November 2, 2022 at 10:06 ampv00170Subscriber
I am performing a multiphase 2D open-channel flow using air (primary phase) and water (secondary phase).
The main objective is to simulate a submerged bridge deck as shown in the figure.
- I have enabled Open channel Flow and also Open Channel Wave BC (even though I don't use waves) is just for having 0 velocity on the air inlet).
- Implicit Body Force.
- Pressure based solver.
- Gravity in the vertical direction -9.81.
- I am using SST k-w with Corner Flow correction (since I expect turbulence inside the girders)
- Fluid is defined as Numerical beach and Free Surface Level is specified.
- Standard initialization: from inlet and flat. (also I have tried with hybrid)
- Inlet: Velocity inlet - Segreagted velocities (3 m/s water 0 m/s air) & multiphase: water level
- Outlet: Pressure outlet - Multiphase open channel: water level
- Open: Pressure outlet - zero gauge
- Floor: No-slip wall
- The thing is that residuals never converge even if I change the mesh. And if they seem to converge, drag coefficient vary sustanciably (60% variations aprox.)
- I know I should leave the simulation run more iterations, is just an example (I have also done it and the drag coefficient still vary a lot)
- Can I use steady state for this problem or it's not applicable?
- Are the BC and models appropriate?
- Is there any recommendation for me to follow?
November 3, 2022 at 9:43 amRobAnsys Employee
For the graphics, in 2d don't pick any surfaces. You'll get a continuous contour as the solver will magically figure it out.
I can't tell if you have supports under the bridge, remember in 2d there's no way for the water to get around these: that could cause some interesting results. If they're buoyant cells that may be different.
Residuals & reports are mostly as expected. You may need to resolve the mesh near the free surface, but I can't see from the image. Generally in multiphase there is something in the flow (reflected waves, ripples etc) that are transient. The question you need to consider is whether these waves etc are altering the data you're interested in. Ie are you wanting to see the flow field and understand the range of drag, or see the speed/rate of any transient effects?
November 3, 2022 at 12:15 pmpv00170Subscriber
Do you mean with the first sentence to pic Fluid for the contours rather than Internal? (I don’t know why there is such high velocity under the bridge slab deck)
In this case I am not considering the supports as I am analysing middle span sections. (The four thin small lines below the deck are steel girders).
Does Fluent consider buoyancy?
What do you mean with “You may need to resolve the mesh near the free surface,” I used a BOI for the interfase
My main focus is to get drag and lift forces and coefficients.
Then, Residuals & reports are like this even though is a steady state?
November 3, 2022 at 1:31 pmRobAnsys Employee
Yes, pick fluid. It's a change on older versions as you didn't pick anything up until a couple of releases back.
BOI is fine, adaption is another option.
Lastly, the acceleration is because you're forcing water through a smaller gap: where else will it go in a 2d model?
Fluent considers buoyancy for fluids, depending on density and if you turned gravity on. Solids would need moving mesh (or immersed boundary) and some other settings to be buoyant. The first example we had was a cube hitting water, then a lifeboat (getting off oil & gas platforms isn't that easy if it's on fire) and now things falling off aeroplanes
November 3, 2022 at 2:23 pmpv00170Subscriber
Yeah, I understand why acceleration is happening. Makes sense.
Is the dynamic mesh for the interface or for the bridge?
The thing is that the bridge is a void area, therefore it cannot move. If it is designed like this, is buoyancy still considered?
In this analysis I just want to get drag and lift coefficients, but since values were varying a lot for a steady state, I don't know if the simulations is performed correctly. (I would understand if values are sinusoidal ish for transient states.
November 3, 2022 at 4:06 pmRobAnsys Employee
Dynamic mesh would be if the bridge was moving. You can probably assume it's fixed, but may want to google Tacoma Narrows Bridge Collapse for when that's not case! It'll only move if you tell it to, so at present it's not going anywhere.
We often talk about "dynamic adaption" which refers to automatic mesh refinement & coarsening. That's commonly used around a free surface to refine the mesh as the surface moves. As you've not got any waves it's probably not necessary.
