Fluids

Fluids

Topics related to Fluent, CFX, Turbogrid and more.

Using a pressure inlet/outlet condition in fluent

    • Navsing
      Subscriber

      Hi

      I'm simulating a 2D multiphase phase change problem of water vapour condensing ontop of a pipe wall. I'm currently following a paper to validate my simulation. However in the paper they use OpenFoam to simulate the problem in which the boundary conditions they state are slightly different.

      For example on the figure below at boundary b), they use a pressure inlet/outlet boundary condition where the boundary condition switches between being a zerograident condition when outflow occurs and a fixedvalue when inflow occurs.

      In my case I will have outflow and inflow since the water vapour will be coming into the domain as the wall temperature is below the saturation temperature of the fluid domain (50 K difference) and outflow will occur as the condensate will drip off the pipe and exit the domain.



    • Rob
      Forum Moderator
      I'd use a pressure inlet around b) and then a pressure outlet at e) How much condensation are you expecting as the gas space is tiny.
    • Navsing
      Subscriber
      I've tried this and my condensate is breaking at the wall interface due to a large velocity flow towards the pipe. And I'm expecting around 0.1 to 0.2 mm of condensate around the pipe.


    • Rob
      Forum Moderator
      What is the operating density relative to the density at the pressure boundary?
    • Navsing
      Subscriber
      I've set the operating density to be equal to the phase that has the lowest density. So in this case it would be the water vapour at a density value of 0.5981 kg/m3
    • Rob
      Forum Moderator
      Does the vapour density vary with temperature?
    • Navsing
      Subscriber
      No it is constant which is set at that value. But my condensate density does vary with temperature in order to prevent the simulation from using the Boussinesq approximation to determine the buoyancy forces. My simultion did not work untill I did that.
    • Rob
      Forum Moderator
      What time step are you using? Which multiphase model?
    • Navsing
      Subscriber
      I'm using adaptive time-stepping method with a max global courant number of 0.4 and using VOF method.
    • Rob
      Forum Moderator
      Try dropping the time step and setting it as fixed. As vapour condenses the volume change is large, and if the initial condition is such that a lot of condensation is created the model may not be very stable.
    • Navsing
      Subscriber
      Ok will do, but initially the condensate forming on the pipe is quite stable show here:
      But as the water liquid starts to leave the pipe, that's where the instability begins.



    • Navsing
      Subscriber
      I've set my time-step to be 1e-08 but I still get vortices forming around the condensate.


    • Rob
      Forum Moderator
      Looking at the two images that's the free surface trying to bunch up. I assume you have surface tension on? As the film builds up and then drips you may find the time step gets very small as the liquid snapping (dripping) could be a fairly fast process.
    • Navsing
      Subscriber
      Yep I have surface tension. And you're right the time-step does get very small as the liquid starts dripping off. The liquid film starts breaking up into droplets (Rayleigh instability).


    • Rob
      Forum Moderator
      I assume the solver is set as laminar? Check the backflow condition and turn on the stability controls for VOF in the solver panel in 2021R1 if you can use the current release.
    • Navsing
      Subscriber
      Yep my flow is laminar. I actually have reversed flow in my case which is fine since its just the water-vapour entering the domain. I tried turning on the stability controls but the simulation crashed instantly so I'll think I'll leave that for now.
    • Rob
      Forum Moderator
      What temperature is the vapour entering at? What is the pipe thermal boundary condition?
    • Navsing
      Subscriber
      The temperature of the vapour is at saturation i.e. 373.15 K and the boundary condition of the pipe is 50K lower than of the surrounding temperature so 323.15 K. The boundary condition I set on the side wall is a slip wall with zero heat flux.
    • Rob
      Forum Moderator
      Put the vapour in a few degrees warmer. If you're at the dewpoint it'll try and condense immediately especially if the solver under/over shoots on temperature in the first few time steps. To add, I assume there's a pressure boundary somewhere too to allow for the volume change?
    • Navsing
      Subscriber
      Ok and yeah I have a outflow boundary condition at the outer side-walls where the condensate leaves the domain. The whole domain is set at atmospheric conditions (p = 1 atm).
    • Rob
      Forum Moderator
      Outflow or pressure outlet? If it's the former, change it now!
    • Navsing
      Subscriber
      It is outflow. I did use pressure-outlet before but I'm uncertain of what to put for the backflow volume fraction condition of the water-vapour phase as if I set it to 1, the condensate will not leave the domain and if I set it to 0, condensation will start to occur on the outlets?
    • Rob
      Forum Moderator
      Use pressure outlet, set the temperature to the free stream value and vapour vol fraction to 1 (ie whatever is in the far field). Outflow is an old boundary type which predates compressible flow and multiphase modelling. It should only be used for incompressible systems with velocity inlets and even then we rarely (never) use it now.
    • Navsing
      Subscriber
      Using the pressure-outlet causes the film to break-up to form droplets on the surface of the tube, which it shouldn't as the contact angle of the tube is 0┬░ so it should have a continous film ontop. If I use outflow it gives me this thin film initally. This was the reason why I didn't use pressure-outlet before.


