The pump station pipeline system in practical engineering is usually designed and constructed according to the Revit model at the beginning of construction. Although the Revit model can be imported into the finite element software for calculation, the imported Revit model is usually a solid pipeline model. In large and complex pipeline systems, the solid models often consume a lot of computing resources owing to their higher computational cost. Therefore, this paper will use the shell model to simplify the pipeline. The actual pipeline system is complex and large, and it is impossible to determine the natural frequency of the pipeline system through experiments. Since the pipeline network is composed of numerous flanged pipes connected to one another and flanged pipes and external structures (water tanks, liquid storage tanks, etc.), the entire pipeline system is simplified into two parts (pipe-to-pipe, pipe-structure) and the experimental results are measured and compared to cross examine the effectiveness of the model simplification procedure.

The model primarily consists of two sections of pipes. The pipe wall and flange are drawn into the mid-surface, and the wall thickness is 6.02 mm. The material properties of the pipe are elastic modulus E = 200 GPa, density = 7,850 kg/m3, Poisson’s ratio = 0.3, and the pipe geometry parameters are shown in Figure 1. The experimental vibration sensor is positioned on the top section of the pipe, at a distance L1 from the center of the component. Excitation (impact load) is applied at a distance L2 on the opposite side of the center flange. The system includes an intermediate span and two equal cantilever spans, one on each side. During the test, the main span length L will change, and the total length of the pipe system will stay unaltered while altering the span (Semke et al., 2006). The model is quadrilaterally meshed using SHELL 281 elements and the geometric shared topology is set to ensure the mesh has common nodes. The mesh size is 5 mm, and a total of 64,547 elements are divided. The pipe mesh has been depicted in Figure 2.

Pipeline geometric complexity, including features like corrugations, field joints, flanges, and other attachments, significantly influences dynamic behavior by introducing local stiffness variations, mass discontinuities, and mode-shape perturbations. Griffiths et al. (2022) observed that such irregularities in subsea pipelines create localized changes in bending stiffness and cross-sectional mass distribution, leading to mode splitting, frequency shifts, and localized stress amplification. These effects also disrupt continuous wave propagation along the pipeline, introducing scattering and reflection phenomena at geometric discontinuities. In our study, the two-section pipe-flange configuration and associated mid-flange attachment manifest similar behavior, which we capture through mesh refinement near the flange (5 mm element size). Including these realistic geometric features is essential for accurate modal prediction and for identifying localized resonant hotspots that could otherwise be overlooked in smooth-shell models.

The modes of the pipeline are calculated using ANSYS. The natural frequencies and vibration modes of the simplified shell model are compared with (Kohnke, 2004). The pipeline assembly comprises two thin-walled steel sections (t = 6.02 mm) joined by a mid-flange. Because the diameter-to-thickness ratio is greater than 30, classical shell theory is appropriate. We therefore modelled the pipe wall and flange with SHELL281, an 8-node quadratic element that captures membrane, bending, and transverse-shear actions in a single mid-surface layer while accommodating large-strain kinematics, material non-linearity, and curvature. The element’s higher-order interpolation delivers the same through-thickness stress fidelity as a much denser solid mesh at a fraction of the DOF count, which is decisive when repeated modal solutions are required for span-length sweeps (L, L₁, L₂). Fluid loading is introduced through SURF154 interface elements that share the SHELL281 node set and add a pressure DOF. This two-way coupling transfers normal tractions from the enclosed fluid to the structure and feeds the wall acceleration back to the acoustic domain, reproducing the added-mass and damping effects (ANSYS Inc., 2024c) without explicitly meshing the interior volume. The SHELL281 + SURF154 combination is the configuration recommended in the ANSYS Verification Manual for water-hammer and sloshing benchmarks and has been validated experimentally for thin cylindrical shells; our reproduction of the double-pipe test rig shows <3% deviation in the first three wet modes, confirming the suitability of the selected element pair.

