Microsoft Word - 35fakandu.docx
CHEMICAL ENGINEERING TRANSACTIONS
VOL. 53, 2016
A publication of
The Italian Association
of Chemical Engineering
Online at www.aidic.it/cet
Guest Editors: Valerio Cozzani, Eddy De Rademaeker, Davide Manca
Copyright © 2016, AIDIC Servizi S.r.l.,
ISBN 978-88-95608-44-0; ISSN 2283-9216
Application of CFD Simulation to Safety Problems –
Challenges and Experience Including a Comparative Analysis
of Hot Plume Dispersion from a Ground Flare
Cristina Zuliani*a, Claudio De Lorenzib, Sabatino Ditalib
a
Saipem SpA, Via Toniolo 1, 61032 Fano, Italy
b
Saipem SpA, Viale De Gasperi 16, 20097 San Donato Milanese, Italy
cristina.zuliani@saipem.com
Integral or phenomenological consequence models are commonly used for safety related studies at onshore
and offshore facilities. These are usually 2D and therefore ignore the influence of the geometry on the
ventilation patterns, the dispersion substances and the generation of turbulence that plays a fundamental role
in case of explosions. More sophisticated Computational Fluid Dynamics (CFD) models can take into account
all these and other relevant phenomena that greatly affect the results. Several design matters can benefit from
the use of CFD models in alternative to the simplified consequence models; these include the dispersion of
dense gases in low wind conditions, the assessment of explosion risk in congested areas, the dispersion of
gases in complex terrains and countercurrent wind, the evaluation of any smoke related impact on plant safety
and efficiency. In this paper, the phenomenon of hot plume dispersion from a ground flare is investigated with
CFD simulations. The results of a comparative analysis between two CFD codes (Fluent and FLACS), applied
to an LNG project, and a phenomenological approach are presented and discussed to identify some peculiar
differences between these models. In addition, the study aims at evaluating the effect two adjacent flare pits in
simultaneous operation.
1. Introduction
LNG facilities often include large ground flares for the safe disposal of large quantities of process gases in the
rare event of emergency situations and/or plant depressurization. One of the major safety concerns related to
this type of installations is the large amount of heat transported by the hot plume. The hot gases emitted from
the flare, due to their high temperature, may pose an hazard to personnel present on elevated platforms and
may lead to degraded performances of some equipment that rely on strict design temperature margins (i.e.
gas turbine air intakes, fin-fan air coolers), especially in LNG plants (Pandya, 2014). For this reason,
dispersion modelling is often performed to calculate the wind induced patterns of the hot plumes leaving the
ground flare, to evaluate the temperature field at specific target points and any interaction with other plant
equipment. Due to the complexity of the phenomenon (crosswind effects, influence of geometry, etc.) CFD
models represent a more reliable mean to perform such analysis and support the engineering team in making
proper design choices.
The purpose of this study is to compare and discuss the results obtained for a large LNG ground flare with two
CFD models: a multipurpose code i.e. ANSYS FLUENT (v. 12) and a specialized tool i.e. FLACS v.10.2
(GexCon). FLACS is developed mainly for safety applications; it is the industry standard for CFD explosion
modelling and is commonly used for modelling flammable and toxic releases. Even though dispersion of hot
combustion gases is not a common application, it is indeed within its range of applicability. Results of a project
study performed for a ground flare of an LNG plant with ANSYS FLUENT (v. 12) are used as a term of
comparison to define the most appropriate set up in FLACS v.10.2 so as to model such phenomenon. The
comparison is based on the iso-surface temperature profile, temperature slice profile and temperature
evaluated at predefined target locations. In addition the behaviour of adjacent flare pits operating
simultaneously is investigated with respect to the same parameters.
DOI: 10.3303/CET1653014
Please cite this article as: Zuliani C., De Lorenzi C., Ditali S., 2016, Application of cfd simulation to safety problems – challenges and
experience including a comparative analysis of hot plume dispersion from a ground flare, Chemical Engineering Transactions, 53, 79-84
DOI: 10.3303/CET1653014
79
Moreover, in order to highlight the main differences and limitations, the same dispersion case form a single
flare has been modelled with a phenomenological proprietary code, DISPGAS (HSE UK, 1996), usually used
to simulate continuous releases from smaller vents / accidental ruptures.
