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 around the butterfly valve disc. The flow stops in front of the disc, accelerates on both sides, and then forms a wake behind it. Let's start. Hello! Welcome to the second part of the CFD valve simulation tutorial with Ansys. This time, we will simulate a butterfly valve with a thin disc rotating in the center of the pipe. The process is the same, from space climb, fluent machine, setup fluent, up to the result contour.
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 ValveButterfly Tutorial
Save the project first with Ctrl + S and name it valve butterfly tutorial, so all simulation files are neatly stored in one folder.
Right-click cell geometry, select replace geometry, then browser. Select the file space climb butterfly valve. This file is an assembly of two 6-meter pipes, valve body, disc, and shaft, with the fluid domain already created using volume extrude. In the butterfly valve, the gap between parts in the original assembly causes the volume extrude to fail, so we use the geometry that has already been cleaned up.
Step 4: Open the geometry in SpaceClaim
Right-click geometry again, then select edit geometry in space climb.
Step 5: Check the fluid domain result from Volume Extract
We check the fluid domain. Hide the default solid components, and the volume component containing the fluid body filling the entire pipe becomes visible. Zoom in around the valve, the disc and shaft are printed as cavities within the fluid. The way to create it is the same as in the ball valve video, that is, prepare, volume extrude, select the faces at both ends of the pipe, then the seat face inside the pipe. Rename the fluid body to volume fluid using the F2 button, then right-click the default component containing all solid parts, and 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 name selections inlet and outlet are already available at both ends of the pipe. Click each to make sure the selected face is correct. This name automatically becomes the boundary type in Fluent Machine, while other surfaces become walls.
Step 8: Save geometry then open " | 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 into Fluent Meshing (Watertight Geometry)
In Fluent, the water-tight geometry workflow is already ready. Click Import Geometry.
Step 10: Do not use Local sizing, then create surface mesh
Local Seizing is not used. In Generate the Surface Mesh, enter minimum size 0.002 meters and maximum size 0.04 meters, then click Generate. If the values are not entered, click Edit, correct the numbers, then Update.
Step 11: Describe Geometry - domain contains only fluid
In Describe Geometry, select the geometry that contains only the fluid region, then click Describe Geometry. In Update Boundaries, change inlet to pressure inlet, since the inlet condition is pressure of 40 bar.
Outlet remains pressure outlet. Update Regions ensures the fluid volume is of type fluid.
Step 14: Add boundary layer (inflation) on the wall
Add 5 layers of boundary from the screen on the wall to capture velocity gradients near the disc and pipe surface.
Step 13: Generate volume mesh (polyhedra)
Generate the Volume Mesh with polyhedra filling. The result is around 108,000 cells with minimum orthogonal quality of 0.1. Click Switch to Solution and confirm to enter the Fluent Solver.
Step 17: General - solver pressure-based, steady, gravity active
In General, pressure-based solver and STAD are already set correctly. Activate Gravity Minus 9.81 on the Y-axis.
Step 18: Models - activate Energy
Open Models and activate Energy, since the geothermal fluid is around 250 degrees Celsius.
Click Multiphase, select Mixture with 2 phases, and activate Implicit Body Force. In Materials, open Fluent Data Base, scroll to the end of the list, select Water Liquid and Water Vapor, click Copy, then Close.
In Tab HSS, the primary phase is named Brine with material Water Liquid, and the secondary phase is named Steam with material Water Vapor. Edit Inlet
Step 22: Boundary inlet - total pressure 40 bar, 523.51 K, vapor fraction 0.2408
Total pressure 4 million pascals, initial pressure 3.9 million pascals, total temperature 523.51 Kelvin, and vapor volume fraction 0.2408 on the Steam phase.
Step 23: Boundary outlet - pressure 25 bar, backflow 523.51 K
Edit Outlet Exit pressure 2.5 million pascals with Bug Flow temperature 523.51 Kelvin. Open Initialization, select Hybrid, then Initialize.
Step 24: Methods - SIMPLE # PRESTO!, then initialize Hybrid
The Simple method with Presto and First Order Upwind is already stable enough.
Step 25: Run Calculation 500 iterations and monitor residuals
In Rencal Culation, fill 500 iterations and then click Calculate. After 500 iterations, residual continuity is still around 10 to the power of minus 3, so we add another 300 iterations. Solution converges around iteration 525, when all residuals are below the criteria. Check the domain boundaries in the Scale menu.
Step 26: Create a mid-pipe cross-section (VZ plane, x | 0,0901 m)
Butterfly pipe points towards the Z-axis, with the pipe axis at X0,09 meter. Create a YZ Plane at that position from the Result tab, Create, Plane.
Step 27: Contour velocity (velocity magnitude) at mid
Create Velocity Magnitude Contour. On the side view, the disc is seen facing the flow. We also add a ZX plane cutting through the disc, then display the contour with the top view. The flow stops at the front face of the disc, is accelerated on both sides up to around 67 meters per second, then forms a low-speed wake behind the disc.
Step 28: Contour static pressure | |
Create Static Pressure Contour. The highest pressure, around 40 bar, accumulates at the front stagnation point of the disc, then decreases on the back side.
Create Turbulent Intensity Contour. Highest turbulence appears at the disc edge and the wake zone just downstream, areas that need to be watched out for erosion.
Step 30: Save project (Save Project)
Finally, save the project. Done. Butterfly Valve has been simulated from geometry to contours. In the next video, we simulate gate valve. Good luck 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. Thank you for watching!
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.
