Abstract: Carbon Capture and Storage (CCS) is an alternative for decreasing greenhouse gas (GHG) emissions by removing carbon dioxide (CO2) from power plants. Accidental discharges from CCS plant will result in a release of dense CO2 gas cloud to the ambience at high concentration which becomes a dominated threat to human health. However, there is a knowledge gap in assessing the release of CO2 via pipeline leakage. Thus, it is necessary to develop an accurate consequence model for CO2 release in order to demonstrate a safe layout and other safeguards. In this study, pure CO2 discharge and dispersion have been detailed out using a three-dimension model with presence of obstacles in a Computational Fluid Dynamics (CFD) software. The realizable κ-ε turbulence model was chosen for simulating the dispersion of pure CO2-air. A case study based on Kit Fox gas experiments of pure CO2 instantaneous release is developed to evaluate the discharge scenario. The results obtained from the model are compared with experimental data available in literatures and validation is achieved.
INTRODUCTION
Carbon dioxide (CO2) is a product of burning solid waste and wood. It is also discharged when fossil fuels (e.g., oil, natural gas, coal) are combusted. For instance, CO2 emissions from fossil fuel power generation (23 Gton-CO2/year) represent approximately 26% the total emissions (Holloway et al., 2007; IPCC, 2005, 2007). CO2 concentration in the atmosphere was observed up to 391 ppmv in 2011 (VijayaVenkataRaman et al., 2012). The high CO2 concentration is the main cause of global warming due to its heat-trapping behaviour. Barker et al. (2007) have reported the increase of the average global temperature near the earth’s surface about 0.78±0.18°C between 1906 and 2005. The consequence from the global warming can be noticed in several phenomena such as a rising of sea levels, melting snow and changing weather patterns (VijayaVenkataRaman et al., 2012). The global warming was determined as the greatest environmental challenge in the 21st century (Akorede et al., 2012).
Carbon Capture and Storage (CCS) is a new technology in decreasing the CO2 emissions. The CCS will assist in achieving 19% of CO2 reduction in 2050 where 9% reduction from industry and transportation and 10% from power generation (IEA, 2009). Over 3000 CCS projects are being planned by 2050. In the CCS system, CO2 is separated by different capture technologies (e.g., post-combustion, pre-combustion and oxy-fuel) from big sources such as fossil fuel power generation. Captured CO2 will be then transported by pipelines across all countries and population areas to storage areas (McCoy and Rubin, 2008; Haugen et al., 2009). Accidental discharges from the CCS are highly likely to happen due to a rupture or puncture of CO2 pipelines (Koornneef et al., 2010). Possible impacts of the accidental CO2 discharges are potential asphyxiant hazards CO2 on human and also the environment due to released CO2 displacing oxygen in the air (Wilday et al., 2011; Koornneef et al., 2012). Exposure to elevated concentration of CO2 can increase the acidity of the blood triggering adverse effects on the respiratory, cardiovascular and central nervous systems of human. It was reported by HSE UK (Wilday et al., 2011) that the allowable exposure limit of CO2 is 0.5% (5000 ppmv) for an 8 h time-weighted average and with a Short Term Exposure Limit (STEL) of 1.5% (15000 ppmv) for 15 min. There are several tragic disasters occurred due to CO2 exposure such as the Noyos Lake on 21st August, 1986 which caused deaths of at least 1700 people and many livestock near the lake and up to 14 km distance from the area in the northwest area of Cameroon, West Africa (Kling et al., 1987). The CCS technology is still under development. A number of knowledge gaps in terms of safety have been identified which require further development (Shuter et al., 2011). One of the knowledge gaps which give rise to research priorities is the modelling of the dispersion of supercritical CO2 releases from pipelines where fracture propagation is a possibility (Koornneef et al., 2012; Shuter et al., 2011; Bilio et al., 2009). This is one of the most important issues in the environmental assessment of CO2 transport pipelines (Bilio et al., 2009).
