Week 9 - Parametric study on Gate valve.

Aim: To perform a parametric study on Gate Valve using steady-state simulation by raising the disc of the valve from `10%` to `70%`

Objective: 

• Obtain the mass flow rates at the outlet for each design point.
• Calculate the flow coefficient and flow factor for each opening and plot the graph.
• Discuss the results of the mass flow rate and flow coefficient. 

Introduction

A gate valve opens by lifting the barrier out of the path of the fluid. It requires very little space to be installed along the pipe's path, thus hardly restricting any fluid flow along the pipe. The gate faces are almost parallel but are commonly wedge (to apply pressure on the sealing surface). The gate valve when fully open does not provide any restriction to the flow when the disc is fully lifted upwards. They are frequently used in pipes (diameter ranging from `frac{3}{4}` inch to larger diameters ).

Some gate valves are used without sealing in heat application and sewer pipes where the minor leak is not a big issue.

The gate valves may have threaded connections (diameter ranging from `frac{3}{4}` inch to `2` inch and may have flanged connections (diameter ranging from `2frac{1}{2}` inch to larger diameters pipes involved in chiller plant room). They are actuated by the threaded stem that connects the actuator to the gate. They are characterized by either rising or non-rising stems depending upon which end of the stem is threaded. Rising stems are fixed to the gate and they rise and lower together as the valve is operated providing a visual indication of how the valve is operated. Non-rising stems are threaded into the gate and have a pointer indicating the valve position, they are used where the vertical space is limited.

The gate valve is made up of cast iron, ductile iron, alloy steels, forged steels.

Application of gate valve

A typical gate valve application includes

• Cooling water systems.
• Fuel oil systems.
• Feedwater or chemical feed system.
• Boiler and main steam vents and drains.
• Turbine lube oil system.

Solving and Modelling approach

• The gate valve is loaded into Spaceclaim
• The components of the gate valve are unchecked except the gate disc.
• The gate disc is moved upward by selecting the option "Move" from the Spaceclaim ribbon. The lift of the gate valve is increased from `10% to 70%` to observe the changes in the mass flow rate of the water and corresponding flow coefficient`
• The fluid volume is extracted from the solid volume using the "Volume Extract option" in the ribbon provided in the Spaceclaim.
• Both sides of the fluid volume are pulled to an extent of `800mm`.
• The named selection (inlet, outlet) is created, and then meshing is done using the default element size of ANSYS-FLUENT.
• The pressure inlet of 10 Pa is applied, the gravity is enabled, the steady-state simulation is executed.
• The necessary contour plots and monitor plots are visualized for the mass flow rate of the water.

Preprocessing and Solver settings

The geometry is loaded into Spaceclaim

The components of the gate valves are checked except the gate disc which is required to be raised as per the challenge

The gate disc is raised to a level of 10mm from the initial position and the parametric point is created for the same.

The components are checked to extract the fluid volume out of solid volume.

Both sides of the volume are pulled to the length of 800mm.

 

 

The components are checked off and suppressed for physics except for the fluid volume. The fluid volume component is loaded into the meshing window for creating the named selections.

Inlet (type pressure inlet)

Outlet (type pressure outlet)

Mesh

It is used for discretizing the entire geometry to obtain a solution that can mimic the original solution with a minimum deviation. It is also helpful in solving partial differential equations. The finite volume method scheme is used for solving the equation as it preserves the conservation property moreover, it can be applied to the unstructured mesh.

Baseline mesh

 

Mesh quality and attributes

Element size	Number of elements	Element quality	Aspect Ratio	Skewness	Orthogonal Quality
`92.892mm`	`136591`	`0.81867`	`2.925`	`0.25189`	`0.74638`

 Please also note that the maximum skewness value for the baseline mesh is `0.98291` which exceeds the skewness value given by the ANSYS-FLUENT which may lead to inaccuracy in the solution.

Refined mesh 

Element size: `6mm`

Please note that during the mesh refinement approach captured curvature is set to yes, captured proximity is set to yes and num gap across cells is set to 1.

 

Mesh quality and attributes

Element size	Number of elements	Element quality	Aspect Ratio	Skewness	Orthogonal Quality
`6mm`	`419826`	`0.83569`	`1.8571`	`0.2302`	`0.76807`

 

Set up

The steady-state pressure-based solver is selected (`Mlt0.3`). The gravity is enabled and the value of `-9.81msec^-2` is computed for the z-axis.

