At most one email a week. Unfollow anytime with one click.
Transcript
The full narration of this video. The current sentence is highlighted while the video plays; click any sentence to jump there.
Show transcript
Introduction
This is the result we will get, the velocity contour inside the ball valve. Two-phase flow of water and steam is sharply accelerated as it passes through the ball opening. Let's start with the geometry. Hello! Welcome to the tutorial series for simulating CFD valve with ANSYS. In this first video, we simulate a ball valve in a 6-meter pipe, containing two-phase flow of water and geothermal steam. All steps are performed with the mouse, starting from Space Climb up to the result contour.
Step 1: Add Fluid Flow system (Fluent with Fluent Meshing)
Open ANSYS Workbench, then click on Ganda Fluid Flow, Fluent with Fluent Machine, in Toolbox.
Step 2: Save the project with the name ValveBall Tutorial
Save the project first with Ctrl S, name it Valve Bowl Tutorial so that all simulation files are neatly stored in one project folder. Get used to saving from the beginning, so that your work is not lost if the program closes suddenly. Right-click on the geometry, select Import Geometry, then Browse.
Step 3: Import STEP geometry of the Ball Valve
Select the File Step Ball Valve. This file contains a 6-meter pipe, valve body, and ball valve in an open position.
Step 4: Open the geometry in SpaceClaim
Right-click the geometry again, then select Edit Geometry in Space Climb.
Step 5: Create fluid domain with Volume Extract
CFD simulation requires fluid volume, not the solid body. Open the Repare tab and select volume extrude. With the right and left views, click the ring face at both ends of the pipe as closures. Hold Ctrl while selecting the second face. Then activate Select Seed Face and click the inner surface of the pipe. Click the green checkmark, and Space Climb creates a new body filling the entire pipe and valve cavity.
Step 6: Name volumefluid and disable solid for physics
Rename the new body to fluid volume using the F2 button. Then select all solid components, right-click, and select Suppress 4P6, so that only the fluid domain is sent to the machine. Hide the solid components so that the fluid volume is clearly visible.
Step 7: Create Named Selection inlet and outlet
Now, name the flow boundary. Select the pipe end face on the inlet side, open the Groups tab, click Create TNS, and name it Inlet. Repeat for the outlet end of the pipe with the name Outlet. This name is automatically read as a boundary type in Fluent Machine. Other surfaces will become walls.
Step 8: Save geometry then open it in Fluent Meshing
Save the geometry, close Space Climb, then double-click cell mesh. In Fluent Launcher, select Double Precision and 12 Processor, then click Start. Wait until Fluent Machine opens with the WaterTik Geometry workflow. In the Import Geometry task, the Geometry from Space Climb is already automatically filled.
Step 9: Import geometry into Fluent Meshing (Watertight Geometry)
Click Import Geometry.
Step 10: Local sizing is not used, then create surface mesh
Add Local Seizing is not used, so directly click Update. In Generate the Surface Mesh, fill in the minimum size 0.002 meter and maximum 0.04 meter, then click Generate.
Step 11: Describe Geometry - domain contains only fluid
In Distribue Geometry, select the Geometry that only contains the fluid region, then click Distribue Geometry. In Update Boundary S, change the inlet boundary type to Pressure Inlet, since the known inlet condition is pressure, which is 40 bar.
Step 13: Update Regions - volumefluid is of type fluid
Update Regions ensures the fluid volume is of type fluid. Click Update Regions.
Step 14: Add boundary layer (inflation) on the wall
Add 5 layers of boundary on the wall. This thin layer is important to capture the velocity gradient near the wall.
Step 13: Generate volume mesh (polyhedra)
Generate the Volume Mesh with polyhedra filling. The result is around 80 thousand cells with minimum orthogonal quality above 0.1, so it is acceptable.
Step 16: Switch to the Solution (Fluent solver)
Click Switch to Solution and Confirm. The mesh is directly moved to Solver Fluent.
