CFDModellingof Rotating Annular Flow Using Wall Y
CFDModellingof Rotating Annular Flow Using Wall Y
CFDModellingof Rotating Annular Flow Using Wall Y
net/publication/336814490
CITATIONS READS
4 595
2 authors:
1 PUBLICATION 4 CITATIONS
Swansea University
35 PUBLICATIONS 1,430 CITATIONS
SEE PROFILE
SEE PROFILE
All content following this page was uploaded by Salim M. Salim on 18 May 2020.
m.s.salim@dundee.ac.uk
Abstract: This project establishes a strategy of accurately modeling rotating annular flow
of drilling fluid to improve the numerical predication of pressure loss in an
annulus. Pressure loss is vital within several engineering applications from
HVAC design to oil & gas drilling. By being able to accurately predict this
through numerical methods it creates the potential for innovation and
efficiency. The project will build on previous recommendation of wall y+ by
Salim et.al [1] that looked at high Reynolds number turbulent flow for the
predication of wall bounded flow. A strategy was established with the aid of
the wall y+ value to investigate the most suitable turbulence model in ANSYS
FLUENT to create a method that will reduce time and costs in the
development of drilling tools. Out of 5 turbulence approaches, the k – ω
model was found to be the most accurate for a wall y+ of less than 5. The k – ε
model performed least well and its was observed that there was a direct link
between the turbulent intensity found in the annulus and the performance of
the turbulence model. The k – ε was found to over predict the turbulent kinetic
energy for the mesh set-up and thus contributed to inaccurate results regarding
the pressure loss in the annulus. This project, therefore, suggests that a
structured mesh with a y+ < 5 and the k – ω turbulence model will provide
sufficiently accurate data in the investigation of pressure loss in an annulus.
This will provide benefit to the industry and to researchers who wish to model
this flow situation where experimental data is not available. The strategy can
be used by design engineers to create drilling tools and allow them to try more
experimental designs, without the need to build expensive and time-consuming
prototypes. It may also be used as an investigation tool for researchers wishing
to gain a greater understanding of the complex fluid flow that occurs during
rotating annular flow.
Key Words: Annular Flow, ANSYS, CFD, Drilling, Rotating Flow, Wall y+.
2 Chapter #
1. INTRODUCTION
With the recent downturn in the oil & gas industry [2,3], innovation and
efficiency are needed more than ever to reduce costs. An area where time
and money can be significantly saved is during the development of drilling
tools; which are used to improve the overall drilling performance. While
tools are intended to enhance drilling efficiency, the negative impact they
have must also be known and investigated during the development stage of
the tool. Maintaining downhole pressure to within the required window is
currently a major challenge for engineers, especially in horizontal and
extended reach (ERD) wells [4]. It is, therefore, vital that the effect the
drilling tool will have on the pressure loss within the annulus is known
during the development stage of the product, so that its performance in
actual drilling operations is better understood. This can be done through
creating a prototype of the product and testing it through an experimental
set-up, however, this can be costly and time-consuming. Computational
Fluid Dynamics (CFD) is a method to overcome this problem by
computationally modelling the product and its effect on the flow properties.
By using the wall y+ as a tool for selecting a suitable mesh and turbulence
model combination, the need for validation through data is removed. This
allows many different flow situations to be modelled without the concern of
getting suitable data to verify the results and in turn makes CFD an attractive
option, not only for product design and development, but also for future
research.
One of the key issues within the industry today is the effective
management of the Equivalent Circulating Density (ECD) of drilling fluid
[4]. ECD is the desnsity exerted by a circulating fluid against the formation
and takes into account the pressure drop above the point being considered. It
is vitial in avoiding kicks, especially in wells with a norrow window between
fracture gradient and pore-pressure gradient [5]. Annular frictional pressure
loss strongly affects ECD and hence if this can be controlled it will aid in the
ECD management. Maintaining control of downhole pressure is also vital to
the safety and successful drilling of a well, this is therefore a significant area
within the oil & gas industry. Experimental studies have taken place to
evaluate annular pressure loss and it has been found that the rotation of the
drill pipe has a significant effect on the pressure loss [6,7]. While
experiments can effectively investigate the effects of rotation some may be
time-consuming to create and costly to operate, depending on the flow
scenario. CFD could allow for simulations to be carried out, reducing the
time and cost, compared to those found when experiments are conducted.
CFD also provides the added benefit of carrying out many different flow
scenarios by simply changing the computational domain and set-up. One of
#. CFD modelling of rotating annular flow using wally+ 3
the reasons CFD may not be implemented is due to the time taken to set-up a
numerical study and the ability to validate it. The need to verify CFD
simulations removes the appeal of this technology. Therefore, there is a need
for a fast, reliable modelling strategy to allow efficient analysis of drilling
tools and remove the need for validation. This strategy gives confidence in
predicting accurate numerical results for this flow situation.
