The study case consists of a pipe, 6 m in length and 600 mm in diameter with a partially closed square –
knife gate valve installed 3 m away from the inlet side. The section is taken from a pipeline 37 meters
away from a reservoir. The pipe continues downstream the valve for 2 meters and then connects with a
bend as shown in figure 3.10.
The fluid domain of the pipe and valve interior were modeled using Rhinoceros 3D. An extension of 1
meter was added to the pipe at the outlet for flow stability and to prevent reverse flow at an early stage of
Critical areas in the fluid domain geometry required mesh refinement. More cell faces were generated
at these locations.
CFD is a numerical method that discretizes the Navier Stokes equations. The discretization is applied by
dividing the fluid domain into finitely small discrete blocks, the operation is called meshing.
There are many methods to mesh three-dimensional models. The accuracy of the simulation and its
convergence is sensitive to the skewness, aspect ratio and orthogonal quality of the mesh’s cells.
Structured meshes are highly recommended for accuracy and convergence.
The cut-cell method was adopted in this study to generate hexahedral isotropic mesh cells and ensures
accuracy and speed.
Two meshes were used for the LES and the RANS simulation, both cases were processed in ANSYS
meshing tool using the Cut-Cell method. The geometry was imported into Workbench as a “.STEP”
extension file and it was then imported into ANSYS meshing tool.
Using the properties window the minimum and maximum size of elements was manually selected, and the tessellation refinement was
The following table lists the statistical input data for the LES and the RANS meshes:
3.3 ANSYS Fluent – Pre-processing
Before running the LES model the case was solved using the K Epsilon model.
The boundaries of the fluid domain (Inlet/outlet) were assigned in the meshing tool, saved as a mesh file
that is compatible with Fluent and then imported.
Transient time was selected from the general menu in Fluent and the standard k-ε model was assigned with the default model constants for the transport
Water was selected as the main fluid for all cases.
Two types of boundary conditions were selected, a mass flow rate of 255kg/s and a pressure of 86 KPa
were assigned respectively to the inlet and outlet boundaries. The mass flow rate was taken as an
average value from the Ultrasonic metering data. The Reynolds number was computed according to the
The solution method selected is the pressure-velocity coupling using the SIMPLE scheme, an iterative
algorithm that solves the discritized momentum, the pressure correction and the transport equations.
Spatial discritization were set to second order upwind for the momentum, turbulent kinetic energy and
the turbulent dissipation rate in the K-ε model and then later changed for the LES case to bounded
For the following simulation, the under-relaxation factors for pressure and momentum were assigned
respectively as 0.4 and 0.5. It is recommended to decrease the under-relaxation factor for the momentum
equation when facing convergence difficulties. Data files were assigned to be generated every 1-time step to be post-processed on Post-CFD from ANSYS.
The total time of the introductory RANS simulation was 0.3s with a time step of 0.1s. The data file
generated in the last time step was edited and switched to LES method. Statistical data sampling was
activated to analyze the unsteady statistical mean and root square mean velocities of the flow. The total
length of the simulation was 12 seconds with a time step of 0.01 second, computations took 10 days to
be completed with the use of 10 processors and 8GB of memory in average. A separate full RANS
simulation (K-ε model) was completed for the same time length with a time step equal to 0.1 seconds.
The residual error for both methods was set at 1.10-5
for the velocities in the LES and RANS case and
for the turbulent kinetic energy and turbulent dissipation in the RANS case.
4.1 Velocity and pressure fields
Velocity magnitude and pressure contours from the RANS and the LES simulations are displayed below for comparison at different time steps:
The following slides show the velocity magnitude and the pressure contours in a plane section taken at the pipe center and along the pipeline starting from y = 1m from the pipe inlet to y=6m at the pipe outlet.
At 1.5 s the velocity downstream the gate valve increased and reached its maximum value of 3.5 m/s as shown in figure 4.10 (LES Case). In contrast, the maximum velocity registered in the same area by the RANS model was 3.1 m/s as shown in figure 4.11. This increase in velocity is due to the restriction in the cross-sectional area which also decreased the pressure in the area.
The downstream flow exhibited turbulent eddies that were captured by the LES model. similarly, in the RANS model eddies were exhibited by an extended recirculation at the upper part of the pipe. Both observations were recorded at a time equal to 3s (displayed in figure 4.12 and 4.13). Between the period of 5 to 12 seconds, the flow maintained a large recirculation that extended 3 meters away from the valve. In contrast, the LES model captured the large eddies circulating and separating from each other traveling along the upper part of the pipe during the whole simulation run-time with observable time-dependent changes.
The following slides show the velocity vectors in the recirculation regions in LES and RANS simulations respectively at a time equal to 12 seconds:
4.2 Statistical Data
The time required for a particle to reach the pipe’s outlet is 5 seconds. Based on that time the unsteady statistical data of the mean filtered velocity and the root mean square velocity were extracted at t = 12 seconds. Cross section planes were drawn in the fluid domain downstream the valve where turbulence intensity was compared between the RANS model and LES based on the average value of the turbulence intensity in the whole section plane.
Turbulent intensity is a factor that indicates the severity of turbulence in the flow.
The cross-sectional planes were selected at y=0, 0.5, 1, 1.5 and 2 meters downstream the valve. The mean velocity values were extracted through data sampling from the LES simulation and were calculated automatically by the RANS method as shown in figure 2-10.
Studying the velocity profiles in the downstream and upstream sides of the valve validates the quality of the mesh and the effectiveness of the near wall function used in LES.
