The unique modular construction of both cabinets allow the non-environmentally sealed section of each cabinet (power amplifiers on RF cabinet and batteries on power cabinet) to be easily removed which reduces the width to approximately 1070 mm (42") for transportation through confined spaces (such as elevators). Due to access restrictions, only two M12 bolts at the top and two at the bottom could be used to attach the smaller power amplifier cabinet to the main portion of the RF cabinet as opposed to traditional cabinet construction, which would have used 8-10 bolts or welds for better distribution of the loads between the two cabinet sections.

Usage of a common heat exchanger in both cabinets required the power cabinet to orient the batteries vertically along one side of the cabinet. This presented a significant challenge for seismic since it drastically raised the center of gravity compared to the more traditional orientation of batteries horizontally along the bottom of a cabinet. A common mounting pattern between the cabinets with only 4 mounting points to support up to 1588 kg (3500 pounds) required thorough analysis of the mounting brackets and attachment of the brackets to the cabinet.

Importance of Seismic Simulation in Cycle Time Reduction

Seismic integrity is extremely important to cellular service providers in regions which often experience seismic activity such as the Asia Pacific and the western United States, both of which contain large numbers of cellular phone users and thus are large and important markets for Motorola cellular base stations. Wireless telephone service often continues to function normally, or can be repaired quickly, following natural disasters that typically down traditional wireline phone lines, which take months to repair.

Bellcore seismic testing which simulates an earthquake is generally the most challenging structural requirement in the design of cellular base stations. For example, the previous generation of Motorola outdoor cellular base station (cabinet originally designed by outside supplier) failed 3 times in seismic testing before finite element analysis (FEA) was used to identify areas of the cabinet that required strengthening. After using FEA to optimize the design, the cabinet passed the next seismic test.

Aggressive schedules for cellular base station development are driven by customer demand and cost reduction. The cellular base station customer base consists of relatively few large customers, so often one or two customers can drive an entire program. Project slippage can cause losses of millions of dollars due to penalty clauses in contracts or missed opportunities for large orders.

In the Motorola SC^TM4812ET program, the cost of slippage was millions of dollars per week. The usage of FEA allowed this program to ship 2 months ahead of the original schedule. Seismic FEA analysis allowed both Motorola SC^TM4812ET cabinets to pass Bellcore seismic certification testing on the first prototype pass and allowed the Motorola SC^TM4812ET power cabinet to go directly from the first prototype to pilot. A failure during seismic testing would have resulted in an estimated 8 week slippage which would have resulted in sales losses of millions of dollars.

SIMULATION REQUIREMENTS AND OBJECTIVES

Simulation Philosophy

Motorola NSS does not have any dedicated structural FEA analysts in our Fort Worth facility, thus FEA analysis has generally been limited to simple static analysis until recently. Motorola NSS physical design is currently encouraging up-front FEA analysis to simulate mechanical certification testing to reduce cycle time by eliminating testing failures. Aggressive schedules require that FEA be done quickly to allow timely inputs to the design team. The primary purpose of analysis for cellular base station products is to ensure that the design will pass the certification tests. Cellular base station products are generally designed with sufficient margin such that the accuracy of the analysis is not critical. Also, mechanical raw material cost is a small percentage of a total base station cost, so detailed analysis to optimize raw material usage is not of prime importance.

Bellcore Zone 4 Seismic Testing

The ability of a cabinet to withstand an earthquake is determined by conducting the Bellcore Earthquake Resistance Test. This Bellcore test has four levels of severity. These severity levels correspond to five geographic areas in the United States, designated Zones 0-4. Zone designations refer to earthquake risk. For Zone 0 geographic areas, no earthquake requirements are specified due to the lack of substantial earthquake risk. Zones 1-4 are based on varying levels of risk, with Zone 4 corresponding to the highest risk areas such as the California coast [1]. Since the Zone 4 test severity level is the highest, cellular infrastructure cabinets are most often certified to this level. Historically, Japanese customers have accepted Zone 4 level earthquake testing as an acceptable certification.

