Vibration Analysis of the Base Structure Supporting a Centrifuge–Motor Assembly in a Petroleum Oil Refinery

A structure carrying a centrifuge and motor in a petroleum oil refinery has been vibrating above the alarm limit of vibration. This has been a recurring problem. The maintenance work undertaken at regular intervals on the basis of time waveform and spectrum analysis could provide only a temporary solution. To investigate the causes of vibration above the acceptable limits, pre-stressed modal analysis of the structure was undertaken by using Finite Element Analysis software ANSYS™ and natural frequencies and mode shapes were extracted. Pre-stressing was done by considering the self-weight of the structure, centrifuge and motor. The structure was analyzed using a combination of beam elements, shell elements and mass elements. The operating deflection shape (ODS) technique which helps to observe the deflection pattern of structure in real time at operating or other frequencies from the measured vibration data was employed to validate the analytical results. ME’scopeVES™ software employing the ODS technique was used in this work. Analytical results obtained from ANSYS™ software are compared well with the ODS test results. The analysis of analytical and experimental results has revealed that the structure was operating in the resonance band.


Introduction
A centrifuge is a machine, generally driven by a motor, with a rapidly rotating container that applies very high centrifugal force to its contents, used mainly to separate solids from liquids. In refineries, it can be used for the effective separation of slurries into liquid and solid phases, with the application of very high centrifugal force. Analysts often encounter failures that seemingly provide no clue as to the reasons for failure while carrying out routine vibration analysis and root cause analysis. The analyst needs to look for other methods of detecting problems when conventional signature (FFT and time waveform) analysis does not help in detecting the problem. One such method that can be used very effectively is operating deflection shape (ODS) analysis. ODS [1] is defined as the deflection of a structure at a particular frequency. ODS data are acquired with the machine operating, and it represents the motion due to a combination of structural resonances and operational forces. It can be accomplished with a single-channel data collector using peak and phase measurements from a tachometer to animate multiples of running speed. Devriendt [2] demonstrated how ODS can be presented using the parameters obtained from transmissibility tests. Heaton and Hewitt [3] performed the ODS analysis of sanders and polishers and established the most appropriate mounting location for the transducers to evaluate the greatest risk of vibration exposure. Ganeriwala [4] investigated the effects of shaft misalignment of rotating machinery on its ODS. In this method, an ODS obtained from multiple accelerometer signals collected at various points on the machine was used to determine shaft misalignment.
Few researchers have performed modal analysis using numerical studies but have not validated their results with experimental studies. Dhakan and Chalil [5] optimized the casing design with a weight reduction of around 12% by performing structural analysis using ANSYS. The vibration behavior of the casing was analyzed using modal analysis and ensured that the natural frequency of vibration of the casing was well above the operating frequency of the turbine limit. Lu et al. [6] determined the natural frequency by performing modal analysis which was essential to optimize the design structure of the crossbeam and bed. This would avoid the region of sympathetic vibrations effectively and guarantee the processing precision of the special-shaped stone multifunction NC machining center. Jiang et al. [7] performed the structure topology optimization of the motor base by using FEA. The natural frequency obtained by modal analysis and operating frequency were compared, and it was found that the structural optimization meets the stability performance. Qiu et al. [8] investigated the effects of changes in boundary conditions and variation of thickness on the natural frequency of the motor base. It was found that constraining all the four sides resulted in the highest natural frequency. The natural frequency was found to increase with the increase in the thickness of the plates.
Although the discussions above have primarily concentrated on the evaluation of modal parameters through numerical investigations, it might also be required to validate the results against experimental findings to confirm the accuracy of the solution. Andren et al. [9] investigated the dynamics of a clamped boring bar using a Euler-Bernoulli beam model, an experimental modal analysis and an ODS analysis. The results indicate a close agreement between the deflection shapes and mode shapes produced by the three different analytical methods. Ribeiro et al. [10] experimentally calibrated a three-dimensional finite element model of a train based on modal parameters. The numerical model significantly improved when experimental and numerical responses were compared before and after calibration, and there was a strong correlation between the results of the calibrated model and the experimental findings. Jamil et al. [11] established a method to determine the natural frequency of machine tool components to improve the conditions during the cutting process on the machine tool. The modal parameters obtained through FEA were verified and corrected by an experimental modal test. Pedrammehr et al. [12] determined the natural frequencies and vibration mode shapes of the model by carrying out modal analysis in ANSYS Workbench. The modal testing was performed on the structure, and the natural frequencies extracted through ME'scope were compared with the results of the modal analysis. Pakzad et al. [13] examined the dynamic behavior and modal parameters of a machine tool structure. The natural frequencies and mode shapes obtained by performing modal analysis were compared with natural frequencies extracted using ME'scope software. Patwari et al. [14] performed experimental modal testing and modal analysis for evaluation of the structural dynamics of a vertical machining center. The results of the modal analysis were compared with natural frequencies and the mode shapes obtained by modal testing of the machine components. Prasad and Singh [15] performed an experimental modal analysis to determine the looseness in the stator windings by examining the ODS. The modal parameters obtained by experimental modal analysis are validated with the findings of theoretical and finite element studies.
In the present work, modal analysis using FEM is performed to determine the natural frequencies and mode shapes of a structure. The structure is diagnosed by comparing these modal parameters with the ODS data and appropriate recommendations are made.

