4.4. Example Simulation of a Piezoelectric Actuated Micro-Pump

www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS



Problem Description

The working principle of micro-pumps is the actuation of a flexible membrane to obtain the driving pressure for the fluid flow. Electro-thermal, electrostatic, or piezoelectric actuators are most commonly used for this purpose.

The benchmark problem is taken from A. Klein and demonstrated 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. To estimate the fluid damping and inertial forces on the membrane, a simplified process of the membrane actuation is considered here. 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, which is maintained at a constant level subsequently.

Figure 4.6  Piezoelectric Micropump Description

ANSYS coupled field element SOLID5 with displacement and voltage DOFs is used for the piezoelectric material and SOLID95 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):

Figure 4.7  Model Dimensions

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.

Figure 4.8  Model Boundary Conditions


Back To Top

Set Up the Piezoelectric and Fluid Inputs

The first step in this example is to create two ANSYS .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 ANSYS runs using the input files piezo.inp and CFX_fluid.inp, respectively. This example provides the models (under /ansys_inc/v110/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. ANSYS and CFX use these names in their communication during the solution.

To create the two ANSYS .cdb files, follow the steps below:

  1. Open the ANSYS Launcher.

    Windows: Choose menu path Start> Programs> ANSYS 11.0> ANSYS Product Launcher.
    UNIX: Type launcher110.

  2. Select the Simulation Environment ANSYS Batch.

  3. Select a multiphysics license.

  4. The File Management tab is activated by default. In the File Management tab:

    • Enter the working directory where the piezo.inp and CFXfluid.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.

  5. Click Run. This input file will create the pfsi-solid.cdb file to be used later.

Repeat this process for the CFXfluid.inp file, using CFXfluid.inp as the input file name, and CFXfluid.out as the output file name. This input file will create the fluid.cdb file that will be used later.


Back To Top

Set up the CFX Model and Create the CFX Definition File

In this series of steps, you will set up the example in the CFX preprocessor.

  1. Start CFXpre from the CFX launcher.

  2. Create a new simulation and name it cfx_mfxexample.

  3. Load the mesh from the ANSYS file named fluid.cdb. The mesh format is ANSYS. Accept the default unit of meters for the model.

  4. Define the simulation type:

    1. Set External Solver Coupling to ANSYS MultiField via Prep7.

    2. Load the ANSYS input file at ANSYS Input File to launch the MFX run from the CFX Solver Manager.

    3. Set Option to Transient.

    4. Set Time duration to Coupling Time Duration.

    5. Set Time steps to Coupling Timesteps.

    6. Set Initial time - Option to Automatic with Value, and set Time to 0 [s].

  5. Create the fluid domain and accept the default domain name. Use Primitive 3D as the location.

  6. Edit the fluid domain using the Edit domain - Domain1 panel.

    1. Set Fluids list to Air at 25 C.

    2. Set Mesh deformation - Option to Regions of motion specified. Accept the default value of mesh stiffness.

    3. In the Fluid models tab, set Turbulence model - Option to None (laminar).

    4. Accept the remainder of the defaults.

    5. Initialize the model in the Initialisation tab. Click Domain Initialisation, and then click Initial Conditions. Select Automatic with value and set velocities and static pressure to zero.

  7. Create the interface boundary condition. This is not a domain interface. Set Name to Interface1.

    1. In the Basic settings tab: - Set Boundary type to Wall. Set Location to FSI.

    2. In the Mesh motion tab: Set Mesh motion - Option to ANSYS Multifield.

    3. Accept the defaults for boundary details.

  8. Create the opening boundary condition. Set Name to Opening.

    1. 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 Static pres. (Entrain). Set Relative pressure to 0 Pa.

    3. In the Mesh motion tab: Accept the Mesh motion - Option default of Stationary.

  9. Create the wall boundary condition. Set Name to Bottom. Edit the wall boundary condition using Edit boundary: Bottom in Domain: Domain1 panel.

    1. In the Basic settings tab: Set Boundary type to Wall. Set Location to Bottom.

    2. In the Boundary Details tab: Set Wall influence on flow - Option to No slip.

    3. In the Mesh motion tab: Set Mesh motion to Stationary.

  10. Create another wall boundary condition. Set Name to Top. Edit the wall boundary condition using Edit boundary: Top in Domain: Domain1 panel.

    1. In the Basic settings tab: Set Boundary type to Wall. Set Location to Top.

    2. In the Boundary Details tab: Set Wall influence on flow - Option to No slip.

    3. In the Mesh motion tab: Set Mesh motion to Stationary.

  11. Create the end symmetry boundary condition. Set Name to Sym.

    1. In the Basic settings tab: Set Boundary Type to Symmetry. Set Location to Pipe.

    2. In the Mesh motion tab: Set Mesh motion to Unspecified.

  12. Create the side symmetry boundary condition. Set Name to Symmetry. Edit the symmetry boundary condition using Edit boundary: Side1 in Domain: Domain1 panel.

