Using Computational Fluid Dynamics ( CFD ) Simulation to Model Fluid Motion in Process Vessels on Fixed and Floating Platforms

Computational Fluid Dynamics (CFD) is a mathematical tool capable of simulating a wide range of fluid flows. Integrated CFD software has been applied to study the flows in twoand three-phase oilfield separators. The influence of inlet nozzle configuration, flow distributors, perforated plates, and outlet nozzles have been studied. Of particular value has been the ability to simulate wave induced sloshing in vessels mounted on floating platforms. The design and placement of baffles to mitigate liquid sloshing was determined by using CFD to simulate fluid flows in vessels destined for service on floating platforms. The simulations accounted for the movement of the vessel based upon its actual location on the platform and identified the influence of process fluid flows on slosh motion. Where possible, laboratory testing has been used to validate CFD simulation results, leading to increased confidence in the mathematical models.  Until recently, the engineering design of twoand three-phase separators was considered to be mature. However, the need for separation systems to operate in challenging environments, such as on floating platforms, has led to a demand for improved vessel designs that require reduced fluid residence times and effective separation even when the fluids are jostled by the six-degrees of motion (pitch, roll, heave, surge, yaw and sway) experienced by a floating platform. CFD allows a designer to observe the simulated fluid flow paths within a vessel and assess how the separator will perform under these difficult circumstances. The application of CFD to solving oilfield related problems can be of value in new product development, vessel design optimization, determining sources of underperformance for existing or proposed vessels, and for evaluating the projected performance improvement when retrofits are installed to upgrade existing process equipment . CFD provides the means to visualize fluid flows within a separator as well as an ability to track the movement of gas/liquid and liquid/liquid interfaces. In newer versions of CFD software, gas bubbles, oil droplets, and solid particles can be tracked through a separator using advanced multiphase models. This permits one to incorporate performance enhancement into the design of a vessel without the need for extensive testing in physical models. Validation of simulated results is recommended when possible, however, to insure that the CFD simulations are in fact providing reasonable predictions. CFD Simulation Parameters The simulations reported here were based upon standard “k” turbulence and volume of fluid (VOF) models. Both steady state and transient simulations were used depending upon the objective of a particular project. The CFD software package used was from Fluent Incorporated (Lebanon, New Hampshire). GAMBIT was used to build the model geometries and their volume meshing. FLUENT was used to run the simulations, and FLUENT's parallel processing capabilities were implemented to accelerate the simulation process. To model the movement of the vessels on floating platforms, a special User Defined Function (UDF) was developed. The UDF allowed the movement of the separator of interest to be calculated based upon its actual location on the floating platform, the Center of Rotation (COR) of the platform, and the periods/amplitudes for each sea-state induced motion. Typically, the sea-state data for the simulation included 1year, 10-year and 100-year storm conditions. Parameters that were derived from the simulation included “drag coefficients” at specified wall surfaces within a vessel, average and/or maximum pressure on the surface of an internal component, and fluid velocity profiles. Although these parameters were useful for comparing the intensity of motion on a relative basis, the most instructive information was generally derived from the 2D and 3D animations that showed simulated fluid movement in response to a vessel’s 2 DR. TED FRANKIEWICZ AND DR. CHANG-MING LEE SPE motion. The animations were augmented with particle tracking, a study of fluid velocity vectors and the distribution of turbulence intensity.  The key components in a typical separator that control fluid path line development include the inlet nozzle, the inlet momentum-breaking device, perforated plates, weir or bucket faces, and outlet nozzles. Some components have been modeled individually as well as in combination during the course of the CFD studies. CFD Modeling of Perforated Plates. Perforated plates are used in separators both to establish good fluid flow distribution, and to control liquid sloshing. In a CFD simulation, the perforated plate is modeled as porous media of finite thickness with directional permeability. The fraction of open area can be varied in the porous zone, but hole sizes in the plate are not specifically modeled. To validate the assumption that flow through porous media approximates that through a perforated plate, a separate CFD study was conducted on the design and engineering of perforated plates. The use of perforated plates to correct short-circuit fluid flow paths that are generated as a result of fluids hitting a splash plate in a separator has been discussed previously. 