Problem Definition
In a petroleum oil refinery, the base structure which is supporting the centrifuge and motor as shown in Fig. 1 was subjected to a very high magnitude of vibration. The  Table 1.
The velocity of vibrations measured on the base structure was about 10.65 mms −1 as on December 17, 2007. This is above the vibration limit of 7.1 mm −1 shown by line AB in Fig. 2 in SKF Machine Analyst software at the operating speed [16]. Hence, it was proposed to undertake this study to identify the causes of abnormal vibration. The natural frequencies and mode shapes (modal parameters) of the structure are determined by performing modal analysis using ANSYS. The structure is diagnosed by comparing the experimental ODS results and analytical results.

Analytical Method Finite Element Modeling
The natural frequencies and mode shapes of the base structure determined by performing modal analysis using ANSYS are compared with the experimental ODS test data, and the base structure is diagnosed. The FEA software ANSYS™ is employed to analyze the base structure of centrifuge-motor assembly. Static analysis is carried out by considering the pre-stress effects caused by the self-weight of the structure and the weight of the centrifuge and motor. Pre-stressed modal analysis is carried out to determine the modal parameters of the base structure. Figure 3 represents the top view of the base structure of centrifuge-motor assembly.
The geometry details of part 1 of the base structure [17] are shown in Fig. 4 and Table 2. Parts 2, 3 and 4 are plates of rectangular cross section. The material for base structure is structural steel Fe410W A with properties as listed in Table 3.
The properties specified in Table 3 are added to the database to simulate material behavior of the structure. The geometry of the structure is created by defining key points and lines. It is discretized to obtain the finite element model with 324 beam elements, 1895 shell elements and 8 mass elements. Figure 5 shows the base structure with boundary conditions.
The base structure supporting the centrifuge-motor assembly is comprised of C-channels and supporting plates of different thicknesses. Beam 44 elements [18] are used to model C-channels. It has 6 degrees of freedom at each node: translations in the nodal x, y and z directions and rotations about the nodal x-, y-and z-axes. Shell 181 elements are used to model the supporting plates. It is a 4-node element with 6 degrees of freedom at each node: translations in the x, y and z directions and rotations about the x-, y-and z-axes. Mass 21 elements are used to represent the masses of centrifuge and motor. It is a point element having up to 6 degrees of freedom: translations in the nodal x, y and z directions and rotations about the nodal x-, y-and z-axes. The masses of the centrifuge and motor are represented by mass elements at nodes A1, A2, A3, A4 and A5, A6, A7, A8, respectively, i.e., at locations corresponding to the bolt positions as indicated in Fig. 5. The inertia load is applied by considering gravitational acceleration, g = 9.81 ms −2 . The base structure is rigidly fixed to the foundation by means of bolts at seven locations as indicated by the nodes B1, B2, B3, B4, B5, B6 and B7 in Fig. 5. Hence, all the DOFs of the base structure at these nodes are constrained.

