MFS/MFX Activation Key, click .
Click .
Click and click .
Select menu path .
Select . Enter .5 for the relaxation value and click .
On the next dialog box, for Select Order, select Solve ANSYS First and click .
Select menu path .
Enter Interface1 for the CFX Region Name.
For Load Type, accept the default of Mechanical.
Click .
Select menu path .
Set MFX End Time to 5e-4.
Set Initial Time Step to 5e-6.
Set Minimum Time Step to 5e-6.
Set Maximum Time Step to 5e-6.
Accept the remaining defaults and click .
Select menu path .
Note the defaults and click .
Select menu path .
Select and click .
On the next dialog box, accept the default of 1.0e-3 for Convergence for All Items and click .
In the Command Input window, type
MFOUTPUT,1 to write the output for every
time step.
In the Command Input window, type
KBC,1 to specify stepped loading.
Select menu path . Name the file mfxexample.dat.
Exit the program.
In this series of steps, you will set up the example in the CFX preprocessor.
Start CFXpre from the CFX launcher.
Create a new simulation and name it cfx_mfxexample.
Select File > Import Mesh. Load the mesh from the fluid.cdb file. The mesh format is . Accept the default unit of meters for the model.
Define the simulation type:
Set External Solver Coupling to ANSYS MultiField via PREP7.
Set Mechanical Input File to mfxexample.dat.
Set Option to Transient.
Set Time Duration to Coupling Time Duration.
Set Time Steps to Coupling Timesteps.
Set Initial Time > Option to Coupling Initial Time.
If Default Domain does not already exist, create the fluid domain and accept the default domain name. Use Primitive 3D as the location.
Edit the fluid domain by double-clicking Default Domain.
Set Fluid 1 > Material to Air at 25 C.
Set Mesh deformation - Option to Regions of motion specified. Accept the default value of mesh stiffness.
In the Fluid models tab, set Turbulence model - Option to None (laminar).
Accept the remainder of the defaults.
Initialize the model in the Initialisation tab. Click , and then click . Select Automatic with value and set velocities and static pressure to zero.
Create the interface boundary condition via Insert > Boundary. This is not a domain interface. Set Name to Interface1.
In the Basic settings tab: - Set Boundary type to Wall. Set Location to FSI.
In the Boundary Details tab: Set Mesh motion - Option to ANSYS Multifield.
Accept the defaults for boundary details.
Create the opening boundary condition via Insert > Boundary. Set Name to Opening.
In the Basic settings tab: Set Boundary type to Opening. Set Location to Opening.
2. In the Boundary details tab: Set Mass and momentum - Option to Entrainment. Set Relative pressure to 0 Pa.
3. Accept the Mesh motion - Option default of Stationary.
Create the wall boundary condition via Insert > Boundary. Set Name to Bottom. Edit the wall boundary condition using panel.
In the Basic settings tab: Set Boundary type to Wall. Set Location to Bottom.
In the Boundary Details tab: Set Mass And Momentum - Option to No slip
Set Mesh motion to Stationary.
Create another wall boundary condition via Insert > Boundary. Set Name to Top.
In the Basic settings tab: Set Boundary type to Wall. Set Location to Top.
In the Boundary Details tab: Set Mass And Momentum - Option to No slip.
Set Mesh motion to Stationary.
Create the end symmetry boundary condition. Set Name to Sym.
In the Basic settings tab: Set Boundary Type to Symmetry. Set Location to Pipe.
Set Mesh motion to Unspecified.
Create the side symmetry boundary condition via Insert > Boundary. Set Name to Symmetry. Edit the symmetry boundary condition using panel.
In the Basic settings tab: Set Boundary type to Symmetry. Set Location to Side1 and Side2. Press … and use the Ctrl key to select multiple locations.
2. Set Mesh motion to Unspecified.
Accept the defaults for Solver Control.
Generate transient results to enable postprocessing through the simulation period.
Click .
Go to Trn Results tab.
Create New via the button on the right. Accept Transient Results as the default name.
Select Time Interval and set to 5E-5.
Accept the remaining defaults.
Create the CFX definition file.
Select menu path . Name the file cfx_mfxexample.def.
Click .
Click .
From the command line, launch the master process by issuing the following commands:
ansys182 -p productname -b -j ansys_mfxexample
-mfm ANSYS -i mfxexample.dat -o mfxexample.out
cat ansys_mfxexample.portThe cat ansys_mfxexample.port command will print the
listening port number to the screen. You will need this port number in the next
step.
Note: This command and the following command must be running simultaneously. Either the 'cat' command and the following cfx command should be run in separate windows, or an ampersand (&) should be issued at the end of the first command so that the following command can be run before the first is terminated.
From the command line, launch the slave CFX process by issuing the following commands:
cfx5solve -def cfx_mfxexample.def -cplg-slave CFX -cplg-hostport#@ansys_hostname
Where port# is the port number from step 1, above,
and ansys_hostname is the name of the master
machine.
You can view results from both the Mechanical APDL and the CFX portions of the run. The following figure shows the response of the vertical displacement of the silicon membrane's center point:
The following figure shows the von Mises stress distribution for piezoelectric and silicon layer at t = 500 μs.
The following figure shows air streamline velocity from CFX at t = 500 μs (CFX).