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.
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.
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
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
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.
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
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.
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.