Static Analysis
Static analysis is carried out to facilitate the subsequent modal analysis of the pre-stressed base structure. It is necessary to consider the stress state of the base structure due to the loads acting on it. Hence, the stress stiffening due to    its stress state is considered. The stress stiffening matrix is internally computed by the software and adds to the original stiffness matrix. The maximum von Mises stress of 47 MPa is observed at location AP as shown in Fig. 6.

Mesh Convergence Study
Mesh convergence study was carried out to determine the optimum number and size of the elements necessary in a model to confirm that the results of an analysis are independent of these factors. Figure 7 shows the findings of the mesh convergence study. The appropriate number of elements obtained by the mesh convergence study (2227 elements) was utilized for further analysis.

Modal Analysis
Pre-stressed modal analysis using the block Lanczos method in ANSYS™ is carried out to determine the undamped natural frequencies and mode shapes of the base structure. QR damped method in ANSYS™ is used to determine the damped natural frequencies based on the values of Rayleigh damping coefficients. Rayleigh damping coefficients α and β are computed as follows: Rayleigh damping [C] can be written [17]

in terms of [M] and [K],
According to tests [19] conducted on mild steel specimens, ζ 1 ω 1 = 2.0 and ζ 3 ω 3 = 3.2, where ω 1 and ω 3 are the first and third undamped natural frequencies. Using the are mass and stiffness matrices.   natural frequencies for first and third modes obtained through analysis, the Rayleigh damping coefficients α and β are evaluated as 3.853 s −1 and 0.0000377 s, respectively. These values are input in ANSYS™ to determine damped natural frequencies (Table 4) using the QR damped method. Figure 8 corresponds to the first bending mode (y-z plane) in the left channel supporting the centrifuge. Figure 9 corresponds to the coupling of the first bending (x-z plane) and twisting modes in the left channel supporting the centrifuge. Figure 10 corresponds to the coupling of the first bending (y-z plane) and twisting modes in the left channel supporting the centrifuge. Figure 11 corresponds to the coupling of second bending (y-z plane) and twisting modes in the left channel supporting the centrifuge. Overall, it can be observed from the mode shapes (modes 1-4) that the left channel is subjected to greater amount of deflection compared to the remaining parts of the base structure.

Experimental Method Experimental Setup
The real-time dynamic behavior of structure is obtained through the ODS technique in ME'scopeVES™ software [20]. The vibration data are measured using the SKF Microlog Analyzer (CMVA 60) with a frequency range of 0.5 Hz to 20 kHz. The line model of the test structure is modeled in ME'scopeVES™ as shown in Fig. 12. Test points are points (DOFs) where vibration data are to be acquired on the real structure. The location of test points can be determined by understanding the way in which the base structure is vibrating. The real continuous structures have an infinite number of DOFs and an infinite number of modes. By having more number of measurements on the base structure, more definitions can be given to its ODS. Based on the desired frequency range of 24-70 Hz, 32 test points are created and route is downloaded to data acquisition device. The corresponding points are marked on the test structure at the site. Vibration data are acquired by attaching the accelerometer to the surface of the test structure at respective points and directions individually. To establish a speed reference, an optical phase reference kit and a reflective tape are utilized. A small size reflective tape is pasted on the shaft and taken as phase reference. An optical sensor is mounted on the moveable arm of the magnetic holder such that light from it falls on the reflective tape. At the start of every revolution, the reflection of light from reflective tape is detected by the sensor which sends a signal to the analyzer. Thus, data are acquired on all degrees of freedom on the test structure at the start of a revolution each time when the accelerometer is attached to the surface of the structure and the button is pressed to collect data.
The time waveforms were evaluated by calculating the inverse of the Fourier spectrums contained in the data block. From the available time domain data, one of the measurements was taken as reference. The reference corresponds to the points where significant level of vibration is observed on the structure. The reference DOFs were chosen in the x, y and z directions, respectively. Reference DOFs were chosen and mentioned as: 6X:32Y:2Z. Roving DOFs were mentioned as 3X (without colons). Auto-spectrum of each roving response and the crossspectrum between each roving response and the reference response were calculated. Each ODS FRF was then calculated by combining auto-spectrum of each roving response with the phase of the cross-spectrum between the roving response and a reference response. The deflection patterns at frequencies corresponding to high amplitude of vibration were observed. The vibration data stored in the analyzer were uploaded to the ME'scopeVES™ software which was stored as a separate file called as data block file. In order to animate shapes from the data block file, each measurement in the data block was assigned to a point and direction of the model. The software then calculates the magnitude and phase at each point through animation equations for measured and unmeasured points on the model. The deflection patterns at frequencies corresponding to high amplitude of vibration were observed.

