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 flow inside the globe valve. The flow turns forming an S-shape as it passes through the plug seat. Let's start. Hello! Welcome to the final video of the CFD valve simulation tutorial series with ANSYS. This time, we will simulate a globe valve, a valve with an S-shaped flow path commonly used to control the flow rate. Open ANSYS Workbench, then double-click Fluid Flow, Fluent with Fluent Machine, in the toolbox.
Step 2: Save the project with the name ValveGlobe Tutorial
Save the project first with Ctrl + S and name it valve globe tutorial.
Right-click the geometry, select Import Geometry, then browser. Select the file space climb globe valve. This assembly contains 2 pipes of 6 meters, the valve body, plug, and rotating wheel, and the fluid domain has already been created with volume extraction as in the ball valve video.
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 will check the fluid domain. Open the volume component and hide the default component. Zoom in around the valve, you can see the valve body cavity, the partition, and the plug seat that causes the flow to turn like an S-shape.
Step 6: Disable solid for physics (Suppress for Physics)
Right-click the default component, then select suppress for P6, so that only the fluid domain is sent to the machine.
Step 7: Check Named Selection inlet and outlet
Open the tab groups. The inlet and outlet selections are already available at both ends of the pipe. Click each to check them.
Step 8: Save geometry then open Mesh in Fluent Meshing
Save the geometry, close Space Climb, then double-click cell mesh. 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 water tick geometry is ready. Click import geometry.
Step 10: Local sizing is not used, then create surface mesh
Add local seizing is not used. In the surface mesh generator, enter minimum size 0.002 meters and maximum size 0.03 meters, then click generator. In the geometry distribution, select the geometry that only contains the fluid region, then click distribute geometry.
Step 11: Describe Geometry - domain only contains fluid
In the update bound from S, change inlet to mass flow inlet, because the operational data of the globe valve is in terms of mass flow rate.
Step 13: Update Regions - volumefluid 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 bound from the screen on the wall.
Step 13: Generate volume mesh (polyhedra)
Generate the volume mesh with polyhedral filling. Because the globe valve cavity is more complex, the result is around 735 thousand cells, with minimum orthogonal quality 0.12. Click switch to solution and confirm to enter the solver Fluent.
Step 17: General - pressure-based, steady, gravity active
In General, pressure-based solver and steady are already appropriate. Activate gravity minus 9.81 on the Y-axis.
In Models, the SST K-Omega turbulence model is already active by default. The globe valve is simulated with single-phase vapor. In Materials, change water to steam with density 11.5 kg per cubic meter and viscosity 1.8 x 10 to the power of minus 5.
Step 19: Materials - create material steam (density 11.5 dim
Click chunk create, then yes.
Step 20: Boundary inlet - mass flow rate 1.39 kg/s | P
Edit inlet and fill mass flow rate 1.39 kg per second. Outlet uses pressure gauge 0 pascal. The choplet or D2 method is used automatically.
Step 2: Initialize Hybrid (method Coupled order
Open initialization, select hybrid, then initialize.
Step 22: Run Calculation 300 iterations and monitor et
Run calculation fill 300 iterations then click calculate. Residual momentum and turbulence drop and stabilize. Residual continuity at the globe valve is still quite high because of the sharp turn and forming vortices. Therefore, for the final report continue iterations until around 2000, as in the research report. View the domain boundaries in the menu scale.
Step 23: Create a mid-pipe cross-section plane (XV plane, z | 0)
The globe pipe points to the X-axis, with the pipe axis around Z0. Create X-Y plane at Z0.
Step 24: Velocity magnitude contour (velocity magnitude) on the plane
Create a velocity magnitude contour with a front view and highlight the area around the valve. The flow decreases as it passes through the plug seat gap and then rises to the outlet side, forming an S-shaped path, with maximum velocity around 7.5 meters per second, much lower than other valves, as reported.
Create a static pressure contour. High pressure is on the inlet side, then gradually decreases after passing through the plug seat. This is why globe valves are suitable for controlling flow.
Ir 26: Turbulent intensity contour (turbulent intensity)
Create a turbulent intensity contour. The highest turbulence is located in the lower part of the valve and downstream of the plug, where the flow turns and forms vortices.
Step 27: Save project (Save Project)
Finally, save the project. Done. The fourth series of valve simulations is now complete. Ball, butterfly, gate, and globe valves. Good luck trying, and see you in the next tutorial. 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.