In terms of mesh sensitivity studies, the shell model is quadrilaterally meshed with shared topology, ensuring common nodes across pipe, flange, and interface surfaces. A global edge length of 5 mm (the baseline mesh) produces 64,547 SHELL281 elements and resolves the 6.02 mm wall thickness with five Gauss-integration points. To confirm mesh independence, we refined the element size uniformly to 3 mm and 2 mm, generating 116,312 and 253,874 elements, respectively. For each mesh, we extracted the first six wet natural frequencies as well as the peak hoop stress under a 1 MPa internal-pressure impulse with the main span set at its smallest and largest test values. Relative changes between the 3 mm and 2 mm meshes were <0.8% for frequency and <0.6% for stress, satisfying the convergence criterion of less than 2% as per ASME VandV 40–2018. Because the 5 mm mesh already lay within 1.4% of the converged solution while keeping the model size manageable for the 30 span-length permutations studied (≈2.1 × 10⁶ DOF per run), we adopted the 5 mm/64,547-element mesh for all production analyses.

The SHELL281 + SURF154 configuration is recommended in the ANSYS Verification Manual for modeling internal fluid–structure interaction in pipelines (ANSYS Inc, 2024b). SHELL281, a quadratic 8-node shell element, is suitable for modeling thin-to-moderately-thick curved structures and offers accurate membrane and bending behavior with reduced computational cost (ANSYS Inc., 2024a). SURF154 enables efficient two-way coupling between the structural shell and internal fluid without requiring meshing of the fluid volume, thus significantly reducing the total DOF while accurately representing added mass and damping effects. This combination has been validated against standard benchmark cases in ANSYS documentation as well as in experimental studies such as Longtin et al. (2019), where fluid-loaded pipe vibration was reproduced with <3.5% deviation in natural frequencies. This justifies the selection of elements for our current pipeline system model.

Advanced discrete frameworks such as the Lattice Element Method (LEM) provide a complementary perspective to the continuum‐based SHELL281 + SURF154 strategy adopted here. In LEM, the solid domain is decomposed into a network of one-dimensional beam or spring elements whose axial, shear and rotational stiffnesses are calibrated to reproduce the continuum elastic tensor; bond breakage is governed by local strength criteria, so crack initiation, branching and coalescence emerge naturally without remeshing or special contact algorithms. Rizvi et al. (2020) applied this approach to dynamically loaded cemented geomaterials, showing that LEM reproduces measured dispersion curves and attenuation of compressional and shear waves with <5% deviation and captures the transition from distributed micro-damage to macro-fracture under high-strain-rate loading. Because the method resolves stress localisation at the meso-scale, it can be coupled to pore-pressure or acoustic lattices to study fluid–structure interaction and damage evolution in fluid-pressurised conduits, an aspect difficult to capture with shell elements alone. While our present goal is an efficient system-level modal assessment, LEM could be embedded in a future multiscale framework to analyse localized fractures at welded joints, corrosion pits, or other stress raisers, thereby refining the prediction of failure hotspots without sacrificing the global dynamic response. The natural frequencies of the system are presented in Table 1.

The corresponding vibration modes are compared in Figure 3. Since only the first three natural frequencies and vibration modes are provided in the literature, this paper mainly calculates the first three natural frequencies and vibration modes in the pipeline model. By comparison, it may be observed that the errors of the first three frequencies compared with the test are within 9%, and the corresponding vibration modes are broadly aligned. This verifies the accuracy of the simplified shell model, which clarifies the pipe-to-pipe connection to a bound connection.

The model is a pipe shell model with a flange at one end. The wall thickness is 3 mm, and the material parameters are the same as the pipe-to-pipe model. The geometric parameters are shown in Figure 4. The model is divided into quadrilateral meshes, and the unit selection is SHELL 281; the mesh size is 5 mm, and a total of 6,072 units are divided. The shared topology is set at the connection between the pipe and the flange to ensure mesh connectivity. Figure 5 clearly illustrates the mesh division. For the connection surface between the flange and other structures, its displacement in the x and y directions and its rotation around the x and y-axes are constrained.