2. Comparative study
2.1 Project case description
The choice of a ground flare system as a design alternative to the elevated flare system configuration for a
large LNG onshore-plant has been evaluated by addressing the potential detrimental effects on personnel and
equipment taking into consideration the temperature mapping at specific locations. A simplified sketch with the
flare dimensions is presented in Figure 1.
The two targets monitored in the study are:
• The gas turbine / power generation area located 400m apart from the flare
• The process air coolers arrays located 670m east and 520m south apart from the flare.
Vertical sampling lines provide information on the temperature trend over the plant’s height, in
correspondence of these two targets. Furthermore detailed 2D plots in correspondence of selected cut-planes
are used to obtain temperature patterns. Also 3D plots of temperature iso-surfaces provide effective views of
the hot plume patterns.
The temperature thresholds considered for the analysis are:
• 70°C for personnel exposure at any elevation (HSE UK, 2013)
• +2°C temperature rise above ambient for efficient operation of air coolers and gas turbine air inlets
(Pandya, 2014).
Figure 1: Ground flare geometry and sampling lines over the plant field
2.2 Scenarios analysed
Flow patterns of the hot plume are mainly affected by wind speed and direction. Based on site specific wind
statistics and preliminary plant layout, the most frequent wind speeds have been selected for the investigation.
The phenomenon is transient as the system operates in case of emergency (e.g. train depressurization) and
for a limited period of time, however conservatively the analysis is carried out considering a constant design
flare load that corresponds to a constant combustion gases discharge rate calculated considering 100%
excess air. Flue gas composition and temperature have been calculated considering complete combustion of
the design release case that consists mainly of methane. Four scenarios are investigated. Table 1
summarises the conditions that have been used in the numerical runs.
Table 1: Conditions used for the scenarios
Case ID Wind direction
Wind velocity
(m/s)
Ambient
temperature (°C)
Discharge rate
(t/h)
Flue gas
temperature (°C)
1 W 7 33 74870 1195
2 W 15 33 74870 1195
3 N-W 7 33 74870 1195
4 N-W 15 33 74870 1195
80
2.3 Modelling approach
The approach used to model the system is based on the following simplifying assumptions:
• the flue gases are thoroughly mixed with entrained combustion air above the flames (at the top of the
flare enclosure). Holding this assumption, the top surface of the flare box has been modeled as an
emitting source of flue-gases with a uniform value of temperature, constant upward velocity and fixed
composition. This has been taken as the initial point for the atmospheric dispersion calculation;
• the mass flow-rate and temperature have been calculated assuming 100% combustion excess air
(respect to the stoichiometric value) and used as input to the CFD model; no combustion chemistry;
• flames are entirely shielded by the flare fences. The possible impairing effects of the plume are only
related to the convective term of the combustion gases.
This same approach was used with both CFD models (FLUENT and FLACS), however some differences in
the computational domain, grid and general set up are highlighted.
In the simulations with ANSYS FLUENT, two different domains were used, based on wind direction: a
1100x900(symmetrical)x500 m with a symmetry plane for the West wind direction; a 1100x1100x700 m for the
North-West wind direction. The numerical grid is an unstructured hexahedral grid.
The boundary conditions applied at the domain faces are the ones suggested by Blocken (Blocken et al.,
2007) so as to guarantee a proper modeling of the wind profile and turbulence parameters in the atmospheric
boundary layer (ABL) which is of paramount importance in determining the plume behavior. A neutrally
stratified ABL (corresponding to the stability class D) is implemented in the study following the subroutines
based on Richards and Hoxey (Richards and Hoxey, 1993). RNG k-epsilon turbulence model is selected.
In the simulations performed with FLACS (GexCon), the domain is 1500x1500x600m. The numerical grid is a
Cartesian grid with cubical 2x2x2m cells in proximity of the flare source. Cells are stretched in the remaining
part of the domain. Wind boundary conditions are defined at the inlet faces: wind speed at a reference height
and Pasquill stability class are the required inputs used to define the stability of the ABL and calculate its
turbulence properties. In FLACS the theory of the characteristic length scale of Monin and Obukhov (Monin
and Obukhov, 1954) is implemented to characterize the stability class. Standard k-epsilon model is used. An
area leak with rectangular shape and dimensions equal to the ground flare section is located in
correspondence of the top surface. The leak is defined as steady state and with a uniform profile across the
section. A dispersion and ventilation simulation set up is used to model the cases. Sufficient time is allowed for
the wind profile to stabilize throughout the domain before the leak is started.