For Zone 4 testing, the cabinet must undergo a prescribed acceleration-time history waveform in each of its three orthogonal axes . This is accomplished by using a shaker table. The shaker table’s acceleration levels are analyzed and must meet or exceed the Zone 4 Required Response Spectrum [1]. For earthquake testing, a response spectrum is a curve that represents the maximum acceleration versus natural frequency for a single degree-of-freedom system. This curve captures the frequency and intensity content of a Bellcore Zone 4 acceleration time-history load [2]. Prior to the axis test, sine sweep surveys are conducted to determine frame-level natural frequencies. All testing is conducted per Section 5.4.1 of Bellcore GR-63-CORE [1].

Bellcore Requirements

To comply with Bellcore, the cabinet must meet the following requirements:

1. The frame-level natural frequency (first natural frequency) must be greater than 2 Hz.

2. The top of the cabinet must not deflect more than 3 inches relative to the base.

3. The cabinet must sustain the waveform without permanent mechanical or structural damage.

4. The cabinet must be electrically functional before, during, and after each earthquake event.

Additionally, Bellcore states as an objective that the cabinet should have a frame-level natural frequency of 6 Hz. A complete description of the physical and functional performance criteria is found in Section 4.4.1 of Bellcore GR-63-CORE [1].

Simulation Objectives

The primary objective of the Motorola SC^TM4812ET seismic analysis was to allow both cabinets to pass seismic certification testing on the first pass, thus preventing costly program slippage. To achieve this objective, the goal was to have first natural frequencies of 10 Hz or higher in all directions and all stresses to be below material yield strength for both fully loaded cabinets. Due to the aggressive schedule, there was a window of opportunity of only 3 weeks to complete initial seismic FEA on each of the cabinets and make recommendations to the design teams. The initial analysis indicated that the basic structure of the cabinets was sufficiently stiff, but it identified several areas which would have experienced localized yielding during seismic testing. Design changes were made to high stress areas, and the analysis was rerun quickly to evaluate the effectiveness of the changes.

SIMULATION TOOLS

Three software tools were used to conduct seismic simulation: Pro/ENGINEER^®, Pro/MESH^®, and ANSYS^®. Pro/ENGINEER^® provides parametric, feature based solid modeling with full associativity to drawing, analysis, and manufacturing modules. Pro/MESH^®, an optional module of Pro/ENGINEER^®, provides FEA preprocessing capabilities within the Pro/ENGINEER^® environment. Pro/ MESH^® allows boundary conditions and bar and mass elements to be associated to the solid model. Pro/MESH^® also provides automatic meshing of the solid model for export to an external FEA software package or solution within Pro/ENGINEER^® with optional modules and an external solver. ANSYS^® is an extensive FEA software package with capability for many types of engineering analysis. ANSYS^® is able to directly read in the mesh and boundary conditions generated by Pro/MESH^®.

Due to the lack of dedicated structural analysts at Motorola NSS Fort Worth, all mechanical design engineers are being trained to do FEA quickly with the use of Pro/ENGINEER^® and Pro/MESH^®. By using the Pro/ENGINEER^® model as the starting point for analysis and Pro/MESH^® to automatically generate the FEA mesh, model building time is significantly reduced compared to traditional FEA model building techniques. User training and expertise is also significantly reduced since Pro/MESH^® is a familiar interface to Pro/ENGINEER^® users. Model simplification can be done quickly on the Pro/ENGINEER^® solid model prior to automeshing. Since the FEA model is generated automatically from the Pro/ENGINEER^® model, the FEA model generated by Pro/MESH^® is typically more geometrically accurate than one constructed by more traditional element building methods. Pro/MESH^® is also a reliable and quick automesher [2]. Material properties and boundary conditions are also assigned within Pro/ENGINEER^® such that they are parametrically related to the solid model. Once the initial Pro/ENGINEER^® and Pro/MESH^® model are completed, design changes can be analyzed very quickly due to the parametric nature of Pro/ENGINEER^® and full associativity to the FEA model via Pro/MESH^®. Once the design change is made to the Pro/ENGINEER^® solid model, the change is reflected in the FEA model simply by remeshing the solid model with Pro/MESH^®.

