DYNAMIC SHOCK SIMULATION OF A COMPUTER HARD DRIVE USING AN ANSYS/LS-DYNA IMPLICIT-EXPLICIT SEQUENTIAL SOLUTION

Chris Andersen
DRD Technology Corporation

John Stricklin
Seagate Technology

ABSTRACT

This paper describes a nonlinear transient dynamic analysis of a computer hard drive using ANSYS in combination with ANSYS/LS-DYNA. The model includes the enclosure, platters, spindle, read/write heads, and other key components. The objective of the analysis was to determine the interaction between the parts in this assembly, such as lift off and impact between the read/write heads and platters, when the hard drive is subjected to a 250 G half sinusoid shock load. This load simulates a shock test, which the manufacturer does to qualify hard drives.

An important aspect of this work was to use SDRC geometry effectively to create the finite element model. The process included using Pro/ENGINEER mid-plane extraction functionality in addition to ANSYS finite element modeling capabilities.

ANSYS/LS-DYNA provided an environment to perform many different aspects of this analysis in a highly productive and efficient manner. The analysis included standard ANSYS normal modes and static nonlinear analysis in addition to an implicit-explicit sequential solution to preload the read/write heads and explicit dynamics analysis.

Severe hourglassing was one of the most difficult problems encountered in this analysis, and this problem was resolved using standard techniques in addition to use of an LS-DYNA 3D fully integrated shell element, which is not officially supported in ANSYS/LS-DYNA.

The model correlated well with experimental results. This analysis demonstrates a cost effective procedure and tool for analysis based design of hard drives to withstand shock.

INTRODUCTION

Computer hard drives must be able to withstand shock loads such as those related to accidentally dropping the computer in which the hard drive is installed. Seagate employs an extensive test procedure to ensure that its hard drives are able to survive shock loads. One of these tests is to subject the hard drive to sinusoid shock pulses.

In hard drives such as the one modeled, the hard drive is assembled so that the read/write heads press against the platters with a preload. It is desirable for the preload to be sufficient to keep the head pressed against the platter during shock. Under severe loads the read/write head can lift off of platter and then slap back down on the platter. This bounce can damage the surface of the platter, which can result in loss of data and damage to the platter.

This analysis is used to determine whether or not this bounce occurs and the magnitude of the contact loads.

 

GEOMETRY

Seagate uses the SDRC CAD system. Since DRD does not have SDRC, Seagate provided most of the hard drive geometry to DRD in the form of SDRC IGES files. Although IGES files can be read directly into ANSYS, DRD read the IGES files into Pro/ENGINEER in order to utilize Pro/ENGINEER’s mid-plane extraction capability to generate surfaces that could easily be meshed in ANSYS using shell elements. Figures 1 and 2 show the geometry in Pro/ENGINEER immediately after reading the SDRC IGES files. Figure 1 shows the hard drive including the enclosure, which is illustrated as translucent. Figure 2 shows the hard drive without the enclosure.


Figure 3 provides a cut away view of the hard drive.


Since the structural components were modeled using shell elements, the geometry in Pro/ENGINEER was converted to mid-planes and written to an IGES file using Pro/ENGINEER’s Pro/MESH module. Then the IGES file was read into ANSYS.

Figure 4 shows the ANSYS solid model, which was created from Pro/ENGINEER IGES files, including labeled components.


The actual hard drive enclosure had fairly complex geometry. Since the enclosure is only of interest in this analysis as a boundary condition for the hard drive, the enclosure was represented as a simple hollow box as shown in Figure 5. The enclosure’s stiffness and mass were adjusted to ensure that the simplified enclosure represents the actual enclosure stiffness and mass with sufficient accuracy. DRD selected an enclosure thickness and set of material properties that result in a fundamental natural frequency for the entire system in the 500-600 Hz range, as Seagate measured for an actual hard drive and enclosure. The model produces a fundamental natural frequency of approximately 600 Hz for the enclosure, which was determined through an ANSYS normal modes analysis.


Figure 5 shows the attach locations for the platter axis, E block axis and the magnet housing to the enclosure.

The primary hard drive structural components were meshed with 4 node quadrilateral shell elements. Figures 6 and 7 show the finite element mesh of the enclosure and hard drive, respectively.


The magnet housing is important to the model in that it contributes significant mass to the enclosure. It is modeled as a lumped mass, which is connected to the top and bottom faces of the enclosure. Figure 8 illustrates the magnet housing model. The ANSYS /ESHAPE utility is used so that the beam and shell elements in this paper look like 3D solids.