Step 17: General - solver pressure-based, steady, gravity active
In General, Solver Pressure Based and Steady are already appropriate. Activate Graffiti with acceleration minus 9.81 on the Y-axis. Open Models, click Ganda Energy, and activate Energy Equation, since geothermal fluid is around 250 degrees Celsius.
Click Ganda Multipase, select the Misture model with two phases, and activate Implicit Body Force. The Mixture model is suitable for a mixture of brine and steam moving together inside a pipe. In Materials, click Create/Edit then Fluent Data Base.
Step 20: Materials - take water-liquid and water-vapor from Fluent Database
Scroll to the end of the list, select Water Liquid and Water Vapor, click Copy, then Close. These two materials represent liquid brine and geothermal hot steam. Unused materials can be deleted to keep the list tidy.
Return to Multiphase, tab Phases. The Primary Phase is named Brine with material Water Liquid. The Secondary Phase is named Steam with material Water Vapor. Click Apply.
Step 22: Boundary inlet - total pressure 40 bar, 523.51 K, vapor fraction 0.2408
Open Boundary Conditions and Edit Inlet on the Misture phase. Enter total pressure 4 million pascal and initial pressure 3.9 million pascal. In the Thermal tab, total temperature 523.51 Kelvin. Then switch to the Steam phase and enter vapor volume fraction 0.2408, according to operational data.
Step 23: Boundary outlet - pressure 25 bar, backflow 523.51 K
Edit Outlet. Exit pressure 2.5 million pascal, or 25 bar. The Bubble Flow temperature is also 523.51 Kelvin.
Step 24: beo Sp 4 PRESTO!, then initialize Hybrid
In Solution Methods, the simple scheme with presto for pressure and first order upwind is stable for the initial calculation. Open Initialization, select Hybrid, and click Initialize.
Step 25: Run Calculation 500 iterations and monitor residual
In Residual Calculation, enter 500 iterations then click Calculate. Residuals keep decreasing, and the solution converges around iteration 315. To view the inside of the pipe, create a cross-section plane.
Step 26: Create a mid-pipe cross-section plane (XV plane, z | 0.6805 m)
From the Result tab, select Create, Plane. Select Hexia Plane at Z0,6805 meter, which is exactly on the pipe axis. This value is read from the domain boundary in the Scale menu. Click Ganda Contors, name the contour as velocity, select Velocity Magnitude, Check Middle Plane, and Save Display.
Step 27: Contour velocity (velocity magnitude) at the center
Adjust the front view, then zoom in around the valve. The flow is accelerated sharply right after the ball gap, reaching about 120 meters per second. This is the effect of Vena Contrakta, which is the narrowing of the flow after the orifice.
Create a second contour for Static Pressure. The pressure around 40 bar upstream drops sharply as it passes through the ball, then recovers downstream near 25 bar.
The third contour is Turbulent Intensity. The highest value appears in the shear layer right after the ball, which becomes the most vulnerable area for erosion on the valve wall.
Step 30: Save project (Save Project)
Finally, Save the Project. Done. We have simulated the ball valve from the geometry in Space Climb, mesh in Fluent Machine, two-phase flow setup, up to velocity, pressure, and turbulence contours. In the next video, we will simulate the Butterfly Valve. Happy trying! Need help with CFD simulation? Cerdas Inovasi Digital offers ANSYS Fluent courses, simulation services for thesis, dissertation, and industry, as well as providing project files from this tutorial. Contact us via WhatsApp, or visit cerdasinovasidigital.com.
Ask the class material
Type a question or keyword; we find the part of this episode that explains it and jump the video there.
My notes
Notes are saved with the current video time and are only visible to you.
Questions & answers
Stuck on a step? Ask here; the instructor and other learners can answer.
No questions yet.
Your instructor
Cerdas Inovasi Digital Team
Software developers, BIM & 3D engineers, and AI practitioners
52 video classes1,276 episodes
We build software, BIM models, games and AI automations for clients every day, and turn that hands-on work into step-by-step classes: every step is shown on screen and comes with a PDF guide you can keep.