In the case of accidental release, CO2 will disperse from accidental sources to the atmosphere. An important impact on the CO2 dispersion is the presence of the obstacles such as buildings and trees surrounding the point of release (DNV, 2010). The dense CO2 release may sink in low-lying areas, for example valleys, streams and ditches. Thus, the mechanism of the CO2 dispersion will depend on the mechanical turbulence (Mo et al., 2012). Therefore, numerical dispersion simulation tools for predicting the pure CO2 dispersion should include assessing the impacts of the obstacles.
Numerical codes and models are increasingly used to investigate the behaviour of a released substance and to predict the consequences of a hypothetical hazardous scenario. A large number of consequence tools include two dimension analysis (2D) such as PHAST, SAFETI and EFFECT and three dimension analysis (3D) such as FLUENT, PANACHE and CFX. Computational Fluid Dynamics (CFD) is able to take into account the effects of obstacles and complexity of the geometry for the realistic accidental loss of contaminants consequence (Tauseef et al., 2011a). FLUENT is widely used for a wide range of industrial applications and has an extensive use all over Europe due to its capability of simulating boundary layer (Di Sabatino et al., 2007). A recent comparison between FLUENT and Atmospheric Dispersion Modelling System (ADMS) stressed that the CFD models were more appropriate for situations in complex environments than ADMS (Riddle et al., 2004). The current approach for the dispersion of dense gas is based on the calculation using the realizable κ-ε model with the presence of the obstacles in FLUENT (Tauseef et al., 2011b). Validation of numerical codes and models is a necessary step before the application of the models to safety and risk assessment analysis. This study will use the realizable κ-ε turbulent model in FLUENT 14.0 to simulate dispersion of pure CO2 instantaneous release. A case of the Kit Fox field experiments will be chosen to set up parameters in a 3D-CFD model (WRI, 1998; Hanna and Chang, 2001). Impacts of obstacles and wind on the CO2 dispersion will be evaluated. Highest peak concentration of CO2 at a sensor closest to the point of release will be predicted and compared with experimental data.
MATERIALS AND METHODS
Kit Fox CO2 dense gas field experiment: The Kit Fox CO2 dense gas experiment was conducted to test the dispersion of pure CO2 gas to the atmosphere with presence of obstacles. This experiment was part of the Petroleum Environmental Research Forum (PERF) 93-16 project carried out in late summer 1995 at the US Department of Energy (DOE) Nevada Test Site (WRI, 1998; Hanna and Chang, 2001). The geometry in the experiment has been used for several modelling of the CO2 dispersion (Hanna and Chang, 2001; Mazzoldi et al., 2008a; Papanikolaou et al., 2011).
Pure CO2 gas was released from the ground level area source of 1.5x1.5 m. An entire experiment in term of size was built to represent 1/10 of actual chemical plant or oil refinery (WRI, 1998; Hanna and Steinberg, 2001). In order to do that, thousands of plywood were installed in 120x314 m whole field size to increase the surface roughness of the experiment area. The plywood obstacles were installed in two different arrays of Equivalent Roughness Pattern (ERP) and Uniform Roughness Array (URA). Details of ERP and URA arrays are explained in the Table 1.
The trial 3-7 of the Kit Fox experiment was chosen to simulate the pure CO2 instantaneous release. Details of the trial obtained from WRI (1998) and Hanna and Chang (2001) are described in the Table 2. Thus, the maximum observed concentration of CO2 at detector closest to release section was a value of 8500 ppmv.
Description of CFD-setup: A three dimension domain was created by a box with 315 m lengthx120 m widthx30 m height. Figure 1 describes computational geometry for simulated process. A pure CO2 release area was set at original coordinator (0, 0, 0). The height of release is at ground level (z = 0 m). For reducing the computational costs and simulation time, a total of 75 ERP obstacles were used without the presence of URA obstacles in the domain. The 3D model, as shown in Fig. 1, is designed using the Design Modeller in ANSYS FLUENT 14.0. The mesh of the domain was created at 385,349 cells. Fine mesh has been created near the ground and the obstacles. The mesh becomes coarser near other domain boundaries.