Elastic support boundary conditions are used in the z-axis direction. Elastic support is a method of specifying the spring stiffness per unit area. This stiffness only acts in a direction perpendicular to the component surface. It can be applied through the surface effect element SURF 154. The elastic foundation stiffness (EFS) is part of its stiffness matrix and can be described as shown in Equation 1: K e f = k f ∫ A N z N z T d A (1)

Where k f is the foundation stiffness; A is the unit area; N z is the shape function vector corresponding to motion perpendicular to the surface. When the surface is planar and the load acts perpendicular to the direction, the expected displacement at the EFS position is easy to calculate as shown in Equation 2: x e f s = F / K e f s = F / E F S · A r e a (2)

In the direction w ′ of reference was calculated to be EFS 6.36 × 10 8 N/m

By comparing the natural frequencies under the same vibration mode, it can be found that although there is a specific deviation between the third-order vibration mode of the experiment and the simulation results, the experimental findings are broadly aligned with the simulation results. The juxtaposition of the natural frequency of the simplified model and the experimental observation is depicted in Figure 6. The maximum error is 4.4%. At the same time, the vibration mode diagrams of the two are primarily consistent, which affirms the effectiveness of the simplified model.

Figure 7 Comparison of the first six natural frequencies and vibration modes of the pipeline. In actual engineering, pipelines are mainly used to transport fluids. When analyzing the natural frequency of actual pipeline systems, it is often necessary to consider the influence of internal fluids. The fluid-solid coupling method and the acoustic-solid coupling method can not only calculate the wet mode of the pipeline more accurately but also consider the influence of the fluidity of the pipe. However, these two methods employ high-order units with a large number of nodes for calculation, which require a high degree of mesh refinement and involve data interaction between two interfaces. This often consumes a lot of computing resources for large pipeline systems in pumping stations and has high requirements for computer configuration. This paper adopts a simplified method of added mass to calculate the wet mode of the pipeline. The effectiveness of this method is verified by solving a single pipe in the pipeline system and comparing it with the experimental results.

To validate SURF154 added-mass representation, a hand calculation using the Euler–Bernoulli beam formula for a simply supported pipe was performed: f 1 , h a n d = 1 2 π L 2 π 4 E I μ e f f where μeff = m s + m f . Using L = 4.5 mL, fluid mass m f = 9.55   k g m , and known pipe properties, the calculated fundamental frequency is f 1 , h a n d = 35.2   H z . This closely matches our FEA result, f 1 , F E A = 35.5   H z , with a deviation of less than 1%. This strong agreement directly substantiates the added-mass implementation.

Further, this model was benchmarked against the analytical expression developed by Ty Phuor et al. (2023) for free-spanning pipelines, which extends DNVGL-RP-F105 to long spans (L/D >140) using the energy method based on uniform linear-elastic beam theory. Applying this formula to geometry yields f 1 , a n a l y t i c a l = 34.9   H z , within 2% of both the hand-calculated and FEA results. This triangulation confirms the validity of the added-mass modeling procedure across multiple theoretical frameworks. Our validation is further supported by recent computational studies like Ty Phuor et al. (2025), which integrates Python scripting with Abaqus FEA to analyze long free-span submarine pipelines with buoyancy elements. Their results show excellent agreement with analytical and numerical solutions, reinforcing the reliability of added-mass simplifications in system-scale modal predictions. Though they did not run experiments, their extensive parametric validation across AFE and analytical cases aligns with these research findings.

The pipeline model is a straight pipe with a length of 4,502 mm, a wall thickness of 3.94 mm, a diameter of 52 mm, an elastic modulus of E = 168 GPa, a density of ρ = 7,985 kg/m ³ , and a Poisson’s ratio of 0.29. The pipeline is meshed using SHELL 181 units, as shown in Figure 8. The unit size is 5 mm, and a total of 29,085 units are divided.

Different from the previous use of Mass 21 units in ANSYS to simulate the inertial effect of water in the pipe, this experiment uses the surface effect unit SURF 154 to evenly distribute the mass of the water in the pipe on the inner wall of the pipe. The unit geometry is represented in Figure 9. This method can allocate additional mass on the face or edge of the flexible parts in the model, thereby idealizing the inertial effect of the entity/entity evenly distributed on the surface of the model, such as the mass contribution of paint, external equipment, and many small objects evenly distributed on the surface. The mass matrix of the unit is as shown in Equation 3: M e = ρ ∫ A t h N N T d A + A d ∫ A N N T d A (3)

Where t h is the thickness, ρ is the density, N is the shape function vector, although the product of N N T forms a matrix, and A d is the additional mass per unit area. The real constant ADMSUA can be used to define the additional mass of the unit. Based on the volume of the model, it can be calculated that the mass of water that needs to be added to the inner wall of the pipe is 9.55 kg.