    1. In the Basic settings tab: Set Boundary type to Symmetry. Set Location to Side1 and Side2. Use the Ctrl key to select multiple locations.

    2. In the Mesh motion tab: Set Mesh motion to Unspecified.

  13. Accept the defaults for Solver Control.

  14. Generate transient results to enable post processing through the simulation period.

    1. Click Output Control.

    2. Go to Trn Results tab.

    3. Create New. Accept Transient Results as the default name.

    4. Choose Time Interval and set to 5E-5.

    5. Accept the remaining defaults.

  15. Create the CFX definition file.

    1. Choose menu path File> Write Solver File. Name the file cfx_mfxexample.def.

    2. Select Operation: Write Solver File.

    3. Click Quit CFX Pre.

    4. Click OK.


Back To Top

Set Up the MFX Launcher Controls

Follow the steps below to set up the MFX controls in ANSYS. The first step reads in the pfsi-solid.cdb input file, which includes the preliminary model and preprocessing information.

  1. Open the ANSYS Launcher.

    Windows: Choose menu path: Start> Programs> ANSYS 11.0> ANSYS Product Launcher
    UNIX: Type launcher110.

  2. Select an ANSYS Multiphysics license.

  3. Set your working directory or any other settings as necessary. See The ANSYS Launcher in the Operations Guide for details on using the ANSYS launcher.

  4. Click Run.

  5. When ANSYS has opened, choose menu path Utility Menu> File> Read Input From and navigate to the file pfsi-solid.cdb. Click OK.

  6. Choose menu path Main Menu> Solution> Multi-field Set Up> Select Method.

  7. For the MFS/MFX Activation Key, click ON.

  8. Click OK.

  9. Click MFX-ANSYS/CFX and click OK.


Back To Top

Set Up the MFX Groups in ANSYS

  1. Choose menu path Main Menu> Multi-field Set Up> MFX-ANSYS/CFX> Solution Ctrl.

  2. Select Sequential. Enter .5 for the relaxation value and click OK.

  3. On the next dialog box, for Select Order, choose Solve ANSYS First and click OK.


Back To Top

Set Up the MFX Time Controls and Load Transfer in ANSYS

  1. Choose menu path Main Menu> Multi-field Set Up> MFX-ANSYS/CFX> Load Transfer.

  2. Enter Interface1 for the CFX Region Name.

  3. For Load Type, accept the default of Mechanical.

  4. Click OK.

  5. Choose menu path Main Menu> Multi-field Set Up> MFX-ANSYS/CFX> Time Ctrl.

  6. Set MFX End Time to 5e-4.

  7. Set Initial Time Step to 5e-6.

  8. Set Minimum Time Step to 5e-6.

  9. Set Maximum Time Step to 5e-6.

  10. Accept the remaining defaults and click OK.


Back To Top

Set Up MFX Advanced Options in ANSYS

  1. Choose menu path Main Menu> Multi-field Set Up> MFX-ANSYS/CFX> Advanced Set Up> Iterations.

  2. Note the defaults and click OK.

  3. Choose menu path Main Menu> Multi-field Set Up> MFX-ANSYS/CFX> Advanced Set Up> Convergence.

  4. Select All and click OK.

  5. On the next dialog box, accept the default of 1.0e-3 for Convergence for All Items and click OK.

  6. In the Command Input window, type MFOU,1 to write the output for every time step.

  7. In the Command Input window, type KBC,1 to specify stepped loading.

  8. Choose menu path Main Menu> Multi-field Set Up> MFX-ANSYS/CFX> Write input. Name the file mfxexample.dat.

  9. Exit ANSYS.


Back To Top

Run the Example from the ANSYS Launcher

  1. Open the ANSYS Launcher.

  2. Select MFX - ANSYS/CFX as the simulation environment.

  3. In the MFX - ANSYS/CFX Setup tab:

    • Enter the ANSYS working directory you have been using. You can type this directory in or select it via browsing.

    • Enter ansys_mfxexample for the ANSYS jobname.

    • Enter mfxexample.dat for the ANSYS input file.

    • Enter mfxexample.out for the ANSYS output file.

    Specify the following CFX settings:

    • CFX Working Directory

    • Enter cfx_mfxexample.def for the CFX definition file. You can leave the remaining CFX settings blank.

    • (UNIX only) Enter the CFX installation directory.

  4. Click Run.


Back To Top

View the Results

You can view results from both the ANSYS and the CFX portions of the run. The following figure shows the response of the vertical displacement of the silicon membrane's center point (ANSYS).

Figure 4.9  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 (ANSYS).

Figure 4.10  von Mises Stress Distribution

The following figure shows air streamline velocity from CFX at t = 500 μs (CFX).

Figure 4.11  Air Streamline Velocity