| Table 1: | Details of obstacles in the Kit Fox experiment |
| Table 2: | Kit Fox experimental used in FLUENT simulation |
| Fig. 1(a-c): | Computational domain with ERP obstacles and CO2 release point, (a) Side view, (b) Front view and (c) Top view |
Boundary conditions
Inflow boundary condition: A wind profile includes wind velocity, temperature, turbulent kinetic energy (κ) and its dissipation (ε) was defined at the inflow boundary condition. Horizontal wind direction was shown as in Fig. 1. The calculation for the wind profile of the Ambient Boundary Layer (ABL) was successfully obtained in Papanikolaou et al. (2011). It showed that the stable conditions of the atmosphere were accurately simulated for the wind profile of Kit Fox experiment. Thus, user defined functions were created on C++ to link into Fluent 14.0 based on Papanikolaou et al. (2011) to model parameters of the wind in the domain.
The wind profile was modelled using the approach of the Monin-Obukhov similarity (Kaimal and Finnigan, 1994; Pontiggia et al., 2009):
| (1) |
| (2) |
| (3) |
| (4) |
| (5) |
where, Cμ is equal to 0.09, κ is von Karman constant (0.4), friction velocity, u*, is taken from the experimental data. Cp is specific heat capacity of dry air (1020 J kg-1 K), g is acceleration of gravity (9.81 m sec-2), k is turbulence kinetic energy (m2 sec-2), ε is the turbulence dissipation rate (m2 sec-3), L is Monin-Obukhov length scale (m), T is temperature (K), Tw is ground temperature (K), T* is dynamical temperature (K), u is velocity (m sec-1), z is height of domain (m), z0 is roughness length (m). The wind conditions of the simulated case are stable (F). For the stable condition, the function φh, φm were given by Eq. 6, 7:
| (6) |
| (7) |
Outflow boundary condition: The outflow boundary condition was set at this boundary because the flow pressure and velocity are not previously indicated.
Top and two sides boundary conditions: Zero gradients of flow through these boundary conditions was made. The symmetry boundary condition was chosen to calculate for this assumption.
Ground boundary condition: A standard wall function was applied at the bottom to specify a no-slip condition. A zero value of velocity will gain at this boundary. This approach is useful for decreasing the numbers of cells near to the bottom to avoid resolving the ground surface roughness in the simulation. Fluent version 14.0 (Fluent Inc., 2012) allowed to simulate wall function of sand-grain in ABL. Thus, the roughness of the wall is modelled by following Eq. 8:
| (8) |
where, Ks is corresponding height, Cs is a model constant required for the wall function (using the default value of Cs is equal to 0.5 in Fluent), z0 is roughness length. In the present simulation, the roughness constant, Cs, is defined through user defined function.
CFD-setup| Step 1: | Simulation of the wind flow: To obtain a steady flow of wind field into the domain before CO2 release, a realizable κ-ε turbulence model was implemented. The wind flow is able to get a full development over the computational domain before gas release at the convergence of 160-240 iterations. |
| Step 2: | CO2 releases: From above initial condition, the CO2 release was simulated by using a realizable κ-ε turbulence model and transient condition state simulation. "Wall" boundary was changed to “mass flow rate” at CO2 release area. The release duration of trial experiment is 20 sec. The mass flow inlet boundary condition is a constant value of 3.65 kg sec-1. |
| Step 3: | Dispersion of pure CO2 into the ambience: In this step, the discharge of CO2 was stopped and the released CO2 was entered into the atmosphere. The “mass flow rate” was changed back to the “wall”. The dispersion was simulated up to 135 sec. The time step in running simulations was set at 0.1 sec. |
RESULTS AND DISCUSSIONS
Simulation of a horizontally Ambient Boundary Layer (ABL): A horizontally ambient boundary layer flow was accurately simulated using the CFD code to predict the dispersion occurs without presence of the obstacles (Blocken et al., 2007). Thus, a test of the same speed profile has been conducted from the inlet to outlet boundary.
| Fig. 2: | Locations of predicted wind velocity in computational domain |
| Fig. 3: | Mean wind speed before CO2 releases |
Three different locations in the present computational domain have been set as was shown in Fig. 2. Mean wind speed plot (Fig. 3) illustrates the result of the wind velocity profile at different locations. It shows that the wind flow is horizontally non-homogeneous at the set-up locations. Particularly, the wind speed increases after the wind moves through the obstacle region. The wind velocity at z = 2 m of the inlet in Kit Fox experiment is a value of 2.7 m sec-1. The predicted wind speed at this location is a value of 3.0 m sec-1.