    • Rob
      Forum Moderator
      Can you replot those images with node values off? I want to see what the solver is calculating, not what is displayed (with a fine enough mesh they're about the same).
    • Navsing
      Subscriber
      Ok like this?

    • Navsing
      Subscriber
      One other thing I should add, to get this continous liquid film using outflow I made my surface tension, density and viscosity as a function of temperature for the water in the materials properties. Without it I dont get the condensate film.
    • Rob
      Forum Moderator
      Perfect, thanks. That explains the issue. You need more near wall mesh as you're not resolving the film. The droplets are formed either due to numerical issues or surface tension: hard to tell which without a very careful look at the model (which I won't be doing).
    • Navsing
      Subscriber
      I managed to make my simulation better now by refining my mesh and using the pressure outlet condition as you stated. However I'm getting this large velocity vector gradient at the bottom side wall which is preventing the condensate from leaving at the tube edge and instead fall slightly adjacent to it. Any idea what could be causing that?

    • Rob
      Forum Moderator
      What is that vertical boundary defined as?
    • Navsing
      Subscriber
      It is defined as a wall slip condition (i.e. 0 shear stress in x and y direction). Contact angle is set to 0┬░ and the heat flux is set to zero so it is an adiabetic wall.
    • Rob
      Forum Moderator
      Turn wall adhesion off for that wall.
    • Navsing
      Subscriber
      Thanks for that. Yeah I've done it and it seems better initally. But after around 0.3 s the adjacent droplet still forms and the falling film starts to thin? And as the adjacent drop falls the flow becomes very unstable and causes the velocity to shoot up for some reason. Should I try to reduce the time-step lower? I'm using a Courant number of 0.1 and set the minimum time step size to 1e-09 s.


    • Rob
      Forum Moderator
      What surface tension value are you using? Zoom in on the interesting parts and see what's going on. Whilst I would usually expect the fluid to reach the bottom and drip, if the film is too thick or viscosity is high it may try and drip before it reaches the bottom. How well converged is it?
    • Navsing
      Subscriber
      I'm actually playing with the surface tension value to see what effect it has on my simulation. At the moment it is set at 0.001 N/m so yes it is quite viscous and does drip. However when I set the surface tension to water (0.072 N/m) droplets start to form. I don't know if this is supposed to happen as theorectically I know that filmwise condensation should occur as the contact angle of the wall is set to 0┬░. And my simulation is quite stable as seen from the residuals. Should I carry on leaving my simulation running to see what happens to the droplets?


    • Rob
      Forum Moderator
      If contact angle is zero the liquid will either bead or stick depending on the phase order. 0.001 N/m isn't that high a surface tension, it you confused the units it's also not all that viscous. Re the beading model, run and see what happens: that's what simulation is for!
    • Navsing
      Subscriber
      Thanks for that. I understand where the problem is now. In order to initalize the fluid domain with water vapour I had to swap the phases around i.e. condensate to water vapour. When I select the contact angle of the wall it states that the contact angle is between water vapour and condensate which means that the contact angle of the wall should 180┬░ instead of 0┬░ as the contact angle is measured inside the primary phase. I did this now and get filmwise condensation.


    • Rob
      Forum Moderator
      You shouldn't need to swap the phases, you just patch the zones. So, I may initialise with all vapour and patch the film, or initialise all water and patch the vapour. It's just a case of getting the 0 and 1 in the right place and order.
    • Navsing
      Subscriber
      Ah I see, thanks. My simulation is working fine now, the fluid exists the domain without any instabilites. Probably would be able to see droplet detachment if I extend the domain further down.


    • Rob
      Forum Moderator
      Looks good. You may need a lot of mesh to pick up the instabilities that lead to break up though.
    • shitizsehgal
      Subscriber
      Hope you are doing well. Will it be possible for you to share your settings for the pressure outlet BC? In particular, the backflow settings for volume fraction for phases, backflow temperature, and species you have in your simulation? I am working on a similar problem and your discussion here with @Rob has been of great help so far. I am asking this question to avoid reverse flow on the vapor side of the pressure outlet as the film progresses down. My email is shitizsehgal@tamu.edu
    • sinan ozbolgili
      Subscriber

      Dear Navsing,

       

      What is contunity ? is it comvatage ? how you  go till 0.3 second with 10^-9 time step? 

Viewing 41 reply threads
  • The topic ‘Using a pressure inlet/outlet condition in fluent’ is closed to new replies.