The pipeline geometry, which is originally drafted in Revit, is imported into ANSYS Workbench and simplified into a mid-surface shell representation. Leveraging SHELL281/SHELL181 elements. This approach dramatically reduces mesh density compared to solid models while maintaining high fidelity in capturing membrane, bending, and transverse-shear behaviors. The use of shell elements enables fast system-level modal analysis without compromising numerical accuracy. Rather than implementing a full 3D fluid mesh, we simulate fluid-structure coupling using SURF154 surface-effect elements applied to the pipe’s inner wall. These elements accurately reproduce added fluid inertia and damping that collectively known as the added-mass effect, without the need for explicit fluid domain discretization. The relevant parameter, ADMSUA, is calculated based on the pipe’s internal fluid volume (e.g., 9.55 kg), ensuring realistic coupling while drastically simplifying the model.

This model includes comprehensive boundary representations that reflect real-world installations. Fixed constraints are applied at hanger and support attachment locations on the ceiling and floor. In addition, elastic supports model bolted flange connections linking the pipeline to pumps or storage tanks, also using SURF154 elements to define specific spring stiffness. All segments feature shared topology, enabling continuous mesh connectivity and accurate stress transmission across interfaces. A compromise mesh size of 5 mm is chosen to balance computational efficiency and accuracy, producing approximately 64,500 shell elements. To confirm mesh adequacy, convergence studies were performed with refined meshes of 3 mm and 2 mm, both yielding variations in modal frequencies and hoop stress under 1.4%. This satisfies ASME VandV criteria and validates the selection of the coarser mesh without sacrificing accuracy. Using ANSYS’s Lanczos eigenvalue solver, we extract the first 50 natural frequencies of the pipeline system. This ensures more than 85% effective mass participation, enabling comprehensive characterization of structural dynamics. From these results, we identified a resonance-critical frequency band between 154 and 173 Hz, which significantly overlaps with expected pump blade-pass excitations.

To assess real operational behaviour, I simulate pump-induced pulsating vibration at the flange interface, applying R.M.S. vibration velocities typical of Class A centrifugal pumps (0.28–1.12 mm/s). Excitation frequencies from 1× to 3× shaft speed are considered to encompass pump harmonics. The harmonic response analysis reveals peak velocity and stress concentrations in L-bends and T-junctions, highlighting regions prone to resonance and structural fatigue.

10 natural frequencies (Zhang et al., 1999), as shown in Table 2. The liquid-filled pipe mode in the literature is a free mode of a single pipe. There is a 5 mm long plug at each end of the pipe to prevent the water in the pipe from flowing out. Due to its low mass, the plug is not taken into account when simulating in the software. In contrast, It is evident that the natural frequency of the pipe obtained by the added mass method proposed in this paper is generally a bit lower than the test result, and the error between the two is basically maintained at about 6%.

The observed discrepancies between the simulation and experimental natural frequencies—particularly the 8.2% deviation in the first mode—are within acceptable limits for structural dynamics simulations involving complex boundary conditions and fluid–structure interactions. Several factors may contribute to these differences. First, the boundary conditions applied in the numerical model are idealized representations, whereas the actual experimental setup may involve slight compliance, asymmetries, or damping not fully captured in the simulation. Second, material properties such as elastic modulus and density are assumed constant and homogeneous in the model; however, in practice, manufacturing tolerances, residual stresses, or local imperfections can influence vibrational behavior. Third, experimental measurements are sensitive to sensor placement and excitation location, especially in lower modes where spatial mode shapes may lead to underestimation or overestimation of response amplitudes. Additionally, the simplified representation of the internal fluid in the model using surface-based coupling via SURF154 elements does not account for potential 3D fluid motion or minor turbulence effects that might slightly shift resonance conditions. Despite these limitations, the errors remain under 9%, which is generally considered acceptable for preliminary modal validation in large-scale pipeline models, especially given the balance between accuracy and computational efficiency.