The only issue with the set up (that I can see) is that the bridge supports are effectively continuous so the water can't go around them. I don't know if that's part of the design but in most cases they probably shouldn't be there.
Drag etc will almost certainly vary with time, in the steady solver it can vary with iteration if the solver can't lock the flow down to a single converged solution. You either need to run transient, or take the steady result with some scatter due to inherent transients in the flow: that's something you may want to discuss with your supervisor.
November 3, 2022 at 5:44 pmpv00170Subscriber
What is seen in the immage are not supports, are girders. It is a cross section. In this case no pier are modelled so water is flowing under the deck.
Is there any way to obtain the percentage/quantity of the pressure on the void (solid) due to buoyancy or I have to do it by hand?
PS: Thanks a lot for your help
November 4, 2022 at 9:37 amRobAnsys Employee
There are force reports on walls, along with volume reports to find out how much air is trapped under the deck.
November 4, 2022 at 10:05 ampv00170Subscriber
When I do florce reports on walls I check drag and lift forces.
But lift forces I assume to be due to hydrodynamic, buoyancy forces and weight of water above the bridge deck.
Is there any direct way to obtain the forces of each of these sources? Like:
- Hydrodynamic - 20000 N
- Buoyancy: +30000 N
- Weight of water: -1000 N
November 4, 2022 at 10:19 amRobAnsys Employee
The solver doesn't know the mass of the bridge, so pressure etc is a function of the water and air volume density in the trapped pockets. If you look there are also forces (x, y & z) as opposed to lift & drag.
November 4, 2022 at 12:35 pmpv00170Subscriber
Yeah I get the solver doesnt know the mass of the bridge, but knows the volume of displaced water, and I imagine it solves buoyancy by using it. I assume there is no direct method to check wich % of the total pressure are due to water weight, buoyancy and hydrodynamic.
With "If you look there are also forces (x, y & z) as opposed to lift & drag" do you mean negative values?
November 4, 2022 at 10:36 ampv00170Subscriber
Yeah I get the solver doesnt know the mass of the bridge, but knows the volume of displaced water, and I imagine it solves buoyancy by using it. I assume there is no direct emthod to check wich % of the total pressure are due to water weight, buoyancy and hydrodynamic.
November 4, 2022 at 2:33 pmRobAnsys Employee
The solver knows the flow and composition, so can find the forces on walls. That isn't broken down by cause.
The forces are what the fluid exterts on the walls, so yes, negative would probably be correct. However, as the bridge has no mass the results may be misleading.
November 4, 2022 at 3:47 pmpv00170Subscriber
I will use 2D CFD results in a 3D FE analysis in which bridge has mass. Then, I will check if drag and lift forces can move the bridge.
Do CFD results vary depending on the mass of the bridge? How can this mislead the results? (Could you explain more, since maybe there is something I am missing)
November 4, 2022 at 3:52 pmRobAnsys Employee
The bridge is fixed so won't do anything in the Fluent solver. Have a look at what Mechanical takes in as boundary conditions, I very much doubt it's lift and drag over the components.
November 4, 2022 at 4:02 pmpv00170Subscriber
I use in the FE analysis: earth gravity for the bridge, fixed/non-fixed supports (depending on the bearings) and imported pressure on the bridge faces (walls) from fluent.
November 25, 2022 at 2:18 pmpv00170Subscriber
Hi Rob, I have another question. When I simulate high velocity (10 m/s) for let's say 5.5 m height water, I get weird results.
Density after initialization (red water, blue air):
Velocity after initialization (10 m/s for the water 0 m/s for the air):
After a lot of iteration water interacts with the structure, but a weird wave is created upwards as seen in the following pictures. Therefore, water height ends up being greater than specified in the inlet. It ends up being like this (not finished running simulation):
Also, the velocity in front of the structure is reduced from 10 to 7 … Drag and lift coefficients are still computed with a velocity of 10 m/s but I don’t think this results are right…
November 25, 2022 at 3:25 pmRobAnsys Employee
Looks like the water can't get under the bridge quickly enough so builds up. Have a look at flooding around bridges: it's an irregular problem!
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2022 Copyright ANSYS, Inc. All rights reserved.