Finite element vibration analysis of the pipeline manifold of the catalytic reforming apparatus under flow pulsation and mechanical loading
|Keywords||Pipeline manifold, catalytic reforming, compressor, separator, vibrations, flow pulsation, vibrodisplacements|
|Programs in use||SolidWorks, ANSYS|
Technological progress in piping systems development demands much pump and compressor plants and pipelines elements safety and work reliability. Pipeline manifolds vibration amplitudes often reaches significant values and might be as a reason of their reliability and safety worsening. Pipeline vibrations may evolve from working stream pulsation as well as from compressor vibrations.
Principal reason for the compressors vibration arising is inertia forces of the unbalanced masses. Besides, the reason of the high pipeline vibration levelcan be operation in mechanical resonance conditions, i.e. at natural pipeline frequencies coincidence with disturbing harmonic frequencies. To provide offset of the system operating conditions from its natural frequencies it is necessary to define their values and mode shapes.
The purpose of this work is 3D vibration analysis of catalytic reforming device pipeline manifolds on various compressor units operating modes. 3D model of compressors-pipelines-supports-separators system is developed. The utilization of finite element analysis system ANSYS allowed:
- to estimate strengthcharacteristics of pipeline support elements;
- to compute the forces originating due to working steam pressure pulsations in the pipelines;
- to define natural frequencies values and to plot corresponding mode shapes;
- to plot amplitude-frequency response curve;
- to define the location and values of maximum displacement.
In the frameworks of this analysis 3D geometrical and finite element models of pipeline manifolds, compressors, separators and support elements are developed.
In figure below there is a compressor plant 3D FE model (hereinafter - compressor). Its foundations, electric motor and compressor casing are simplified for modeling, but their mass and strengthcharacteristics are retained. Absorption and discharge pressure buffers and also their support elements are the most compliant structure elements; therefore they are modeled taking all geometrical features into consideration.
3D FE model of the compressor
3D FE model was created on the basis ofdeveloped pipeline manifolds solid models. The FE model allows carrying out vibration state analysis. Pipeline manifolds straight zones are modeled using 3D beam elements PIPE16 with corresponding geometrical characteristics. Pipe-bends, adapters and T-bends are modeled with the use of beam elements PIPE17 and PIPE18. During creating FE model reinforcement and insulation mass and strengthcharacteristics were considered.
The pipeline manifold model contains 72 stiff support elements, 4 fixed support elements, 3 vertical stiff support elements for vertical pipelines, 12 bend support tubes and 101 sliding support elements. FE model consists of 120 000 elements and has 380 000 degrees of freedom.
3D FE models of the pipeline support elements
3D FE model of the pipeline manifolds
In this work with the purpose to perform the pipeline binding vibration analysis the following force factors are considered:
- compressor vibrations;
- pipeline working stream pressure pulsations;
Vibration analysis of the considered system is carried out for three compressors operating modes (only two of three compressor plant are working simultaneously).
Load application scheme
For the transient force loads (caused by the pipelines gas pressure pulsations) the method consisting of two stages is developed. At the first stage the pipeline system pressure transient distribution is computed. Pipelines direct parts are modeled using 3D finite elements FLUID116. These elements allow to model fluid flow using Bernoulli equation in taking loss due to friction into consideration. Pipe-bends and T-bends are modeled using finite elements FLUID116 taking local hydraulic resistance (obtained on the basis of reference data) into consideration. At the second stage (on the basis of obtained pressure transient distribution) transient force influences on pipelines computation is implemented.
Taking those vibration influences into consideration the vibration analysis of catalytic reforming plant pipeline manifolds is carried out. For natural frequencies and mode shapes definition the Lanczos method providing high convergence value for systems with big degrees of freedom number is used. For forced vibrations (caused by influence of harmonious driving force) computation the harmonic analysis taking mode shapes up to 5w1(for three cases of simultaneous work of two compressors - one compressor is under repairing or in the reserve) and assigned damping coefficient into consideration is applied.
Using FE modeling and analysis of the pipeline manifold vibration state (at all compressor operating modes) resulting characteristic points are chosen, where the maximum displacements on working and multiple to it frequencies are reached. For the selected point amplitude-frequency responses are plotted, i.e. vibro-displacements amplitudes from driving force frequency dependence graphs.
Ux displacements at work regime
As a result of analysis it is proved that for each compressor operating mode the maximum displacement amplitudes are observed for driving force frequency 2w1 in point A and are equal accordingly to 0.4Ucritical, 0.3Ucritical and 0.1Ucritical, that does not exceed the admissible level of vibro-displacements Ucritical amplitudes.