4 Figure 1 shows path lines calculated in a 3-dimensional CFD simulation for fluid flows through a perforated plate in a laboratory test chamber. In this study, physical testing was used to validate the CFD simulation results. The liquid enters the chamber through an off-center inlet. The perforated plate redistributes the flow, but flow path lines develop quickly downstream of the perforated plate and fluid short-circuiting is both predicted by the simulation and observed in laboratory tests. To prevent this short circuiting, a second perforated plate just upstream of the outlet nozzle is required. 4 A general rule of thumb that has emerged from CFD studies is that the inlet fluid immediately anticipates the outlet and will develop high velocity flow channels unless means to prevent this are installed in the vessel. Type of Platform Affects  The type of floating platform on which a separator is installed has a significant impact on the sloshing of fluid inside the separator . Figures 2A and 2B show representative locations for a large separator on a TLP and on an FPSO as well as the Center of Rotation (COR) for each platform. The length of the moment arm, i.e., the distance from the platform’s COR to the separator, affects the intensity of sloshing in a vessel. The moment arm on an FPSO or TLP may be 50 to 200 ft. But the COR of a spar is generally quite low in the water. Thus the moment arm between the COR and the separator can be quite long, 300 to 400 feet not being unusual. Thus, although the degree of pitch for a spar may be low under storm conditions, the long moment arm can result in large periodic spatial displacements of the separator. In one study, a 2-degree pitch for a spar during a 10-year storm resulted in 11 feet of translation for a vertical separator with a period of 10 seconds. This kind of motion can generate significant momentum waves within a separator that require additional modifications to the vessel internal designs in order to adequately dampen the slosh waves. A separator installed on an FPSO will generally experience more roll motion than that on a spar or a TLP. The roll motion, which may or may not remain in phase with the pitch and surge, requires the use of special weir designs to control water spillover without interfering with the normal flow of oil over the weir. One type of slosh motion control baffle that has been installed in separators on floating platforms is a horizontal ring baffle. According to published research 7, , the ring baffle is capable of dampening liquid slosh motion when properly sized and positioned. CFD simulations confirm a minor reduction in slosh amplitude in the presence of a ring baffle, but the reduction is far less than what is required in a typical 3-phase separator. Other studies 9 have shown that these horizontal ring baffles can, if improperly placed, generate significant interface turbulence within a vessel that is counter productive for oil-water separation. CFD Separator Models Including Vessel Internals. Criteria that must be considered for the design and installation of perforated plates include the fraction of opening area of the plate, the size and layout of holes that provide the opening area, the amount of open area under the plate to allow for sand migration, the locations for baffle placement, and the number of baffles required to control flow distribution and/or liquid sloshing. A separate CFD study was conducted within NATCO to determine a preferable range for the fraction of open area required in a perforated baffle to control fluid flow patterns. Where possible, the results of these studies were compared with standard engineering calculations 10 in order to calibrate and validate the CFD simulations. The targeted fractional open area is a compromise between the need to restrict flow through the plate and the need to minimize the shearing of oil or water droplets to avoid creating emulsions. The complexity of flow through a perforated plate is illustrated in  Figure 3A shows the development and decay of fluid jets through holes in a perforated plate. Note that when flow approaches the plate with a strongly nonuniform velocity distribution, the flow downstream of the plate tends to spread. Figure 3B is a plot of velocity distribution for the liquid as it approaches the perforated plate and then flows through. Each point represents the velocity for the liquid at a specific volume element within the vessel. The top of the plot is essentially the values of maximum fluid velocity at various distances downstream of the plate. Figure 4 illustrates the high velocity for liquids that can occur under a perforated plate when open are