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 of the steam flow inside the gate valve. The flow moves straight through the open valve, while the gate chamber contains slow-moving flow. Let's start. Hello! Welcome to the third tutorial series of CFD simulation for valves using ANSYS. This time, we are simulating a gate valve, a valve with a door that rises and falls to cut the flow. Different from the previous two videos, here we use a single-phase steam flow with a specified inlet velocity.
Step 1: Add Fluid Flow system (Fluent with Fluent Meshing)
Open ANSYS Workbench, then double-click Fluid Flow, Fluent with Fluent Machine, in the Toolbox.
Step 2: Save the project with the name ValveGate Tutorial
Save the project first with Ctrl + S and name it 'valve gate tutorial', so all simulation files are neatly stored in one folder.
Right-click on the geometry, select Import Geometry, then browse. Select the file 'space climb gate valve'. This assembly contains two pipes, the valve body, the gate door, and the rotating wheel. The fluid domain has already been created with volume extrusion, because the flange in the original step file closes the end face of the pipe.
Step 4: Open the geometry in SpaceClaim
Right-click the geometry again, then select Edit Geometry in Space Climb.
Step 5: Check the fluid domain result from Volume Extract
We check the fluid domain. Open the volume component and hide the default component containing the solid parts.
Step 5: Check the LA fluid T Extract
The fluid volume body is visible, filling both pipes and the valve body chamber.
Step 5: Check the fluid domain result from Volume Extract
Zoom in around the valve to see the shape of the gate chamber and its seating. Right-click the default component, then select Suppress for Physics, so only the fluid domain is sent to the machine.
Step 7: Check Named Selection inlet and outlet
Open the Groups tab. The inlet and outlet selections are already available at both ends of the pipe. Click each to ensure the selected face is correct. Save the geometry, close Space Climb, then double-click Cell Mesh.
Step 8: Save the geometry then open Mesh in Fluent Meshing
In the Fluent Launcher, select Double Precision and 12 processors, then click Start.
Step 9: Import geometry to Fluent Meshing (Watertight Geometry)
In the Fluent Machine, the workflow for the geometry is already ready. Click import geometry.
Step 10: Local sizing is not used then create surface mesh
Local seizing is not used. In the surface mesh generator, enter the minimum size of 0.002 meters and maximum size of 0.04 meters. A self-intersection message appears in the gate valve, so click edit, open advanced options, and increase the smooth folded facet limit to 200. Click update and surface mesh has been successfully created.
Step 11: Describe Geometry - domain only contains fluid
In Destribe Geometry, select the geometry that contains only the fluid region, then click Destribe Geometry. In the S boundary update, inlet is of type velocity inlet because we are providing an inlet velocity, and outlet is of type pressure outlet.
Step 13: Update Regions - volume fluid is of type fluid
Update Regions ensures the fluid volume is of fluid type.
Step 14: Add boundary layer inflation on the wall
Add 5 layers of boundary layer on the wall to capture the velocity gradient near the wall.
Step 13: Generate volume mesh (polyhedra)
Generated the volume mesh with polyhedra filling. The result is approximately 218 thousand cells with a minimum orthogonality quality of 0.11. Click switch to solution and confirm to enter the fluent solver.
Step 17: General - pressure-based, steady, gravity active
In General, the pressure-based solver and steady state are already suitable. Activate gravity minus 9.81 on the Y-axis.
In the Models, the SST K-Omega turbulence model is already active by default. For the gate valve, we do not use multiphase and energy, because the fluid is single-phase vapor. In Materials, open water and rename it to steam, with a density of 5.76 kg per cubic meter and a viscosity of 1.34 x 10^-5.
Click Cange Create, then Yes to overwrite the water.
Step 20: Boundary inlet - velocity 23.41 m/s
Edit Inlet. Set velocity magnitude to 23.41 meters per second, according to operational data.
Step 21: Outlet - gauge pressure 0 Pa
The outlet uses gauge pressure in pascal, so just check and close it. In Methods, for single-phase flow in Fluent, the coupled scheme with second-order accuracy is used, which is fast and accurate.
Step 22: Methods, Coupled order 2, then initialize Hybrid
Then open Initialization, select Hybrid, and click Initialize.
Step 23: Run Calculation 300 iterations and monitor residual
In Rencal Culation, turn off data sampling, enter 300 iterations, then click Calculate. Residual momentum and turbulence have dropped below 10 to the power of minus 4, while continuity continues to decrease steadily.
Step 24: Create mid-pipe cross-sectional plane (VZ ng
Check the domain bounds in the Scale menu. The pipe is aligned with the Z-axis, with the pipe's axis at X0,316 meter. Create a Yezet Plane at that position.
Step 25: Contour velocity (velocity magnitude) on the plane
Create a velocity magnitude contour and display it in the right view. The gate is in the raised position, allowing the flow to pass straight at around 26 meters per second, while the gate cavity above and the seat below contain slow-moving flow.
Create a static pressure contour. The pressure decreases gradually along the pipe, with a maximum pressure of around 1140 pascal at the inlet, as reported.
Step 27: Contour turbulent intensity (turbulent intensity) w
Create a turbulent intensity contour. The highest turbulence occurs at the corners of the gate cavity and at the flow junction after the valve, areas prone to erosion.
Step 28: Save project (Save Project) j
Finally, save the project. Done. We have simulated the gate valve from geometry to contours. In the final video of this series, we will simulate a globe valve. Happy trying.
0 uh Ie IM Si at Naa at eco irtlietstai aib tabinta) "1 Oett binti aa
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.
