oa CFD Simulations of Abnormal Flow in Horizontal Pipes for Offshore Hydrocarbon Transport

Introduction: Industrial pipelines for multiphase transportation can result in unstable flows which often cause major operational problems. Due to liquid wave growth and phase interactions (hydrodynamic slugs), liquid arriving in larger, intermittent chunks may cause flow instabilities in pipelines. At an increased air volumetric flow rate, the surface wave amplitudes become larger to the pipe/conduit and wave forms frothy slug where it touches the wall of the pipe. When the slugs travel at a velocity higher than average liquid velocity, it can cause severe vibration that could reduce the integrity of or damage equipment. In order to tackle the problems associated with slug flows, there is a clear need to better understand the multiphase flow leading to various flow phenomenon in the pipelines. The multiphase flows are characterized by flow patterns or regimes that define a particular distribution of phase volume fraction in pipeline.

While there are several numerical models characterized the development and evolution of slugs and slug flows, studies which describe the stress analysis of these slug flows and their effects are scarce. This study compares two CFD codes (ANSYS CFX and FLUENT) in slug development in jumper and the stress analysis of slug movement in jumper. As well, the effects of flow parameters such as fluid superficial velocity, fluid density ratio, and viscosity on slug were investigated.

The model considered in the present study is based on a quasi-3D formulation where the governing equations are based on volume averaging and ensemble averaging of Navier-Stokes equation. In present study, proposed benchmark relies on focusing on two CFD tools, FLUNT and CFX, to simulate surface instabilities and slugs on stratified flow in a horizontal channel considering slip, surface tension, and frictional momentum transfer between the phases (liquid and gas).

FLUENT Set-up The setup mimics the modified version of the experimental study previously investigated by Vallee and Hohne (2007), the flow channel with rectangular cross-section was modelled using Computational Fluid Dynamics (CFD) package, FLUENT code. The dimension of the model are 4000 ×  300 ×  30 mm³ (length ×  height ×  width). The simulation was performed by a grid consists of 4 ×  462 hexahedral elements and 4 ×  46152 nodes applying a quasi-3D model that consider the wall effect of channel in a 2D model. The volume-of-fluid (VOF) model is used for modeling the fluid domain with air and water. This model is well suited for separated flows with no mixing at the interface. The fluid interface shape is represented by geometric reconstruction scheme. For the two-phase flow, 1.0–1.5 m/s superficial velocity of water and 5.0–11.5 m/s of air were chosen for the CFD calculations. The model inlet was divided into two parts: in the lower half of the inlet cross–section, water was injected and in the upper half air. An initial water level of 50 mm was assumed for the entire model length. As well, initial inlet velocity 1 m/s was considered for water and air, and the velocity of air was increased gradually to simulate different scenarios until final velocity 11.5 m/s considered in this work. The reference pressure considered during the simulation was 1 bar and surface tension of 0.072 N/m. A hydrostatic pressure was also assumed for the liquid phase. For surface instability generation with subsequent slugs, the interfacial momentum exchange and turbulent parameters had to be modeled accurately (Razavi and Namin). In this regard, turbulent model of K-ε model was chosen as the viscosity that is able to model surface instabilities and turbulence of slug flow. Solution for calculating 15s of simulation time on 6-processors lasted for 48 hours. Selected discretization schemes were PRESTO for pressure, Geo-Reconstruction for volume fraction, and First Order Upwind for other cases. Variable time step between 10–6 and 10–3 was appropriate steps for the simulation.

CFX Set-up Building the geometry in ICEM, the mesh was then imported to the ANSYS CFX-Pre in order to define the simulation parameters. Air and water were defined as the two gaseous and liquid phase and using the expressions, the height of water is set to 0.05 (half of the area section) through the entire domain. According to (Frank, 2005), Shear Stress Transport (SST) turbulence model was selected for the simulation and the term “Production and Dissipation” was added to the equations. Surface tension coefficient was set to the value of 0.072 (N/m), interface length scale to 1 (mm), and drag coefficient to 0.44 ( − ) (Frank, 2005). The mixture model was chosen for the interphase transfer. The inflow type was chosen as ‘inlet” and the fractional intensity was set to the value of 0.05 with the eddy length scale equal to the liquid height at the upstream (Razavi & Namin, 2011). The mass flow rate of air and water were set to the values of 0.074 (kg/s) and 7.83 (kg/s), respectively. Several simulations were conducted in order to improve the simulation results and due to the blockage of the outlet in the previous runs, the outflow boundary type was set to “opening” instead of “outlet” with a pressure controlled and medium intensity (5%) turbulence in the boundary details.

The liquid and gaseous phases were defined based on their volume fraction in downstream at outflow. The wall boundary type was set to “wall” and for both phases “no slip wall” and “smooth wall” options were assigned to the mass and momentum and the wall roughness, respectively (Hohne, 2009). The analysis type was set to transient with the total simulation time of 8 (s) and time steps of 0.001 (s), according to the similar study conducted by (Razavi & Namin, 2011). In the solver control, a second order backward Eulerian approach was chosen with high resolution turbulence. Due to the instability and fatal errors in the previous simulations, the minimum and maximum number of loops were set to 1 and 200 (due to divergence problem), respectively with the convergence criteria of 1 × 10^–4.

Figure 1: Abnormal flow simulations (L =  4 m, D =  0.3m, Ug =  9 m/s and Ul = 1 m/s). References: S.Y. Razavi and M. M. Namin. Numerical Model of Slug Development on Horizontal Two-phase Flow, Proc. of Int. Conf. on Recent Trends in Transportation, Environmental and Civil Engineering 2011.

A. Ashrafian, J-C. Barbier and S.T. Johansen. Quasi-3D Modeling of Two-Phase Slug Flow in Pipes. 9th International conference on CFD in the minerals and process industries CSIRO, Melbourne, Australia, 2012.

T. Frank. 2005. Numerical Simulation of Slug Flow regime for an air-water two-phase flow in horizontal pipes, The 11th International Topical Meeting on Nuclear Thermal Hydrualics (NURETH-11), Avignon, France, 2006.

R.E.M. Morales et al. 2013. A comprehensive Analysis on Gas-Liquid Slug Flows in Horizontal Pipes. Offshore Technology Conference, Brazil. OTC 24437.

D. Duraivelan, Y. Dai and M. Agrawal 2013. CFD Modeling of Bubbly, Slug, and Annular Flow Regimes in Vertical Pipelines. Offshore Technology Conference. OTC 24245.