The E block and spindle axles and their bearings are important in that they connect the E block and spindle to the enclosure, and, therefore, affect the dynamic behavior of the system. The axles and bearings are modeled using 3D beam finite elements, whose stiffnesses were measured by Seagate and provided to DRD. Seagate also provided to DRD the orientation of the bearings with respect to the axles. Figure 9 shows a typical axle and bearing assembly.

 


The load springs connect the read/write heads to the E block. The load springs deflect when the hard drive is assembled and the read/write heads are pressed against the platters. Since lift off of the read/write heads from the platters is a critical aspect of this analysis, the load springs were modeled in detail. Figure 10 shows a single load spring.


The load springs have ridges along their edges, which provide significant additional stiffness. If the ridges were modeled as shell elements, their tiny dimensions would force the ANSYS/LS-DYNA explicit solver to use much smaller time steps than would otherwise be needed. To avoid these small time steps, these stiffening edges were modeled using 3D beam elements. Since these beams are located in the plane of shell elements that represent the load springs, the beam stiffnesses were adjusted so that the load springs have the overall correct stiffness and account for the actual location of the ridges with respect to the plane of the shell elements.

 

LOADS AND BOUNDARY CONDITIONS FOR THE ANSYS IMPLICIT MODEL

After creating and fine tuning the finite element as previously described, the model was run in ANSYS as a nonlinear static implicit analysis with large deflection effects in order to pre-load the load springs and put them at their correct position. Each corner of the bottom surface of the enclosure was constrained. In addition, a displacement constraint was applied to each read/write head in the direction perpendicular to the surface of the platters to position each read/write head on the appropriate platter surface. Figure 11 shows the displaced shape of a typical load spring. The /ESHAPE graphic option is used in Figure 11 to display shell and beam element thicknesses. The /ESHAPE utility was very useful in locating the read/write head precisely where it needed to be.

LOADS AND BOUNDARY CONDITIONS FOR ANSYS/LS-DYNA EXPLICIT MODELS

As in the ANSYS implicit model, each corner of the bottom surface of the enclosure was constrained. In addition, displacement constraints on the read/write head were removed so that the LS-DYNA 3D nonlinear contact algorithm was able to simulate interaction between the load springs, and platters as well as between the E-block arms and platters.

Next, the ANSYS/LS-DYNA implicit-explicit sequential solution scheme was used to initialize the LS-DYNA 3D model using the implicit static ANSYS results for the load spring pre-load. This process is easy and highly automated using ANSYS/LS-DYNA.

Inertial loads corresponding to a 1 ms 250-G half-sinusoid downward acceleration were applied to the model to simulate the shock load. The entire simulation lasted 5 ms. The model was first allowed to 'settle' for .5 ms to facilitate a transition from the displacement constraints on the read/write heads in the implicit model to the nonlinear contact used to simulate read/write head, load spring, and platter interaction in the explicit model. Next, a 1 ms half-sinusoid downward acceleration was applied to the corners of the enclosure. Finally, the model was allowed to vibrate freely for the remaining 3.5 ms of simulation time. Figure 12 illustrates the entire 5 ms base acceleration time history.


LS-DYNA 3D's automatic surface to surface (ASTS) contact algorithm was used to model nonlinear contact between the E-block arms and platters, and between the load spring-read/write head assemblies and platters. LS-DYNA 3D offers several contact algorithms. We chose automatic surface to surface contact over several other algorithms because it allows postprocessing of contact forces for each contact pair, automatically accounts for shell thickness, and has no problems dealing with the 3rd node of each beam element used to orient the beam cross sections.

 

IMPLICIT-EXPLICIT MODEL CONVERSION

ANSYS/LS-DYNA automates conversion of the ANSYS implicit models used to pre-load the model to the LS-DYNA 3D explicit model. ANSYS/LS-DYNA automatically converts the implicit Shell 181 elements to explicit Shell 163 elements. It also converts implicit Beam 4 elements to explicit Beam 161 elements. Finally, ANSYS/LS-DYNA converts the implicit Mass 21 lumped mass elements to explicit Mass 166 lumped mass elements. Since LS-DYNA 3D requires a third node to orient all beam 161 finite elements, we used the third node option for the implicit Beam 4 elements in order to have identical node sets for the implicit and explicit models.