Annular frictional pressure loss occurs due to the movement of the
drilling fluid and cuttings through the annular space. This incorporated with
the rotation of the drill pipe, which would be experienced during drilling
operations, creates a complex flow situation due to the secondary flow and
the formation of Taylor Vortices [8,9]. This project, which will expand on
the publication by Davidson & Salim [10], uses CFD to model a horizontal
section of a well and investigate the effects drill pipe rotation has on a non-
Newtonian power-law fluid. A strategy will then be suggested for selecting a
mesh configuration and turbulence model when experimental data is not
available with the aid of the wall y+.
This will be achieved by replicating experimental data by McCann [11]
in ANSYS FLUENT and investigating the following five turbulence models;
k – ω, k – ε, k – ε enhanced wall, Spalart- Almaras and RSM. The most time-
consuming section of a CFD study can be generating a suitable mesh that
captures the correct resolution; especially due to the impact of walls in wall
bounded flow [12]. The most conventional method, known as a grid
independence test, is to run many simulations with different mesh sizes and
configurations until the results match experimental data. This removes one
of the main advantages of CFD compared to experiments by increasing the
time taken to complete a numerical simulation. The y+ can be used as
guidance for developing a reliable mesh and turbulence model strategy. By
removing the need and time for validation and a grid independence test the
main advantages of CFD are restored.
2. PREVIOUS WORK
when tools are being designed for a specific well where there is no previous
data available or when a variation of a drilling fluid is being investigated.
Salim and Cheah [1] investigated a strategy for dealing with 2-D wall
bounded turbulent flows using the wall y+ as guidance for mesh
configuration and the most suitable turbulence model. Walls have a
substantial impact on turbulent flow and hence the mesh in this area must be
refined sufficiently to obtain an acceptable solution. The quality of the mesh
at a wall can be checked by the y+ value which is a dimensionless number to
represent the distance from a wall to the centre of the nearest cell.
The main applications for using the computed wall y+ as guidance in
selecting the appropriate mesh density and corresponding turbulence model
are situations where reliable experimental data are not available to validate
CFD models. The investigation found that a wall y+ value in the range of 30-
60 provided acceptable results for relatively high turbulent flows. They also
suggest the mesh should not be within the buffer region as neither the near
wall treatments nor wall function is able to solve it accurately and thus the
overall solution is inaccurate. This paper shows the effectiveness of using
the wall y+ as a tool to assist in selecting a suitable mesh and turbulence
model combination. The paper highlighted the time taken to carry out a grid
independence study and therefore the need for developing a meshing strategy
to reduce this time. The results show that the best combination of mesh
structure and turbulence model depend on the flow scenario and the property
being investigated. This paper has been useful within several different
industries, including wear on turbine components and heat transfer of
refrigerant, and has been cited over 165 times for research and investigation
studies.
Ariff et.al [16] built on this work and extended the investigation to 3-D
turbulent flows over a cube by using the y+ as guidance. The study was
divided into two parts for low and high Reynolds numbers. For the low
Reynolds number study, a y+ > 30 was unable to be investigated as it gave a
poor mesh resolution. For this part of the study, the Spalart- Allmaras was
found to be the most suitable for predicting the reattachment when compared
to the theoretical data. The second part of this study was for a higher
Reynolds number of 40,000. The y+ value was approximately 33 and thus
solving in the log-law region of the turbulent boundary layer. It is found that
most of the RANS turbulence models provide results to an adequate
accuracy with some performing better for certain situations such as
separation and re attachment. The work on wall y+ from both these papers
served as guidance for this project.
This project will differ from the previous work by investigating the flow
of a non-Newtonian fluid in a rotating annulus, using the wall y+ value to
#. CFD modelling of rotating annular flow using wally+ 5
obtain accurate results by selecting the most suitable turbulence model and
mesh set-up.
3. METHODOLOGY
For this project, a 3D numerical study was carried out using ANSYS
FLUENT v14.5 to replicate the experimental conditions by McCann [11].
McCann investigated the effect drill pipe rotation had on the pressure loss
within the annular space. Five combinations of RANS turbulence models
and near-wall treatments are tested to identify the most appropriate pairs.
The results are then compared to the experimental results using wall y+
values to aid in the selection of the most suitable model and mesh
configuration.
tube of 38.1mm diameter. This set-up, Figure 1, allows for the annulus to be
concentric or fully eccentric while the motor can produce rotation speed of
the drill pipe up to 900 rpm. The pressures are obtained by two pressure taps,
1.22m apart, at each end of the annulus. A variety of fluids, pipe rotation
speeds and annulus alignments were tested in this paper. The focus on this
project will be on increasing pipe rotation for the concentric annulus on a
non-Newtonian fluid as this relates to drilling conditions. Rotating annular
flow is not only applicable to oil & gas drilling and could also be applied to
turbines and components where fluid is used as a lubricant. The fluid is
denoted as Fluid B in the paper and its properties are detailed in table 2.