Calculating Reynolds number for the flow

`R_e=frac{rho*v**D}{mu}`

`R_e=frac{998.2**0.1415**0.1}{1.003**10^-3}`

`R_e=14028.82` which is `gt``4000` which justifies that the flow is turbulent in nature. 

Viscous model

The viscous model is set to `k-epsilon` realizable scalable wall functions. The `k-epsilon` turbulence model consists of two transport equations one for turbulent kinetic energy(k) and one for the turbulent dissipation rate `epsilon` to calculate the rate of dissipation of kinetic energy.

The turbulent viscosity term has been formulated differently. The turbulent dissipation rate (`epsilon`) has been developed from the mean square vorticity equation.

The purpose of the usage of scalable wall function is to force the usage of log laws in conjunction with the standard wall function approach. This is achieved by introducing the limiter in the `y**` calculation  such that 

`y^~**=MAX(y**,y**li mit)`

where `y**li mit``=11.225`

The y* formulation used in the standard wall function formula is replaced by `y^~**`

It also prevents any errors originating from the viscous sub-layer and the buffer layer.

Materials 

The default material taken by ANSYS-FLUENT is air(`rho=1.225frac{kg}{m^3}` `mu=1.7894e-05frac{kg}{m-sec}`), which is to be replaced by water(`rho=998.2frac{kg}{m^3}` `mu=1.003**10^-3frac{kg}{m-sec}`. The "Material" option is clicked. By clicking on Fluent database water is copied. In order to avoid the redundancy by the ANSYS-FLUENT, the cell zone under the name volume_volume is clicked. The edit option is clicked and in the material option air is replaced by water, followed by deleting of air in the "Material" option of ANSYS-FLUENT.

Boundary condition

Inlet (type pressure inlet): The pressure inlet type is selected for the inlet, the gauge total pressure is selected as 10Pa and the rest values will be the default value for ANSYS-FLUENT. 

Outlet(type pressure outlet): The outlet is selected as a pressure outlet, the values will be the default values from the ANSYS-FLUENT.

Wall: The wall motion is stationary and the shear condition is no-slip, and the rest values will be the default values from the ANSYS-FLUENT.

Initialization

The standard method is selected and the initialization is done by selecting it from the inlet of the pipe.

After initialization, the required monitor plots and contour plots are set up to visualize the mass flow rate with the change in the lift of the disc.

Results

Baseline mesh

Element size: `92.892mm`

Pressure-velocity coupling schemes: SIMPLE

Residual Plot

Mass flow rate 

Pressure-velocity coupling schemes: SIMPLEC

Residual Plot

 Mass flow rate 

 

Pressure-velocity coupling schemes: COUPLED

Residual Plot

Mass flow rate 

Comparison of all cases

Mesh	Number of elements	Pressure-velocity coupling schemes	Mass flow rate  `frac{kg}{s}`
Baseline mesh	`136591`	SIMPLE	`0.1485678`
		SIMPLEC	`0.1485463`
		COUPLED	`0.1486235`

It was observed that when the simulations were performed for the baseline mesh using three pressure velocity coupling schemes (SIMPLE, SIMPLEC, COUPLED), the COUPLED scheme performs better than the two segregated schemes. The COUPLED scheme took 25 iterations for convergence whereas SIMPLE and SIMPLEC took 100 iterations for convergence. The COUPLED scheme is robust, solves the pressure and velocity equation instantaneously but requires more space. The SIMPLE and SIMPLEC scheme are segregated schemes solves pressure and velocity equations sequentially and requires less space.

For the COUPLED scheme the gradient is set to the least square cell method, pressure is set to the second-order scheme, momentum is set to the second-order upwind scheme, turbulent kinetic energy, and turbulent dissipation rate to the first-order upwind scheme. The second-order scheme for pressure makes use of a central differencing scheme which is more accurate than Standard and Linear Schemes and robust than skewed schemes. The first-order upwind scheme makes use of quantities at the cell faces as the cell average value indicating that it is first-order accurate. The reason to have the turbulence terms discretized using a first-order upwind scheme is that it is computationally less expensive and has a more stable output.

 

 

Parametric lift

 

The gate disc is lifted by `10%` is set to parametric. The section view of the gate valve will be seen as shown below

 

 

The "Volume" body is expanded in the structure and the "Update volume body in context" is selected as shown below

 

The "Bottom" component of the gate valve is selected, followed by selecting the 3D mode option.

