TAGGED: evaporation-condensation
-
-
May 6, 2021 at 1:16 pmNavsingSubscriber
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.
-
May 6, 2021 at 4:47 pmRobForum ModeratorI'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.
-
May 7, 2021 at 2:22 pm
-
May 7, 2021 at 2:56 pmRobForum ModeratorWhat is the operating density relative to the density at the pressure boundary?
-
May 7, 2021 at 8:30 pmNavsingSubscriberI'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
-
May 10, 2021 at 12:37 pmRobForum ModeratorDoes the vapour density vary with temperature?
-
May 10, 2021 at 2:04 pmNavsingSubscriberNo 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.
-
May 10, 2021 at 3:43 pmRobForum ModeratorWhat time step are you using? Which multiphase model?
-
May 10, 2021 at 3:54 pmNavsingSubscriberI'm using adaptive time-stepping method with a max global courant number of 0.4 and using VOF method.
-
May 11, 2021 at 9:41 amRobForum ModeratorTry 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.
-
May 11, 2021 at 1:35 pm
-
May 16, 2021 at 1:57 pm
-
May 17, 2021 at 8:31 amRobForum ModeratorLooking 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.
-
June 3, 2021 at 11:57 am
-
June 3, 2021 at 1:45 pmRobForum ModeratorI 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.
-
June 3, 2021 at 7:46 pmNavsingSubscriberYep 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.
-
June 4, 2021 at 11:41 amRobForum ModeratorWhat temperature is the vapour entering at? What is the pipe thermal boundary condition?
-
June 8, 2021 at 10:02 amNavsingSubscriberThe 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.
-
June 8, 2021 at 11:09 amRobForum ModeratorPut 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?
-
June 8, 2021 at 11:47 amNavsingSubscriberOk 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).
-
June 8, 2021 at 3:59 pmRobForum ModeratorOutflow or pressure outlet? If it's the former, change it now!
-
June 9, 2021 at 10:04 amNavsingSubscriberIt 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?
-
June 9, 2021 at 10:56 amRobForum ModeratorUse 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.
-
June 14, 2021 at 11:29 amNavsingSubscriberUsing 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.
-
June 14, 2021 at 1:00 pmRobForum ModeratorCan 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).
-
June 14, 2021 at 1:24 pm
-
June 14, 2021 at 1:37 pmNavsingSubscriberOne 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.
-
June 14, 2021 at 1:37 pmRobForum ModeratorPerfect, 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).
-
July 9, 2021 at 9:36 amNavsingSubscriberI 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?
-
July 9, 2021 at 2:10 pmRobForum ModeratorWhat is that vertical boundary defined as?
-
July 12, 2021 at 10:05 amNavsingSubscriberIt 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.
-
July 12, 2021 at 1:38 pmRobForum ModeratorTurn wall adhesion off for that wall.
-
July 13, 2021 at 3:12 pmNavsingSubscriberThanks 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.
-
July 13, 2021 at 4:04 pmRobForum ModeratorWhat 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?
-
July 14, 2021 at 10:28 amNavsingSubscriberI'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?
-
July 14, 2021 at 12:52 pmRobForum ModeratorIf 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!
-
July 14, 2021 at 2:08 pmNavsingSubscriberThanks 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.
-
July 14, 2021 at 2:30 pmRobForum ModeratorYou 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.
-
July 15, 2021 at 2:23 pm
-
July 15, 2021 at 3:08 pmRobForum ModeratorLooks good. You may need a lot of mesh to pick up the instabilities that lead to break up though.
-
April 4, 2022 at 5:47 pmshitizsehgalSubscriberHope 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
-
August 22, 2023 at 7:26 amsinan ozbolgiliSubscriber
Dear Navsing,
What is contunity ? is it comvatage ? how you go till 0.3 second with 10^-9 time step?
-
- The topic ‘Using a pressure inlet/outlet condition in fluent’ is closed to new replies.
- Non-Intersected faces found for matching interface periodic-walls
- Unburnt Hydrocarbons contour in ANSYS FORTE for sector mesh
- Fluent fails with Intel MPI protocol on 2 nodes
- Help: About the expression of turbulent viscosity in Realizable k-e model
- Cyclone (Stairmand) simulation using RSM
- error udf
- Mass Conservation Issue in Methane Pyrolysis Shock Tube Simulation
- Script Error
- Facing trouble regarding setting up boundary conditions for SOEC Modeling
- UDF, Fluent: Access count of iterations for “Steady Statistics”
-
1411
-
599
-
591
-
555
-
366
© 2025 Copyright ANSYS, Inc. All rights reserved.