From contour of wind velocity in Fig. 4, it is shown that the velocity rises up to the height of domain and reduces to a value of zero near the obstacles. The CO2 will not disperse well in the obstacle region. Thus, CO2 may be trapped and promote accumulation of high concentration in this region.
Analysis of CO2 cloud concentration simulation: Pure CO2 of 3.65 kg sec-1 has been released from the release point at ground level (z = 0 m). The CFD set-up for solving this problem has been shown above. After the wind flow has fully developed over the computational domain, CO2 has started to release at initial condition (t = 0 sec). Figure 5 shows the mole fraction of CO2 in created cloud. It is observed that toxic cloud gets wider as distance increases from the release point, as shown in. Fraction of CO2 is high at the region close to the release point, indicating very high toxic concentration in that area.
| Fig. 4: | Contour of wind velocity at central plane before CO2 releases |
| Fig. 5(a-b): | The mole fraction of CO2 in created cloud, (a) Top view and (b) Side view |
The nature of CO2, which is denser and less viscous than air, therefore, CO2 tends to come down to the ground, imposing major risks to humans especially in the condition of complex geometry and low wind speed.
CO2 predicted concentration at location of sensor (x = 25 m, y = 0 m, z = 0.3 m) closest to the release point is illustrated in Fig. 6. These simulation results were compared with CO2 experimental data. The CO2 concentration plot (Fig. 6) shows that the CO2 predicted concentration peaks at a higher value and at an earlier time than was determined during the experiment. The CO2 predicted concentration then becomes lower than the experimental data and remains lower for the remainder of the simulation. The maximum volumetric predicted concentration of CO2 is 9,411 ppmv. It indicates that the maximum CO2 concentration was over predicted compared to the concentration from the experiment.
In the present study, the realizable κ-ε turbulence model in FLUENT 14.0 predicted a value of maximum CO2 concentration of 9,411 ppmv at a distance of 25 m while the experimental data is 8,500 ppmv at the same location. The UK occupational reported exposure limit of CO2 is 0.5% (5,000 ppmv) for an 8 h time-weighted average (Wilday et al., 2011). Thus, the FLUENT 14.0 model is able to predict approximately the harmful threshold concentration to determine the safety distance.
It should be noted that the developed model in this study is to simulate the mixing of CO2 with air and subsequent dispersion of the toxic cloud within the obstacles. Therefore, the impacts of impurities in CO2 stream (such as hydrogen sulfide) on phase, temperature and pressure during release process were not strictly addressed. Dispersion may differ between pure CO2-air and CO2-H2S-air due to the above impacts (Koornneef et al., 2012). In addition, the conditions of CO2 release such as pressure and temperature drop, phase change and sublimation were not calculated.
| Fig. 6: | Comparison of CO2 volume fraction between experimental data and simulation results at a point of x = 25 m, y = 0 m, z = 0.3 m |
A source term model was developed based on choked conditions to calculate the condition of the CO2 outflow in the near field (Mazzoldi et al., 2008b). Hence, CO2 discharged from a 10 mm hole of a pipeline at 10 Mpa pressure and 3.7 kg sec-1 leakage flow rate. The leakage flow rate is similar with the present study (3.65 kg sec-1). However, the flow conditions during release process are various. For supercritical/liquid CO2 releases, a dry ice bank may be formed in the outflow.
CONCLUSIONS
A 3D model has been developed to simulate the dispersion of pure CO2 from accidental releases using FLUENT 14.0. The realizable κ-ε turbulence model was used to predict the dispersion of pure CO2 instantaneous release from the ground. A wind profile and description of surface roughness were defined at the inlet and the ground boundary respectively through user defined functions. The simulation results have a good agreement with the experiment. FLUENT-CFD can be used as a tool for CO2 concentration prediction in atmospheric release with certain over prediction as a case study of CO2 in the far field.
ACKNOWLEDGMENTS
The authors would like to thank Universiti Teknologi PETRONAS for the support and assistance throughout the study.