Once the FEA mesh with boundary conditions has been generated from Pro/MESH^®, the actual seismic analysis is performed within ANSYS^®.

Simulation Model Building

The first step in the simulation procedure was to create a spreadsheet containing the mass and centers-of-gravity for all cabinet components. If component masses were unknown, preliminary Pro/ENGINEER^® models were used to determine the mass properties. From the spreadsheet, a total mass and frame-level center-of-gravity was computed. This spreadsheet provided for a consistency check with ANSYS^®’ total mass and center-of-gravity calculations.

The second step was to build simulation models for each cabinet. Simplified solid models of the actual part models were built in Pro/ENGINEER^®. The actual cabinet database was not used for two reasons. First, the cabinet database wasn’t complete; the analysis phase was conducted in parallel with the design phase. Second, actual cabinet part databases contain design features which complicate part meshes and are not structurally significant. Both cabinets were fabricated out of sheet metal of various thicknesses, with 1/8" being the thickness of the outer skin. Therefore, simple thin-walled structures were used to simulate cabinet components.

Meshing, Preprocessing the Simulation Model

All meshing and preprocessing was conducted in the Pro/ENGINEER^® environment using Pro/MESH^®. Shell elements were used to model all sheet metal parts, including structural members such as vertical stiffeners, mounting rails, etc. No solid elements were used. Using the ANSYS^® Shell63 element, an elastic shell element with four nodes [3], Pro/MESH^® automatically generated the element mesh from the Pro/ENGINEER^® model. Bolts and fasteners in the cabinets were simulated using beam elements. The majority of welds were also modeled using beam elements. Some welded and riveted pieces were simulated using variable thickness shells, a technique which saves time but sometimes results in a liberally stiff structure. Variable thickness shells were used only where appropriate (i.e. where so many welds or rivets were used that the two pieces could be structurally considered as one).

Card cages and other electronic equipment were simulated using mass elements, which are point elements having six degrees of freedom (translation and rotation), mass, and mass moment of inertia properties [3]. The mass elements were applied at datum points located at the component centers-of-gravity, and were tied into the cabinet frame using massless, rigid beams. The rigid beams were installed in such a manner as to prevent artificial stiffening of the cabinet.

The only loads applied to the model were displacement boundary conditions at the cabinet mounting locations. The cabinets are mounted with 12 mm anchor bolts using 51 mm (2") washers. Therefore, a 25 mm (1") diameter circle concentric with the anchor bolt centerline was fixed in all translation and rotation directions at all four mounting points. Fixing the entire mounting bracket and/or the cabinet base is unrealistic due to irregularities of outdoor concrete mounting pads and rooftop installation sites. No forces were applied to the model since the response spectrum analysis determines the accelerations experienced by the cabinet model based on the modal analysis results.

The automatic meshing feature of Pro/MESH^® greatly reduced the mesh generation time and user expertise requirements. The simplified RF cabinet model with mass nodes and beam elements is shown in Figure 2. The RF cabinet mesh is shown in Figure 3. Both cabinet models had approximately 26,000 elements: 30-40 Mass21 elements, 200-400 Beam44 elements, and 25,560-25,770 Shell63 elements. All mesh and preprocessing information was outputted from the Pro/ENGINEER^® environment for solution in ANSYS^®.

Figure 2. RF CABINET SIMULATION MODEL WITH BEAM ELEMENTS
AND MASS NODES SHOWN

Figure 3. RF CABINET MESH

Modal Analysis

Using the mesh and preprocessing information from Pro/MESH^®, a modal analysis was conducted using ANSYS^®. Modal analysis consisted of solving for the cabinet-level front-to-back and side-to-side mode shapes and natural frequencies. If the first mode extracted was not cabinet-level and limited to a section of the model, the finite element model was modified in the Pro/ENGINEER^® environment to stiffen the components and members. If applicable, the stiffening modifications were discussed with the designers to determine equivalent design changes to the actual cabinet database. Modal analysis was then repeated until the first mode extracted had a cabinet-level mode shape (front-to-back for both cabinets) and the second cabinet-level mode shape was also extracted (side-to-side).