3. Results
3.1 Temperature comparison in correspondence of gas turbine (GT) location – Case 1&2
In case1 and 2, the plume at one of the above-defined threshold temperature can affect only the gas turbine
target located 23m of elevation on the ground level.
FLACS estimates slightly higher temperatures than FLUENT both at height and at ground level. Differences
are in the range of max 5%.
Similar behaviour of the plume can be observed. The main difference is identified in the top view of the iso-
surface temperature profile (Figure 2): FLUENT predicts a bifurcated plume while in FLACS this behaviour is
not so evident in the temperature plot but it is clear from the velocity streamlines (Figure 3). Plume bifurcation
is a well-known phenomenon (Ponchaut et al., 2012) that occurs in certain weather and terrain conditions
when the plume enters into a cross flow (i.e. wind) giving rise to counteracting vortices. This difference is
probably due to the different constant of the k-ε turbulence model in the equation of the dissipation rate and
the description of the inlet wind turbulence.
In case 2 the wind has a higher bending effect on the hot plume: this remains close to the ground for longer
downwind distances.
For both scenarios FLACS predicts higher temperatures at large downwind distances from the flare. +2°C
temperature contour extends more than in FLUENT results. However conclusions are unvaried.
Table 2: Comparison of FLACS vs. FLUENT temperature readings for CASE 1 and CASE 2
CASE 1 – W 7 m/s CASE 2 – W 15 m/s
FLUENT FLACS FLUENT FLACS
70°C temperature on GT at 400m from flare Not reached Not reached Reached Reached
Max downwind distance of 70°C contour from
flare (reached at height)
600m at 220m 380m at 160m 800m at 180m 550m at 115m
Max T reached at height 325 K at 205m 334 K at 226m 354 K at 105m 354K at 87m
T reached at 23m height at GT 307K 316K (+3%) 329K 345K (+5%)
81
70°C
FLACS
70°C
FLUENT
Figure 2: Case 1 - Wind from West; Wind Velocity=7m/s –70°C temperature iso-surface
Figure 3: Case 1 - Wind from West; Wind Velocity=7m/s – Velocity streamline
FLACS
FLUENT
Figure 4: Case 1 - Wind from West; Wind Velocity=7m/s (+2°C temperature respect to the Tamb threshold Pic 1
at 23m height AC, Pic 2 lateral view)
3.2 Temperature comparison in correspondence of air coolers (AC) location – Case 3&4
In case 3 and 4, the plume at one of the above-defined threshold temperature can affect only the air coolers
array located in elevation. FLACS estimates pretty much the same temperatures as FLUENT both at height
and at ground level. In correspondence of the selected target differences are in the range of 1% and however
are very close to ambient value (306K).
Slightly different plume behaviour is observed: FLUENT predicts iso-surface plume bifurcation while FLACS
predicts a more uniform iso-surface temperature of limited extension with respect to FLUENT. In addition to
the points previously highlighted, this may be related also to grid refinement that may affect vortex/turbulence
prediction in the far field. FLACS predicts a slightly wider +2°C temperature profile at ground level but overall
results are quite similar and same conclusions can be drawn.
Table 3: Comparison of FLACS vs. FLUENT temperature readings for CASE 3 and CASE 4
CASE 3 – NW 7 m/s CASE 4 – NW 15 m/s
FLUENT FLACS FLUENT FLACS
70°C temperature on AC at 500m from flare Not reached Not reached Not reached Not reached
Max T reached at height (AC) 317K at 275m
325K at 400m
317K at 362m 322K at115m 317K at 192m
T reached at 23m height at AC 306K 308K (+0.5%) 306K 310K (+1%)
82
70°C
FLACS
70°C
FLUENT
Figure 5: CASE 3 Wind from North West; Wind Velocity=7m/s –70°C temperature iso-surface
FLACS
FLUENT
Figure 6: CASE 4 Wind from North West; Wind Velocity=15m/s – (+2°C temperature respect to the Tamb
threshold at 23m height AC)
3.3 Analysis with a phenomenological model (DISPGAS)
The phenomenological code DIPSGAS has been applied to the single flare pit considering an equivalent
circular source of 160m diameter at 16m above ground level. The same cases were screened with the
characteristic that W and N-W wind directions make no difference due to the symmetry. The results given
below show a much shorter distance and higher elevation reached by the 70°C contour respect to the
distances evaluated with the CFD models. Target locations are not reached by the plume.
