SIMULATION OF AN ULTRASONIC PIEZOELECTRIC TRANSDUCER

by David H. Johnson, P.E., Penn State-Erie
and Dharmendra Pal, Cybersonics, Inc.

ABSTRACT

This paper presents the piezoelectric, coupled field capability of the ANSYS/Multiphysics™ product in both linear and nonlinear simulations. A piezoelectric transducer assembly is modeled, including a discussion of vendor-supplied property data as it relates to the ANSYS material input requirements. A cylindrical geometry is treated as an axisymmetric model using the PLANE13 element type. The transducer model is used in modal and harmonic analysis solutions to understand its mechanical behavior and to aid in design modifications to optimize its weight, performance, and electrical power consumption.

Experimental measurements made with a Philtec optical sensor are compared to harmonic analysis amplitude results. This sensor device, using a light source, fiber-optic transducer and an oscilloscope display, can measure the high frequency (~22 kHz) vibrations of the transducer assembly.

INTRODUCTION

A piezoelectric transducer has been designed by Cybersonics, Inc. of Erie, PA, USA to be included on the NASA/JPL Mars rover mission in 2003. This device will be used to drill core samples of rocks on Mars in the search for traces of water and organic matter in the history of Mars, when the rocks were formed. A piezoelectric device is a viable design for this program because of its low power requirement compared to a conventional, rotating drill. The R&D for this device has been underway for several years at Cybersonics and functional prototypes have been produced. The ultrasonic transducer designed for this purpose operates by developing axial vibrations in piezoelectric ceramic rings. This motion is transmitted through the front mass (or horn) to a hollow tube probe which can drill through stone much like a jack hammer (see Figure 1).

Along with the typical, minimum weight requirement for a rocket launch and transport on an interplanetary mission, this design was also given an operating target of less than 5.0 Watts of power consumption. Operating a conventional, hand-held carpenter's drill requires power at 200-400 Watts and is quite far from the low power level allocated for this Mars rover mission. The piezoelectric device prototypes do perform well at the target power level and can drill effectively through common rock specimens of earth. Beyond the focus of this project, Cybersonics Inc. produces a variety of piezoelectric devices with industrial applications in ultrasonic cleaning, as well as, medical uses for pacemaker lead replacement, clearing the pores in brain shunt tubes, and breaking up thromboses (blood clots) without invasive surgery.

PIEZOELECTRIC MATERIAL DATA

Most manufacturers of piezoelectric materials do not publish the material properties in a format that can be directly entered into an ANSYS model. The published data must be converted and transformed to populate the necessary material matrices that ANSYS expects for the piezoelectric material input. Specifically, ANSYS [1,2] requires a dielectric matrix [e], a piezoelectric matrix [e], and either a compliance matrix [d] or a stiffness matrix [c].

The dielectric matrix, [e], defines the electrical permittivity in typical units of Farads/meter. This matrix is a 3x3, diagonal matrix for a 3D model and the data is entered into ANSYS as an orthotropic material property with the labels PERX, PERY, and PERZ. (In a 3D model, PERZ is the axial or polarized direction in the element coordinate system). In a 2D model, only the PERX and PERY values are entered, with PERY being the polarized direction.

The piezoelectric matrix, [e], relates the electric field to stress and typically has units of Coulombs/meter². For a 3D model, this matrix is a 6x3 matrix and the data is entered into ANSYS as a material data table of type, PIEZ. In a 2D model, the piezoelectric matrix is 4x2 in size.

While ANSYS will accept stiffness data in terms of the elastic modulus and Poisson's ratio, it seems more common in practice to define either the compliance matrix [d] or the stiffness matrix [c] for a piezoelectric coupled-field analysis. Units for the terms in the compliance matrix [d] are typically meter²/Newton, while in the stiffness matrix [c], Newtons/meter² is commonly used. The analyst selects which matrix to input with the element option switch for the coupled-field element type, then enters the 6x6 symmetric matrix data as a material data table of type, ANEL. In a 2D model, the stiffness or compliance matrix is 4x4 in size.