Response Spectrum Analysis

After extracting the cabinet-level modes, a Bellcore Zone 4 response spectrum analysis was conducted in ANSYS^®. During the response spectrum analysis, the maximum response of each distinct mode is combined to produce an estimate of the maximum displacement response [4]. Typically, the first cabinet-level mode accounts for the greatest percentage of the total response.

Response spectrum analyses were conducted on both cabinet models in both the front-to-back and side-to-side directions. The response spectrum input corresponded to the Bellcore Zone 4 Response Spectrum as shown in Table 1. Displacement and stress results were viewed in the ANSYS^® postprocessor. As expected, the majority of the stress concentrations were located at the mounting brackets. Due to its larger weight, several mounting bracket designs were evaluated with the power cabinet model. The reaction forces at the fixed locations were added to predict the total tensile and shear loading on the mounting bolts.

As a result of the response spectrum analysis, the following was completed: the mounting brackets were quantified and sized, restraining screws were added to heavy components, additional structural members were added, and the anchor bolts were sized.

Both cabinets’ response spectrum results indicated that the cabinet would pass the Bellcore Zone 4 Earthquake Resistance Test.

EXPERIMENTAL TESTING SUMMARY

Experimental correlation of the simulation results was conducted during the scheduled mechanical certification testing of both the RF and Power cabinet products. During the testing, the primary goal was the completion of the tests on schedule, and not the correlation of the simulations. No tests were repeated for the sole purpose of correlation.

Each cabinet, installed onto concrete pads with anchor bolts per field installation, was mounted onto a shaker table for testing. The experimental testing consisted of sine sweeps to establish the cabinet vibration characteristics (determine natural frequencies) and earthquake qualification tests in all three axes (front-to-back, side-to-side, and up-and-down). The following measurements were taken for comparison with the simulation results for both the front-to-back and side-to-side axis earthquake events:

1. Natural frequencies

2. Cabinet top displacement

3. Mounting bracket strain

4. Cabinet wall strain

For both cabinets, two strain gages were located at the back left corner of the frame. For both cabinets, the front-to-back natural frequency and earthquake test was conducted before the side-to-side tests.

The RF cabinet testing was uneventful for all three axes. Upon completion of the testing, no structural damage was observed and the cabinet complied with all Bellcore requirements and objectives.

For the Power cabinet earthquake testing, during the front-to-back drive axis, the rocking momentum of the battery-loaded cabinet overcame the friction forces at the two back mounting bracket/cabinet interfaces. This interface consisted of two M12 bolts torqued to 55 ft-lb. Once the friction forces were overcome and the cabinet became loose, the cabinet moved relative to the bracket, with the M12 bolts being pulled up until striking the tops of the slots into which they had been inserted. This occurred repeatedly, with the cabinet gaining more momentum as the test progressed. This physical response greatly contributed to the maximum displacement measured and reduced the cabinet stiffness considerably. However, upon conclusion of the earthquake test in each axis, no permanent structural damage was observed and the cabinet complied with Bellcore requirements and objectives.

Although the Power cabinet passed the Bellcore test, further testing of the M12 bolts was conducted to experimentally determine the maximum allowable torque to be specified in the bolts’ installation. As a result, the specified torque was increased to prevent movement of the cabinet during a seismic event.

CORRELATON RESULTS AND DISCUSSION

Pre- and Post-Test Simulations

Simulations were conducted before and after the experimental testing. There were two reasons for repeating simulations:

1. For the Power cabinet, the experimental cabinet was 480 lb. heavier than the pre-test simulation model because heavier batteries were used in the testing.

2. For the RF cabinet, the experimental displacement results were higher than the pre-test simulation model results.

In regard to reason 1, the original weight of the 24 batteries used in the pre-test simulations was 85 lb. each. However, for the experimental testing, different batteries were used with a weight of 105 lb. each. Therefore, the mass of each battery mass node was increased by 20 lb., adding 480 lb. total to the post-test simulation model.