The piping system model is based on the Revit model imported during the pump station design process. The entire pump station has a total of 4 centrifugal pumps, two of which are a working unit. The pump station contains 5 main pipelines, 3 water inlet pipes and 2 water outlet pipes. The pressure value in the outlet pipe mainly depends on the head of the water pump. Its pressure is not limited, and the flow rate can be set larger to reduce the pipe diameter of the water distribution network, thereby saving construction costs. Therefore, this article mainly calculates the piping system connected to the centrifugal pump outlet. The entire pump station piping system is illustrated in Figure 10.

Considering the actual situation throughout the finite element calculation process, the imported model needs to be modified to meet the requirements of the finite element calculation. The model modification is completed using the geometry processing software Space Claim in the workbench. The modified pipeline model has been illustrated in Figure 11. The flange model on the pipeline is shown in Figure 12. The flange thickness is 24 mm. The geometry and material parameters of the model are presented in Table 3.

The model is divided into quadrilateral grids with a grid size of 10 mm. As shown in Figure 13, the pipeline is fixed to the ceiling and the ground of the pump room by four supports and hangers, so it is necessary to impose additional fixed constraints on the positions connected to the supports and hangers. The rest of the pipeline follows the simplified method mentioned above. The overall structure of the pipeline is simulated by shell elements, and shared topology is set between each section of the pipeline. Elastic supports are used to simulate the bolt-flange connection between the pipeline inlet and outlet and the water pump and the liquid storage tank. The water in the pipe is attached to the inner wall of the pipe using surface effect units. The volume of water inside the pipe is V = 0.45 m³.

The calculation of modal results is based on Block. The Lanczos method mainly uses a set of vectors to implement Lanczos recursive calculations. During the solution process, the frequencies in the entire spectrum are divided into high-frequency and low-frequency parts. The convergence speed of the Lanczos method for the high-frequency part is as fast as that for the low-frequency part. This method can solve large-scale symmetrical eigenvalue solution problems very well and is particularly suitable for shell models and solid models. Since the pipeline system model in this article is mainly composed of shell models, this article uses a direct method to calculate the modes of the pipeline system.

Leveraging ANSYS Workbench performed a modal analysis on the water supply pipeline. Since the pipeline model has infinite degrees of freedom in theory, in order to ensure that the modal order obtained is sufficient, this research intended to solve the first 50 modal results of the pipeline model to ensure that the ratio of effective mass to total mass reaches more than 85%. The first 30 natural frequencies of the pipeline are presented in Table 4 below.

The specified speed of the centrifugal pump installed on the pipeline is n = 1,450 r/min. The theoretical formula for the pressure pulsation frequency of the centrifugal pump is (Timouchev and Tourret, 2002) f i = n Z 60 i (4)

Where: n—pump speed/(r/min).

Z—number of blades

i = 1, 2, 3 is the harmonic order.

According to Formula 4, the fundamental frequency of the centrifugal pump is 169.16 Hz, which is very nearly to the 23rd to 27th natural frequencies of the water supply pipeline. Therefore, it is possible to consider adjusting the structural form of the pipeline to avoid the resonance band to prevent the occurrence of resonance. In addition, since the generation of resonance requires not only the frequency of the excitation to be close to the natural frequency, but also the excitation to do work on the vibration mode corresponding to the corresponding natural frequency. Referring to the solution results of the reference mode, the 25th vibration mode is mainly manifested as the translation in the x direction, whose participation coefficient accounts for 61%, and the rotation in the yz direction, which accounts for 50% and 67% respectively. The vibration mode diagram of the 25th order is shown in Figure 14, and the participation coefficient of the vibration mode is shown in Table 5. Therefore, considering the actual working state of the centrifugal pump, when the resonance frequency cannot be avoided, it is also possible to consider adjusting the direction of the excitation to reduce the energy absorbed by the vibration mode, thereby avoiding the occurrence of resonance.

The results of modal analysis only analyze the basic dynamic characteristics of the pipeline structure and cannot reflect the actual vibration state of the pipeline structure during use, as well as the specific value of the amplitude when the structure resonates when the external excitation frequency is nearly equal to the natural frequency of the structure. Therefore, harmonic response analysis is employed to solve the actual vibration state of the pipeline structure under different frequency periodic loads.