Results and Discussion
From the spectrum plots shown in Fig. 13, it can be seen that there is high amplitude of vibration at frequencies 24.36 Hz and 46.39 Hz, which correspond to the operating frequencies of the motor and centrifuge, respectively. From Figs. 13 and 14, it can be seen that the maximum amplitude of vibration is 4.429 mms −1 RMS at point 1 on the left channel supporting the centrifuge in the Z direction (Figs. 11 and 12). From Figs. 12 and 13 it can also be seen that the maximum amplitude of vibration is 10.56 mms −1 RMS at point 5 on the left channel supporting centrifuge in the Z direction (Figs. 11 and 12) which is crossing the alarm limit (7.1 mms −1 ). The excitation frequencies at which maximum amplitude of vibration is observed in the data block corresponding to points 1 and 5 are 24.36 Hz and 46.39 Hz, respectively.

Comparison of FEA and Experimental Results
The base structure is diagnosed by analyzing the damped natural frequencies and mode shapes obtained by modal analysis using ANSYS™ software and comparing it with excitation frequencies. It is observed that the natural frequencies (second and third modes) from Table 4 are close to the excitation frequencies and hence the resonance condition exists. Figures 14 and 15 show the ODSs at 24.36 Hz and 46.39 Hz, respectively.
The ODS [1] would closely approximate mode shape for a frequency close to the natural frequency of a structure. The ODS at 24.36 Hz in Figs. 13 and 14, does not correspond to the second mode shape shown in Fig. 8 (25 Hz). The behavior predicted by test points 3 and 4 (refer to Figs. 11 and 12) almost corresponds to the nodes of the structure. Hence, more measurement points would be needed between test points 3 and 4 in order to gain more definition at this frequency. It is also observed that ODS at 46.39 Hz in Fig. 15 is a linear combination of third (41 Hz) and fourth (53 Hz) mode shapes shown in Figs. 10 and 11, respectively. Hence, it does not correspond to the third mode shape.

Conclusions
In this study, vibration analysis of a base structure supporting a centrifuge-motor assembly was carried out. The important points that can be summarized are • ODS analysis was performed using ME'scopeVES, and the possible excitation frequencies were extracted. • Modal analysis of the base structure with pre-stressed effect was done using a combination of shell and beam elements. • The observed excessive vibration at the operating speed of the centrifuge was attributed to resonance since the structure is operating in the resonance band of frequencies. • Structural modification with appropriate reinforcement is recommended.
Funding Open access funding provided by Manipal Academy of Higher Education, Manipal. This research did not receive any specific grant from funding agencies in the public, commercial or not-for-profit sectors.

Declarations
Conflict of interest The authors declare that they have no conflict of interest.
Open Access This article is licensed under a Creative Commons Attribution 4.0 International License, which permits use, sharing, adaptation, distribution and reproduction in any medium or format, as long as you give appropriate credit to the original author(s) and the source, provide a link to the Creative Commons licence, and indicate if changes were made. The images or other third party material in this article are included in the article's Creative Commons licence, unless indicated otherwise in a credit line to the material. If material is not included in the article's Creative Commons licence and your intended use is not permitted by statutory regulation or exceeds the permitted use, you will need to obtain permission directly from the copyright holder. To view a copy of this licence, visit http:// creat iveco mmons. org/ licen ses/ by/4. 0/.