For the transducer design discussed in this paper, PZT-8 material was selected. PZT-8 is an appropriate choice for this application because " PZT-8 is a high power material generally similar to PZT-4 but it has much lower dielectric losses under high electric drive and has greater resistance to depolarization."^[3]

Morgan Matroc Inc., a popular manufacturer of piezoelectric ceramics, lists data ^[3,4] for the PZT-8 material as:

Relative dielectric constant (free):

where the dielectric constant of free space, eO = 8.85 x 10^-12 farads/meter. The superscript notation, e^T, indicates that the dielectric constant is measured on a free (as opposed to a clamped) specimen. The subscript notation, 11 and 33, indicate the transverse and axial directions, respectively.

Piezoelectric charge constants:

These constants relate the voltage and displacement behavior of the piezoelectric material and the subscript notations indicate the transverse coupling factor (31), the longitudinal coupling factor (33), and the shear coupling factor (15).

Elastic constants, short circuit:

These constants define the material compliance, measured as the strain over the stress. The superscript notation, E, indicates that the data is measured with the electrodes connected, i.e., at a short circuit condition. The subscripts identify the transverse directions (1 and 2), the axial direction (3), and the shear axes (4, 5, and 6).

Using the manufacturer's published data, the proper ANSYS input must be computed for the piezoelectric material. This is accomplished quite easily using the PIEZMAT macro ^[5], available from ANSYS Inc. The published material data is converted by this macro into the format needed for the ANSYS model.

The 3D dielectric matrix becomes:

The 3D piezoelectric matrix:

The 3D symmetric compliance matrix:

For a two-dimensional model with the PLANE13 element type, these matrices are modified and reduced further. In the 2D system, the Y-direction is the "polarization" direction and requires a 90 degree transformation of the 3D matrices, which switches the y and z directions. The rows and columns representing "z" and "yz" terms are finally deleted from these matrices, leaving the proper input for a 2D system.

In 2D, the dielectric matrix becomes:

The 2D piezoelectric matrix reduces to:

The 2D, symmetric compliance matrix is:

One additional modification may be useful regarding the polarization direction and the 4x2 piezoelectric matrix. Often, the piezoelectric parts are assembled such that each adjacent pair has opposite polarity. This tends to increase the response of a transducer since the parts will both expand away from their common face or contract toward that face, depending on the polarity (i.e., sign) of the applied voltage. In the ANSYS material definition, this is treated by simply changing the signs of the terms in the piezoelectric matrix for a second material definition. As an example, the transducer shown in Figure 1 has four stacked piezoelectric disks. The first and third rings have identical polarity while the second and fourth rings also have identical polarity, but exactly opposite to that of the first and third rings. The two materials used to define this have exactly the same values in the dielectric matrix [e] and in the stiffness matrix [c]. However, in the piezoelectric matrix, [e], each term has a reversed sign:

FEA MODEL

The 2D axisymmetric model of the transducer shown in Figure 1 was developed for both modal and harmonic analyses. The bolt and back mass were made of steel and the horn (or front mass) was a titanium alloy. The properties of these materials are listed below.

In addition to the matrix input for the piezoelectric material, density of the PZT-8 material was defined as 7500 kg/m³.

For the linear analyses (model and harmonic solutions), the probe or drill tip is excluded from the model. Due to the impact or changing contact between the front mass and probe tube, this behavior cannot be modeled in the linear analyses. Figure 2 shows the linear model and VOLT d.o.f. constraint used for modal analyses. The electrical contacts are modeled as coupled d.o.f. sets at each interface between the piezoelectric ceramic disks. This is an appropriate treatment of these parts because the disks actually have a thin silver coating to insure excellent electrical contact.

This model ignores the insulating material, often used between the ceramic disks and the bolt shank, forbids radial sliding between the parts, and does not include the pre-compression of the stack during the assembly. Further, although transducer performance has been observed to drift slightly during operation as the ceramic warms up, temperature effects are ignored in this study.

Figure 2. Modal Analysis Model

MODAL ANALYSIS

Modal analysis of this piezoelectric transducer involved two cases which spans the extremes of the piezoelectric coupling effect on the voltage and displacement degrees of freedom. The first case is commonly called the "resonance" condition. A constant voltage of zero is applied at the electrical contacts (interfaces) of each ceramic disk. This is a condition of "short-circuit" where all voltage potentials are connected in common. The second case, called "anti-resonance", uses a common, zero voltage only at the outer face of the ceramic stack (where contact with the metal parts occurs) and at every other ceramic-to-ceramic interface. The intermediate ceramic faces have no voltage specification and this condition represents an "open-circuit".

