Fluids

Fluids

Results not converging in open channel flow

    • pv00170
      Subscriber

      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)

       Boundary conditions:

      • 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

      My questions:

      • 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?

       

    • Rob
      Ansys 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?

      • pv00170
        Subscriber

        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?

    • Rob
      Ansys 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  

       

      • pv00170
        Subscriber

        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.

    • Rob
      Ansys 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. 

       

      • pv00170
        Subscriber

        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

    • Rob
      Ansys Employee

      There are force reports on walls, along with volume reports to find out how much air is trapped under the deck. 

      • pv00170
        Subscriber

        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 
    • Rob
      Ansys 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. 

      • pv00170
        Subscriber

        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?

    • pv00170
      Subscriber

      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.

      With "If you look there are also forces (x, y & z) as opposed to lift & drag" do you mean negative values?

    • Rob
      Ansys 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. 

      • pv00170
        Subscriber

        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)

    • Rob
      Ansys 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. 

      • pv00170
        Subscriber

        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. 

      • pv00170
        Subscriber

        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…


         

    • Rob
      Ansys 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! 

Viewing 9 reply threads
  • You must be logged in to reply to this topic.