After performing the implicit analysis, redefinition of the shell and beam real constants was required for the explicit analysis. This was necessary because ANSYS and LS-DYNA 3D require specification of real constants in different orders. The actual values of the real constants are the same. For example, the implicit Shell 181 element uses the first real constant as thickness while the explicit Shell 163 element uses the third real constant as thickness. In addition a shear factor of 5/6 is defined for the explicit shell elements.

ANSYS/LS-DYNA 3D supports 11 different formulations for the LS-DYNA 3D explicit shell element. The default formulation, called Belytschko-Tsay, was used for most of the shell elements in the model. Due to hourglass energy problems, the LS-DYNA 3D fully integrated shell formulation was used to model the load springs and read/write heads. This element is referred to as TYPE 16 in LS-DYNA 3D. ANSYS/LS-DYNA 3D does not officially support the LS-DYNA 3D fully integrated shell element, so it was necessary to manually edit the file.k file created by ANSYS/LS-DYNA 3D before initiating the LS-DYNA 3D solution. Since the LS-DYNA 3D fully integrated shell element is not officially supported, it is not currently possible to postprocess stresses for this element using ANSYS. The postprocessor LS-POST from LSTC, the developer of LS-DYNA 3D may be used to postprocess stresses for the fully integrated shell elements. This was, however, not required for this project because stresses in the load springs and read/write heads were not the objective.

The ANSYS/LS-DYNA implicit-explicit sequential solution scheme was employed to initialize the LS-DYNA 3D solution while using the ANSYS implicit nonlinear static solution for initial conditions. In order to avoid numerical problems resulting from this stress initialization procedure, the birth time option for the LS-DYNA 3D contact algorithm was used so that the nonlinear contact was not active until the stress initialization procedure is complete.

 

EXPLICIT MODEL DAMPING AND HOURGLASS CONTROLS

Both stiffness (BETA) and mass (ALPHA) damping were used in the LS-DYNA 3D model. LS-DYNA 3D currently has a limitation that the BETA damping coefficient must be smaller than the model time steps. Since the model time steps are approximately 5e-10 seconds, we applied a BETA damping coefficient equal to 1e-10 to all materials. We also applied an ALPHA damping coefficient equal to 94 to all materials, which corresponds to 3% damping at 250 Hz.

The Flanagan-Beyltschko stiffness form of hourglass control with a coefficient of .03 is used to minimize hourglass energy for all materials in the model. The actual command used is edmp,hgls,i,5,.03, where i is the material ID.

 

ANALYSIS RESULTS

Figure 13 shows the displaced shape of the E-block, load springs, read/write heads and platters at 2.35 ms into the simulation. Lift off of some of the read/write heads from the platters is evident in Figure 13. In addition, Figure 13 indicates that load springs and read/write heads in between platters may collide with one another, although collision between these parts was not anticipated, and was, therefore, not modeled.

Figure 13. Displaced Shape of Model at 2.35 ms

 


The time-varying behavior of the model is best depicted using animation in combination with time-history graphs of key analysis results. It should be noted that the ability to plot the model results with element thickness turned on using the /ESHAPE utility was extremely useful in postprocessing this model’s results. This is a significant advantage of using ANSYS/LS-DYNA for LS-DYNA 3D models. Unfortunately, ANSYS/LS-DYNA 3D does not support the thickness representation of the Explicit161 beam elements, so the load spring stiffening ridges are not visible as 3D solids when postprocessing.

Figures 14, 15, and 16 show the contact forces as a function of time between various components in the model. Figure 14 shows contact forces between the top E-block arm and top platter, and indicates that these components collide once during the simulation. Figure 15 shows contact forces between the top load spring-read/write head assembly and top platter, and shows 4 distinct bounces. Figure 16 shows the contact forces between the second load spring-read/write head assembly and top platter, and also shows 4 distinct bounces.


CONCLUSIONS

This finite element model predicts that the hard drive read/write heads will lift off of the platters and then strike them when subjected to a 250 G 1 ms half sinusoid shock load. Seagate has observed that the actual hard drive exhibits similar behavior, and has concluded that this model appears to accurately predict the hard drive read/write head behavior when the drive is subjected to shock loads.

This analysis demonstrates an accurate and cost effective method for subjecting hard drive designs to shock tests using finite element model prototypes. This analysis method provides Seagate with a tool for testing hard drives for shock before committing to expensive physical prototypes. It also provides Seagate the opportunity to bring new hard drives to market faster. Since finite element models can be inexpensively modified and run again, this analysis method also provides Seagate with the opportunity to optimize hard drive designs to withstand shock.