In regard to reason 2, DRD Technology Corporation, the ANSYS^® software distributor, suggested the following modifications:

1. Remove mass moment of inertia properties from the mass elements.

2. Rotate all nodal coordinate systems to the active coordinate system.

By specifying mass moments of inertia and using rigid beams to tie the mass elements to the cabinet frame, rotational resistance was unrealistically increased. In regard to coordinate rotation, the output file created by Pro/MESH^® specified rotations on specific nodes, affecting displacement results.

Pre- and Post Test Simulation Comparison Results

For the natural frequency and displacement results, both pre- and post-test results are given. For the RF cabinet, removing mass moment of inertia properties from the mass nodes resulted in a 12-17% increase in natural frequencies and a 30% increase in maximum displacement. Rotating all nodal coordinate systems to the active coordinate system resulted in an additional displacement increase of 60%.

For the Power cabinet, the addition of 480 lb. to the total weight of the system contributed to lowering the simulated front-to-back natural frequency by 30% and increasing the displacement by 300%. The effects of the 480 lb. weight addition, removal of mass moments of inertia, and nodal rotation were not isolated on the Power cabinet model. However, the RF cabinet effects results indicate that the weight increase was the primary contributor to the Power cabinet natural frequency decrease and displacement increase.

For the remainder of the results discussion, only the post-test simulation results will be compared to the experimental measurements.

RF Cabinet Natural Frequencies

The RF cabinet modal analysis results are shown in Table 2 and plotted in Figure 4. Only the first natural frequencies were measured because the Bellcore test specification [1] requires only a first natural frequency measurement for each test axis. This is because earthquake acceleration levels are largest at lower natural frequencies (see Table 1). The simulated natural frequencies correlate extremely well with errors of 0% and 6% for the front-to-back and side-to-side mode shapes, respectively. The front-to-back and side-to-side mode shapes are shown in Figures 5 and 6.

Table 2. RF Cabinet Natural Frequencies (Hz)

Figure 10. POWER CABINET NATURAL FREQUENCIES

Power Cabinet Displacement

For the power cabinet, correlation between the simulated and measured results is invalid. The divergence between the simulation and experimentation displacement values was exacerbated by the cabinet’s response to the earthquake event in the front-to-back direction. Therefore, the front-to-back displacement correlation error would be much higher than the equivalent RF cabinet displacement error and misleading in regard to the validity of the modeling techniques. Displacement results between the simulation and test are also incomparable in the side-to-side direction due to the previously mentioned weakening effect.

Power Cabinet Strain Measurements

The Power cabinet strain results are shown in Table 7 and Figure 11. For the font-to-back direction, the differences between the vertical and horizontal mounting bracket strains and the measurements are 20 and 30%, respectively. For the cabinet wall, the simulated and measured strain values are incomparable due to the cabinet becoming loose relative to the mounting brackets during the test, inducing extremely high strain in comparison to the simulation results. For the side-to-side direction, a comparison between the simulated and measured strain values is also not valid due to the previously mentioned weakening effect.

TABLE 7 POWER CABINET FRONT-TO-BACK MICROSTRAIN

Location and Direction	Simulation	Experimental Measurement
Mounting Bracket Horizontal	700	535
Mounting Bracket Vertical	1500	1895

Figure 11. POWER CABINET STRAIN FRONT-TO-BACK AXIS

CONCLUSIONS

ACKNOWLEDGEMENTS

The authors would like to thank Ken Huang, Roger Gandee, and John Dascanio of Motorola and Chris Andersen and Andy Bax of DRD Technology Corporation for their support and encouragement in this endeavor.

REFERENCES

1. Bellcore, GR-63-CORE "Network Equipment-Building System (NEBS) Requirements: Physical Protection," Issue 1, 1995.

2. Bax, A. and Andersen, C., "Bellcore Seismic Analysis Calls on ANSYS^®," Analysis Solutions, Spring 1998.

3. ANSYS^® Inc., ANSYS^® Help System, Revision 5.4, 1997.

4. Cook, R.D., Finite Element Modeling for Stress Analysis, John Wiley and Sons, New York, 1995.

5. DRD Technology Corporation, Advanced ANSYS^®/ProFEA: Finite Element Analysis for Pro/ENGINEER^®, Revision 2, 1997.