 

The set-up case will be the same as the baseline mesh except "Create output parameter" is selected for the monitor plot "Mass flow rate", and is updated for each and every design point. The Design points are created for each gate disc lift for the refined mesh and increasing mass flow rates are observed and the corresponding residual plots and monitor plots are observed for each case.

Design points for gate disc lift created in the Workbench

The negative sign suggests that the fluid is flowing out of the volume.

Evaluation of flow coefficient and flow factor

Flow coefficient can be defined as the device efficiency to permit the fluid flow. In the case of gate valve, it can be described as 

`C_v=Qsqrtfrac{SG}{triangleP}`

where 

`Q=`Rate of fluid flow (US gallons per minute)

`triangleP`= Pressure drop across the valve in psi.

SG represents the specific gravity of the water which equates to 1.

Flow factor

It is related to the flow coefficient except for the rate of fluid flow and the pressure drop is expressed in the metric system of units. The flow coefficient is calculated for `60^@F` temperature and pressure `1frac{lb}{i n c h^2}`. The flow factor is calculated for `5^@C` to `30^@C` and pressure 1bar.The flow factor and the flow coefficient is related to each other by 

`K_v=0.865**C_v`

Units conversion

`1frac{kg}{s}=21.44` US GPM.

`1Pa``=``0.000145` pound-force per square inch

 Element size : `6mm`

`10%` lift of the gate valve.

Residual plot

 

Mass flow rate 

 

Contour-velocity

 

Contour pressure

 

`20%` lift of the gate valve`

Residual plot

Mass flow rate 

 

Contour-velocity

 

Contour pressure

 

`30%` lift of the gate valve`

Residual plot

Mass flow rate 

 

Contour-velocity

 

Contour pressure

`40%` lift of the gate valve`

Residual plot

Mass flow rate 

 

Contour-velocity

 

Contour pressure

`50%` lift of the gate valve`

Residual plot

Mass flow rate 

 

Contour-velocity

 

Contour pressure

`60%` lift of the gate valve`

Residual plot

Mass flow rate 

 

Contour-velocity

 

Contour pressure

 

 `70%` lift of the gate valve

Residual plot

 

 Mass flow rate 

 

Contour-velocity

 

Contour pressure

 

 

Comparison of all cases 

Valve opening (%)	Lift      (mm)	Mass flow        rate    `frac{kg}{sec}`	areaAvePressure(@inlet)              (Pa)	areaAvePressure(@outlet)              (Pa)	Pressure drop  areaAvePressure(@inlet)-areaAvePressure(@outlet)    (Pa)	Flow coefficient  `C_v`	Flow factor  `K_v`
`10`	`10`	`0.14753`	`9.82243`	`-0.00191658`	`9.82434658`	`83.8048`	`72.4912`
`20`	`20`	`0.23062`	`9.56551`	`-0.00272211`	`9.56823211`	`132.7461`	`114.825`
`30`	`30`	`0.33829`	`9.06395`	`-0.00710933`	`9.07105933`	`199.9866`	`172.9884`
`40`	`40`	`0.4511`	`8.33482`	`-0.00294179`	`8.33776179`	`278.1562`	`240.6051`
`50`	`50`	`0.5659`	`7.38188`	`-8.23785e-07`	`7.38188082378`	`370.8488`	`320.7842`
`60`	`60`	`0.66107`	`6.42838`	`0`	`6.42838`	`464.2345`	`401.5628`
`70`	`70`	`0.74839`	`5.42521`	`0`	`5.42521`	`570.6723`	`493.6315`

 

 Flow coefficient, Flow factor, Mass flow rate vs Lift of the disc

 

 

 Conclusion

• The steady-state simulation and parametric study on the gate valve were performed successfully in ANSYS-FLUENT 2021R1.
• It was also observed that the handle wheel of the gate valve can be rotated in a clockwise and anticlockwise direction which causes the gate disc to move upward and downward to regulate the movement of water flow through it.
• As the lift increases from 10mm to 70mm, it was observed that the mass flow rate also increases.
• Flow coefficient and flow factor are directly proportional to the rise of gate disc representing the amount of fluid that can pass through it, implying that the flow coefficient also increases which further resulted in an increase in flow factor.
• The selection of gate valves will primarily depend upon their material of construction, service life, and providing maximum flow coefficient and minimum pressure drop.
• The increase in the rise of the gate disc is the main reason for varying velocity and pressure contour plots in the region, and the flow coefficient and flow factor determine the selection of the gate valve.