Two lines, wall to wall were drawn in two different planes, the first cross-sectional plane was created 2 meters in the upstream side of the valve and the second one 2 meters downstream, four plots were produced.
4.3 Results Analysis
The results obtained from the study case in two different simulation methods both showed an intense sudden pressure loss caused by the gate valve as shown in figures 4.10 to 4.21. The static pressure upstream changed slightly due to friction loss with the wall and then dropped suddenly by 4000 Pa on average just downstream the valve. Pressure then stabilized further down the pipe reaching 86800 Pa at y = 1.5 m. The velocity field upstream the valve was characterized by a developed turbulent flow as shown in the velocity profiles for both RANS and LES cases in figure 4.28 and 4.30 conforming with the power law profile predicted in turbulent flows. The velocity field was suddenly skewed in the downstream side of the valve where a separation of flow was observed in the RANS case between t = 5 to 12 seconds with a large recirculation in the pipe’s upper part as shown in figure 4.21 and 4.24. As for the LES case, the turbulence in the flow was detected with more precision by capturing large eddies in the pipe in the downstream side of the valve as shown in figures 4.14, 4.16, 4.18 and 4.20 between t = 5.5 seconds to t= 12 seconds. The LES model as predicted was more accurate in capturing the eddies due to its capability of filtering the small scales and resolving the large ones giving an accurate representation of the nature of the flow.
The RANS (K-ε model) is a time-averaged method that models turbulence statistically, hence, the numerous circulations in the upper side of the pipe were not detected by this model. .
The average turbulent intensity on both simulations showed a very high level of turbulence in the downstream section of the valve which exceeded 30 % and in advanced locations it reached high levels up to 60 % as shown in the LES case proving the existence of high-velocity fluctuations from the averaged mean filtered value.
Figure 4.29 represents an asymmetric velocity profile down-stream the valve in the LES case. The first section of the profile is from z = 0 to z = 0.38 m where the velocity’s amplitude reached 2.20m/s and then a recirculation appeared from z = 0.38 to z = 0.43m due to a negative value in the y velocity. The second part showed an increase in the velocity between z = 0.43 to 0.55 m with an amplitude of 0.75 m/s. These variations in the velocity profile suggest large differences in the velocity between the two sides of the pipe’s wall and this is mainly caused by the gate valve which bounded the flow through a constrained area and then released it back to a wider area.
Figure 4.31 represents the y velocity profile in the RANS model showing clearly a flow separation pattern.
The simulations completed for this study showed that turbulence intensity levels downstream were high (30 to 60 %), an analysis for its intensity concluded that up to 2 meters away from the valve and just at the inlet side of a bend, turbulence did not decay.
High levels of turbulence and the presence of vortices explains the different velocity readings at separate locations. The valve contributed in the amplification of turbulence and creating swirls ahead downstream.
To avoid swirl formation, it is recommended to keep a comfortable distance between any 2 fittings allowing turbulence to naturally decay.
The LES simulation provided better results in predicting the behavior of the flow with respect to time and that was evident in the showcase presented where larger eddies were captured. This method is preferable for in-depth analysis and to acquire a more realistic perception of the flow’s turbulent nature.
Although LES is more advantageous than RANS method, it is important to note that it is much more expensive and more difficult in handling meshes with appropriate near wall damping functions.
The implementation of Van Driest’s near wall damping function is recommended to improve the result of the simulation in addition to a better refinement of the mesh specifically near the boundary layer. For a better understanding of the relationship between high turbulence and its effect on the measurement data the study case herein should be expanded to include a significant section of the pipe downstream with all bends and fittings included.
The gate valve modeled in this simulation has an irregular profile (Figure 3.12) due to corrosion, it is also recommended to make a comparative study between normal and corroded valves to study the effect of corrosion on the behavior of the flow.
: Further Studies of Flows and Balances at Mitcheldean Waterworks, Gloucestershire, Dr. Richard Furness.
: An introduction to computational fluid dynamics, the finite volume method, second edition,
K Verteeg and W. Malalausekera, p.41.
:http://www.mit.edu/course/1/1.061/OldFiles/www/dream/SEVEN/SEVENTHEORY.PDF figure 2.
: About Boussinesq’s turbulent viscosity hypothesis: historical remarks and a direct evaluation of its validity, Francois G. Schmitt. CNRS, FRE 2816 ELICO, Wimereux Marine Station, Universit´e des Sciences et Technologies de Lille – Lille 1, 28 av. Foch, 62930 Wimereux, France.
: An introduction to computational fluid dynamics, the finite volume method, second edition,
K. Verteeg and W. malalausekera p.75 equation 3.45 and 3.46
: Fluent 6.3 User’s guide 12.9.3 Subgrid -Scale Models.
: Survey map by Severn Trent Water Ltd.
: A cut-cell non-conforming Cartesian mesh method for compressible and incompressible flow,
J. Pattinson, A. G. Malan and J. P. Meyer. Department of Mechanical and Aeronautical Engineering, University of Pretoria, Pretoria 0002, South Africa, International journal for numerical methods in engineering, 2007; 72:1332–1354.
: J. Pattinson, A. G. Malan and J. P. Meyer. Department of Mechanical and Aeronautical Engineering, University of Pretoria, Pretoria 0002, South Africa, International journal for numerical methods in engineering, 2007; 72:1332–1354, figure 1.
: International Journal of Heat and Fluid Flow 24 (2003) 147–156, Reynolds averaged simulation of unsteady separated flow, G. Iaccarino, A. Ooi, P.A. Durbin an M. Behnia