Week 9 - Parametric study on Gate valve.

Abstract:
The flow of water (at 20∘C) through a gate valve is examined for increasing stem travels (valve openings). The study is parametric with stem travel as input parameter and volume flow rate, flow factor & flow coefficient as output parameters in ANSYS Workbench. The simulations are carried out with commercially available CFD tool ANSYS® Fluent® 2021 R2 Student version.

Introduction:
A gate valve, also known as a sluice valve, is a valve that opens by lifting a barrier (gate) out of the path of the fluid. Gate valves require very little space along the pipe axis and hardly restrict the flow of fluid when the gate is fully opened. Gate valves are used to shut off the flow of liquids rather than for flow regulation. The gate valve geometry is shown below.

Geometry:

• The valve inlet & outlet faces are extended in ANSYS Spaceclaim. This is so that the inflow velocity profile is parabolic and outflow conditions are captured adequately. The resulting fluid volume is extracted as shown below.

• The pipe diameter is 100 mm so varying the opening from 10% to 80% corresponds to stem rise from 10 mm to 80 mm. The stem travel is parameterized in Spaceclaim and can be seen in the parameters tab of Workbench.
• Changed domain geometry & fluid domain (blue region) for each design point is shown below.

Computational domain:

• The mesh is fine with an element size of 10 mm for each design point. The no. of cells change for each design point but the refinement level remains more or less the same. The mesh (for 10 mm gate rise) & mesh settings are as shown below.
• Inlet & outlet faces are named so that fluent can apply wall Boundary conditions on these surfaces.

Numerical model:
Turbulence model:
For reduced computational effort RANS based Realizable k−ε turbulence model is used with scalable wall functions for near-wall modeling. Scalable wall functions enforce the usage of the log law in conjunction with the standard wall functions approach even in the range 11.225<y+<30. This helps avoid problems of successive refinements in standard wall function meshes.

Solution method:
The solution procedure is iterative and is based on coupled scheme for Pressure-Velocity coupling. The discretization is 2nd order for pressure and 2nd order upwind for other variables. The gradient is computed using the Rhie-Chow distance-based method. Commercially available CFD tool ANSYS® Fluent® 2021 R2 Student version is used which has a limit of 512,000 cells in the mesh.

Boundary Conditions:

Boundary conditions applied in fluent are summarized in table below.

Boundary	Type	Momentum B.C.
Inlet	Pressure inlet	Constant pressure
Outlet	Pressure outlet	Constant pressure
Inner walls	Wall, Stationery, No-slip	-

Solver settings:

• The mach number of flow (0.142/343≈10−4) is less than 0.3 hence steady-state pressure-based solver is used with gravity enabled (−9.81m/s2 in Zdir).
• Realizable k−ε model with scalable wall treatment is used for capturing turbulence.
• The simulations were done for 300 iterations after standard initialization from the inlet.
• Mass flow rate at the outlet is made an output parameter.
  

Initial simulation:

• The residual and mass flow rate plot for the case with 80 mm gate rise is shown below. It can be seen that mass flow rate converges after about 250 iterations and residuals show repetitive patterns hence all simulations were carried out for 300 iterations.
• Convergence plots are similar for all cases hence in the next section only pressure contours are shown.

Post-Processing:

Flow factor and Flow coefficient

Flow coefficient and flow factor values are used as a standard method of comparing valve capacities and sizing valves for specific applications and are widely accepted by the industry. The flow coefficient of a device is a relative measure of its efficiency at allowing fluid flow. It describes the relationship between the pressure drop across a valve or other assembly and the corresponding flow rate. Mathematically,

CV=Q√SGΔP

Where,

Q=Volumetric flow rate, in gal/min

SG=Specific gravity of fluid

ΔP=Pressure drop across valve, in psi

Flow factor is exactly the same as flow coefficient but is defined in S.I. units instead of Imperial units. Flow coefficient is used in U.S. while Flow factor is used everywhere else. A conversion between the two values can be done using,

KV=0.865⋅CV

To compute these values, expressions are defined in ANSYS CFD-Post and then parameterized as output values. Since the simulations are done in S.I. units firstly flow factor is calculated followed by flow coefficient using expression definitions as shown below.

Pressure contours

10 mm 20 mm

------------------------------------------------------------------------------------------------------------------------

30 mm 40 mm

------------------------------------------------------------------------------------------------------------------------

50 mm 60 mm

------------------------------------------------------------------------------------------------------------------------

70 mm 80 mm

------------------------------------------------------------------------------------------------------------------------

Table of design points

Chart plots

Inferences:

• The negative value of mass flow rate simply indicates that mass is flowing out of our domain which gets more negative with gate rise as expected.
• From the pressure contours, it can be seen that pressure everywhere is much above the vapor pressure of water (at 20∘C). This is desirable as below vapor pressure cavitation takes place which shortens valve life and can even damage pipeline downstream.
• From the graph, it can be seen that mass flow increases rather slowly than flow factor & flow coefficient which show their exponential nature.
• Hence much larger flow coefficient & flow factor each time there is an increment in mass flow rate.