Table 4: Results of DISPGAS for CASE 1 and CASE 2
CASE 1 CASE 2
Max downwind distance of 70°C contour from flare (reached at height) 163m at 301m 243m at 160m
T reached at 23m height at target distance 305K at 400m 306.3K at 400m
4. Effect of adjacent flare pits operations
In many plants more than one flare pit can operate simultaneously. The effect of two adjacent flare pits (40m
separation distance) is investigated with FLACS for the same scenarios listed in Table 1. Results in
correspondence of targets are reported in Table 5. Comparison of system behaviour for CASE 1 is shown in
Figure 7. Overall the plume behaves as if it originates from a single larger flare; this is due to the limited
separation distance which is responsible for the interaction of the vortices originating from the adjacent flares.
Their interaction, especially in the low wind scenarios, generates a single longer and wider plume. In this
specific case the presence of an adjacent flare does not alter the conclusions of the analysis.
Table 5: Temperatures results of FLACS for two adjacent flares
ADJACENT FLARES CASE 1 CASE 2 CASE 3 CASE 4
70°C temperature at target (GT/AC) Not reached Reached Not reached Not reached
Max downwind dist. of 70°C contour from flare 540m at 128m 610m at 43m 400m at 128m 510m at 81m
Max T reached at height - GT/AC monitor points 331K at 102m 348K at 65m 324K at 226m 318K at 119m
T reached at 23m height 321K 345K 309K 312K
83
Figure 7: Comparison of CASE 1 results – Single vs Adjacent flares (Pic 1&2 70°C iso-surface; Pic 3&4 70°C
temperature side view; Pic 5&6 +2°C contour respect to the Tamb at 23m height; Pic 7 velocity streamlines)
5. Conclusions
Hot plume dispersion from a ground flare has been investigated with two CFD models: ANSYS FLUENT and
FLACS and compared also with the results of a simpler model DISPGAS. The study presents results of the
iso-surface temperature profile, temperature slice profile and temperature evaluated at predefined targets.
Even though the two CFD models are based on slightly different approaches, results are in relatively good
agreement and conclusions are the same. Temperatures at specific target locations differ no more than 5%.
The profile of the +2°C temperature rise above ambient extends a bit more in FLACS. On the other hand the
extension of the 70°C temperature profile is slightly smaller in FLACS.
Possible reasons for these differences in the results are:
• Turbulence model: strength of buoyancy production in the transport equation of the turbulence
dissipation rate is different; in FLACS there is less production of turbulence dissipation (more
turbulence), therefore more mixing, that in the lower layers, at temperature close to ambient leads to
a larger extension of the +2°C temperature rise above ambient, but at the same time leads to a
shorter 70°C iso-surface;
• Inlet wind turbulence conditions; this is responsible for the length of the plume in particular at large
distances downwind;
• Grid resolution.
Overall the differences between the results of the two CFD models are minimal and main conclusions are not
affected. On the other hand, DISPGAS shows a more buoyant plume probably due to fact that effect of
geometry (flare fence) is not considered and the different way wind turbulence is modelled.
The simultaneous operation of adjacent flares shall always be investigated as the interaction of the hot gases
may produce longer and wider plumes leading to larger areas affected by the temperature increase at ground
level or at sensitive locations.
References
Blocken B., Stathopoulos T., Carmeliet J., 2007, Atmospheric Environment vol. 41, CFD Simulations of the
Atmospheric Boundary Layer: Wall Functions Problems, 238-252
HSE UK, 1996, Evaluation study of models used in predicting smoke and gas ingress on offshore structures,
OTH 95 498
HSE UK, 2013, Indicative human vulnerability to the hazardous agents present offshore for application in risk
assessment of major accidents, SPC/Tech/OSD/30,
accessed 26.02.2016
Monin A. S., Obukhov, A. M., 1954, Basic laws of turbulent mixing in the surface layer of the atmosphere, Tr.
Akad. Nauk SSSR Geofiz. Inst 24, 163–187
Ponchaut N. F., Kytoomaa H. et al., 2012, Modelling of ground flare pits, 12th Spring meeting & 8th global
congress on process safety
Pandya H., 2014, Consider factors affecting onshore LNG plant design, Gas processing
accessed 26.02.2016
Richards P.J., Hoxey R.P., 1993, Journal of Wind Engineering and Industrial Aerodynamics 46-47,
Appropriate Boundary Conditions for Computational Wind Engineering Models Using the k-ε Turbulence
Model
84