Figure 2 portrays the computational domain used for the CFD study. As
the fluid flow in the annular space is being modelled this is the only region
that needs to be created, the outer face of the cylinder represents the
stationary wellbore while the inner face represents the rotating drill pipe.
The computational domain replicates the experiment set -up.The length of
the annulus is created to ensure fully developed flow. Following
recommendations by Sorgun et.al [13] the length required for fully
developed flow is found through equation (1).
(1)
Where RePL is the Reynolds number for a Power – Law fluid which is
found by equation (2)
(2)
The boundary conditions are set to match the experiment, with the flow rate
converted to 0.9055m.s-1. The boundary conditions are summarized below in
table 3.
4. MESH
As was the case in the study by Ariff, the y+ value available for
investigation was determined by the Reynolds number. The low Reynolds
number found in this project restricted the uses of a y+ value to only less than
5. For this reason, the 5 turbulence models listed in table 1 were all
investigated to determine the most suitable for a mesh of this type. To create
a mesh with a y+ < 5 it was refined
at each of the two walls. A
structured mesh was created with
the use of the various tools in
ANSYS fluent to give a greater
refinement at the wall, the area
where the fluid is strongly
impacted by the boundary layer.
Figure 3 displays the mesh cross
section of the annulus.
The generated mesh produced a small y+ value due to the low Reynolds
number produced with the current boundary conditions. As can be seen from
Figure 4, the y+ value begins at around 1.2 at the inlet but decreases to less
than 0.2 for the remainder of the pipe length. The structured mesh produces
identical y+ value for the walls of the well and the drill pipe. A wall y+ value
of < 5 indicates that the mesh resolution captures all 3 layers of the boundary
layer created by the wall.
1.2
Wall Y Plus Drillpipe
0.8
Y+
0.6
0.4
0.2
0
0 0.5 1
Z [m]
Figure #-4. Wall y+ value for both walls
#. CFD modelling of rotating annular flow using wally+ 9
drill pipe creates a complex flow situation that replicates turbulent flow. For
this reason, the turbulence intensity was investigated to analyse the result of
the turbulence models, as shown below in table 4 & 5 for 200 & 800 rpm
respectively to show the effect of increasing rotation speed.
1 2 2 2 2
𝑢′ = 𝑢′ + 𝑢′𝑦 + 𝑢′𝑧 = 𝑘 (4)
3 𝑥 3
The above equation clearly shows that the turbulent velocity fluctuations,
and hence the turbulent intensity, are dependent of the turbulent kinetic
energy k. The turbulent kinetic energy for both models were retrieved for the
same location in the annular space at rotation speeds of 800RPM. The
contours of turbulent kinetic energy were viewed through CFD post and the
data was exported as shown in Figure 6.
Figure #-6. Kinetic energy in the annulus for both turbulence models
#. CFD modelling of rotating annular flow using wally+ 13
6. PROPOSED STRATEGY
The frictional pressure loss occurs due to the dynamic movement of the
fluid. This is caused by the mean flow of the fluid and the secondary flow
created by the rotation of the drill pipe. The turbulent intensity was
investigated which is a ratio of turbulent velocity fluctuations and the mean
velocity. On examination of the turbulent intensity it was found that a
relationship occurred between the worst performing models and the
magnitude of the turbulent intensity. To verify this, the turbulent kinetic
energy for each model was compared. It was verified that the k – ε model
predicted a higher turbulent kinetic energy and thus higher turbulent velocity
fluctuations, giving a larger turbulent intensity and an over predication of the
annular pressure loss.
The results and analysis from this flow situation determine that the k – ω
turbulence model with a y+ of less than 5 would be the most suitable
combination for obtaining accurate annular pressure loss values within a
rotating annulus for non – Newtonian fluids. The proposed strategy is
displayed is table 6.
7. CONCLUSION
This study has displayed the use of the wall y+ as an effective tool in
selecting the most suitable turbulence model and mesh configuration for
predicting the pressure loss in a rotating annulus. Based on previous work by
Salim and Cheah [1], this project utilizes the wall y+ value as a method for
creating a reliable meshing strategy for rotating annular flow in the oil & gas
industry. The analysis of the turbulence models within ANSYS FLUENT
has allowed a strategy to be recommended for predicting the pressure loss in
a potentially faster and more cost-effective manner than if it was to be found
through experimental means. This project suggests a highly structured mesh
with a y+ value of less than 5 and the k – ω turbulence model. Due to the
difficulties drilling engineers face with ECD management, especially in
ERD wells, it is vital that the positive or negative impact tools have on this
are known. The use of this strategy will allow designers of drilling tools to
gain an understanding of how their tool will impact the pressure loss in an
annulus during the development stage, thus reducing the cost of expensive
prototypes and experimental testing before the final design is created. By
using the wall y+ value as guidance in selecting a mesh and turbulence model
combination, the need for a grid independence test and validation is
removed. This restores the flexibility and time saving advantages of CFD
when compared to experiments, and aids towards adding innovation and
efficiency to both industry and academia.
REFERENCES