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 final result we will obtain, the water surface profile along the 2D wave flume at the 20th second. Waves are generated on the left side, travel along the flume, pass through the submerged quarter area at the 60-meter position, and are then dissipated by the numerical beach at the right end. Hello! In this tutorial, we will create a simulation of a 2D wave flume in ANSYS Fluent. The flume is 100 meters long, 2 meters wide, 1.5 meters deep, with a model scale of 1 to 50, and a submerged quarter area in the middle. All steps are performed using menus, without scripts.
We start in ANSYS Workbench. From the toolbox, add the fluid flow fluent system. Click on the geometry cell, then in the properties panel, change the analysis type to 2D, since the flume is modeled as a longitudinal cross-section. Open Space Climb from the geometry cell.
Step 2: SpaceClaim - draw a rectangular domain flume
On the XE sketch plane, select the rectangle tool, then draw a rectangle starting from the origin as the domain flume. Its dimensions will be set in the next step.
Step 3: Domain dimensions - length 100 m, height 3 m
Use the dimension tool. Click on the bottom side of the rectangle and type 100 meters as the flume length. Then click on the left side and type 3 meters as the domain height, 1.5 meters of water and the rest as air above it. Select the rectangle tool again and draw a small rectangle attached to the bottom of the flume.
Step 4: Draw a rectangular breakwater at the bottom of the flume
This will become the submerged quarter area.
Step 5: Breakwater dimensions - height 1.2 m, width 2 m
Give dimensions to the submerged quarter area, with a height of 1.2 meters, so that its peak is 30 cm below the water surface, and a width of 2 meters.
Step 6: Move breakwater exactly | x:60m son
To position it accurately, select the submerged quarter area with the selection box, use the move tool, then shift it to the left by 2066 mm, so that its left side is exactly at X60 meters. Click and sketch.
Step 7: Finish sketch - forming a 2D surface
The sketch now becomes a 2D surface, the domain flume and the surface of the submerged quarter area.
Step 8: Delete breakwater surface - so the bottom aa
Select the submerged quarter area surface and press delete. This area is now empty, so Fluent will treat it as a solid wall at the bottom of the flume.
Step 9: Save geometry and close santa
Save the geometry with Ctrl S, then close Space Climb. The geometry is now ready. Go back to the workbench, double-click the cell mesh to open the ANSYS Machine.
Step 10: Open Meshing from the Mesh cell
Wait until the flume geometry appears.
Step 11: Named Selection - inlet, outlet, top, bottom
Create a name selection for the domain boundary. Use box select mode and select the edges. Select the left side, click name selection, and name it inlet. Repeat for the right side as outlet, top as top, and all bottom edges including the quarter as bottom. Click the mesh node, set element size to 0.08 meters, then click generator.
Step 12: Mesh - element size 0.08 m then Generate
The result is a neat quadrilateral mesh throughout the flume.
Step 13: Check mesh in sita sat and statistics
Zoom into the quarter region to check the mesh. In the statistics section, there are approximately 47 thousand elements. Save the work.
Step 14: Save, close Meshing, open Setup
Close machine and return to workbench. Make sure the cell mesh is up-to-date, then double-click cell setup to open the Fluent launcher. In the Fluent launcher, the dimension is already 2D, check double precision and fill the solver process S8, then click start.
Fluent is open and the flume mesh appears directly.
Step 16: General - Transient, gravity V - -9.81 m/s2
In the general panel, select time transient because the waves change over time. Check gravity and enter E-9.81. Notice, gravity must be applied, not X.
Step 17: Viscous Model - Laminar
Open models, double-click fish chose, and select laminar. For non-breaking regular waves, the laminar mode is sufficient.
Step 18: Multiphase - VOF, Open Channel Flow and Wave BC
Double-click multi-base, select volume of fluid. Check open channel flow and open channel wave BC, then click apply. Fluent automatically selects the implicit formulation.
Step 19: Material . (water-liquid) from Fluent Database
Now we need to add water material. Open materials, create to edit, then fluent data base. Scroll down, select water liquid, click copy, then close both dialogs. Now there are 2 materials, air and water.
Step 20: Phase - phase-1 air, phase-2 water
Open again multi-base, tap passes. Phase 1 remains air. Select phase 2 and change phase material to water liquid, then apply. This step is important. Without water, waves will not form. Open boundary conditions, select inlet, edit.
Step 21: Inlet - Aa Wave BC, Airy H 0.2 m, L10.m
Check open channel wave BC. In multi-base fill free surface level 1.5, bottom level 0, wave height 0.2 meter, and wavelength 10 meter with water theory order 1. Reference wave direction select normal to boundary, then apply.
Step 22: : - Open Channel, water surface 1.5 m
Select outlet, edit. In multi-base check open channel, fill free surface level 1.5 and bottom level 0, then apply.
Step 23: Numerical Beach - damping x - 80 until 100 m
Open cell zone conditions, edit fluid zone, tab multi-base, check numerical child beach. Fill water surface 1.5, bottom 0, end point 100 meter, and wavelength 10. With 2 wavelengths, numerical beach dampens waves from 80 to 100 meter to prevent reflection. Open reference values and fill depth 2 meter.
Step 24: Ng - Depth 2 m (flume width)
In 2D model, this value represents the width of the flume 2 meter.
Step 25: Solution Methods - PISO
In solution methods, change pressure velocity coupling scheme to pressure-based, which is suitable for transient simulation.
Step 26: Initialization - Standard Initialization
Click initialize from ribbon solution for standard initialization. At this stage, the entire domain still contains air.
Step 27: Cell Zone - water area 0 to 1.5 m
We mark the water region. Right-click cell zones, new, region. Name the region underscore water, then fill X from 0 to 100 and Y from 0 to 1.5 meter. Click save. Click patch.
Step 28: Patch - fill water in the water area
Select phase 2, variable volume fraction, value 1, and register to patch the water area. Turn off the 2 smoothing options, then click patch. 23,000 cells are filled with water.
Step 29: Contour of water fraction initial condition
Display the contour of phase 2 volume fraction in the fluid zone. Red is water up to 1.5 meters, blue is air, and broken water is visible at the bottom.
Step 30: Run Calculation - time step 0.02 s, 1000 steps
In the solution ribbon, enter time step size 0.02 seconds and number of steps thousand, so the simulation runs for 20 seconds. Click calculate and wait until it finishes.
Step 31: Results - contour of wave at t - 20 s
After it finishes, display the water fraction contour again and enlarge the broken water area. The water surface is now wavy and waves are crossing over the submerged broken water.
To view the water surface profile, create an ISO surface from phase 2 volume fraction with value 0.5. We name this surface water underscore surface. Create an X-Y plot with Y coordinate on the water surface against position X.
: Step 33: XY Plot - free surface profile along the flume
It is visible that the wave series have a length of about 10 meters, amplitude that decreases after the broken water at 60 meters, and calm water surface in the numerical Chalbich area.
: Done! 2D wave flume project saved
Finally, save the project from the file menu, Save Project. Our 2D wave flume simulation is complete. Complete graphs, transmission coefficient, and energy reduction are in the PDF report. Thank you for watching. Need help with CFD simulation? Cerdas Inovasi Digital opens ANSYS Fluent courses, simulation services for thesis, dissertation, and coastal or hydraulic projects, as well as providing project files and reports 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
53 video classes1,281 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.