No structural constraint was used for the modal analysis producing a simulation of an unrestrained transducer assembly. This state is similar to the physical testing where the transduced rests on the table with no restraint.

Actual measurements of the natural frequency of this transducer are made with a Hewlett-Packard 4194A Impedance/Gain Phase Analyzer. This system measures the transducer response at very small voltages over a user-selected frequency range, and graphically shows the resonance and anti-resonance frequencies, the phase angle between the input and response, and the electrical impedance of the transducer over the frequency sweep. A comparison of the resonance and anti-resonance results for the FEA model and the physical test are in excellent agreement:

HARMONIC ANALYSIS

The same 2D axisymmetric model was used for a harmonic analysis. The input for this simulation was a voltage amplitude imposed across the piezoelectric ceramic disks. The input varied sinusoidally between +/-1000 volts at the second and fourth electrical contacts (see Figure 3), while the first, third, and fifth contacts were set at zero voltage.

Harmonic Analysis Model

The harmonic analysis included a structural support on the flange of the front mass. This axial support represents a housing or case, in which the transducer is mounted on an o-ring, resulting in a very flexible support. The o-ring, "spring" support was constructed with axisymmetric solid elements, making a short cylinder with axial stiffness (AE/L) computed to match the flexibility of the o-ring. Figure 3 also shows UY coupled d.o.f. are used to attach the top of the spring to the flange on the front mass of the transducer.

The harmonic analysis was performed over a frequency range of 20-24 kHz in equal steps of 20 Hz. At each frequency, ANSYS computes the steady-state response of the system to a sinusoidally varying input, i.e., the +/- 1000 Volts on the ceramic disk stack. A constant damping ratio was assumed over all frequencies of the harmonic analysis sweep. The result of particular interest in this solution was the axial motion of the horn tip. This motion will be significant to the drilling effect of this transducer and was also the quantity measured in physical testing. Tip deflection results from the ANSYS time history postprocessor are shown in Figure 4, for two assumed values of damping ratio.

Figure 4. Harmonic Analysis

This transducer's performance was measured using the Philtec Fiber Optic Displacement Sensor, Model RC25-H3Q. This device can detect high frequency, low amplitude motions using the fiber optic sensor and displays the measured response on an oscilloscope. Sweeping the frequencies near the resonance point of the transducer, a maximum response was detected at 21.84 kHz and the peak-to-peak displacement value was 94.40x10-6 m. (3716.72 x 10 -6 in.).

The model's predicted frequency at maximum response was within 1.1% of the measured frequency at the peak response (21.84 kHz). However, the model's tip amplitude was quite sensitive to the level of damping assigned to the transducer. The harmonic analysis used a constant damping ratio which was entered as a percentage of the critical damping factor and was assumed constant over all frequencies. Values of 0, 1, and 3% of critical damping were used for this study. The results in Figure 4 and the table above show that with values of 0 and 1% of critical damping, the FEA model results bracket the measured response.

CONCLUSION

The modeling of a piezoelectric transducer was carried out with considerable success. Excellent agreement was observed with physical test measurements on the actual device. This paper also illustrated the process of converting typical manufacturer's piezoelectric data into the format required for the ANSYS model.

The comparison of the harmonic analysis results for several values of the damping ratio, showed that proper characterization of damping in this transducer is critical to the accuracy of model results. It may turn out that an alternate definition of damping could be better that the constant damping ratio assumed for this study.

This model would be appropriate to continue into further simulations of nonlinear transient behavior where the contact and impact with the drill probe could be included in the investigation.

REFERENCES

1. ANSYS Coupled-Field Analysis Guide, Release 5.5, ANSYS Inc., September 1998, pp. 3-3 though 3-6.
2. ANSYS Elements Reference, Release 5.5, ANSYS Inc., September 1998, pp. 2-33, 34.
3. "Piezoelectric Technology Data for Designers," Morgan Matroc Inc., Electro Ceramics Division., p.14.
4. "Guide to Modern Piezoelectric Ceramics," Morgan Matroc Inc., Electro Ceramics Division.
5. Personal communication with Dr. J. W. Thompson, ANSYS Inc., Customer Support Group, PIEZMAT Macro and supporting documentation, May, 25, 1999.