Back flow issue in triangular duct

radsrads Member Posts: 16
edited February 23 in Fluids

Hello all,


I am trying to simulate a PCM-Water hybrid system. One of the pipes contains PCM, while other pipe which is interacting with first one has water flowing through. Heat transfer is taking place from a face of PCM-pipe to PCM and then to water. When I simulate the individual systems, that is, PCM only and water pipe only, in transient state, and all settings same, it works fine. My PCM melts completely, and my water reaches a steady state. But when I combine the systems, and have both of these in same model, I am facing an issue of back-flow, right at the beginning, and it cant be ignored as it goes to about 20-30% in just a few iterations.


I am using SIMPLE model , and have adaptive time step method for calculation. My mesh quality is fine too. What could be the reason for such an issue.




Solving method


Calculation strategy


Residuals


Outlet pressure



Thanks and regards,

Radhika

Answers

  • DrAmineDrAmine GermanyForum Coordinator Posts: 6,642

    Backflow might be issue if not physical. If numerical it should disappear as you move to pseudo steady state. So you have two different cell zones and in each you have a different fluid: please check that. Also ensure that you are doing a proper initialization. Where are you seeing the backflow in the water leg or PCM leg? Which outlet boundary is used there?

  • radsrads Member Posts: 16
    edited February 23

    Yes, both cell zones are different. Backflow is occurring in water leg. It's the outlet of water pipe, with pressure boundary condition. As far as initialisation is concerned, I am using hybrid initialisation.

  • radsrads Member Posts: 16

    Tried to run the simulation for a longer time to see if the backflow issue goes away. But it hast. About 40% of area has backflow throughout the time.


    Residuals


    Outlet pressure on water pipe


    Average temperatures.


    It seems to be giving wrong physical temp, as the outlet of my water has less average temp than the entire water average temp, and this is probably because about 40% of the outlet area has backflow, and the backflow is happening at 300k.


    Also, this simulation was rum by having time step size as 1sec , because 0.01s was too slow. Everything else in setup is same as sent in previous SS.

    Not sure whats going wrong and how to proceed.

  • radsrads Member Posts: 16

    I was just going through the model, and checking the boundary conditions.

    I found some weird lines as this in them


    When i zoom in, it just turns into a line. I tried reloading, re-meshing, and even recreating the entire model from scratch. but these lines dont go away. And I would have assumed it to be some display issue, but I don't think its just that for two reasons:


    1) the same model, when it had only a PCM or Water pipe, and not both together, did not display such issues.

    2) When i checked the temperature and pressure gradients in one of the runs of this model, I rem getting very weird contours with these lines being approximately the dividing points. That is, from inlet to this line, the contours were physically plausible, but beyond this line division, got weird.


    If any of you could give me some insights, it would be helpful. Thanks.

  • RobRob UKForum Coordinator Posts: 8,371
    edited February 24

    That line is the partition as you're running in parallel, it's graphics and can be ignored. There's a tick box option in 2021R1 to turn them off.

    Back flow is a different issue. Check the flow field to see what is causing this, what is different in the heat transfer from the separate models to the combined case?

  • DrAmineDrAmine GermanyForum Coordinator Posts: 6,642

    Do not use Hybrid if you are starting from initial time = 0.0 [s]. Use real state as starting point of unsteady run.

  • radsrads Member Posts: 16
    edited February 25

    Okay @Rob , I tried running the simulation and realized that the line dint have any effect. There is practically no difference in combined model and individual. In the individual water model, I have only suppressed the pcm domain keeping all other boundary conditions and domains intact.


    @DrAmine I even tried using standard hybridization, but it seems to have no effect.


    I did some post processing and realized a couple of things:

    1) when I have just water leg, there is no negative pressure in the outlet.

    2) when I have only PCM, it has negative pressure near one of the top vertices of triangle.

    3) I have tried to replace PCM domain with water, i.e I have two triangular ducts, both having water in them, and still there is no negative pressure in any of the ducts.


    So what I have concluded is, the presence of PCM is somehow causing the water to reduce the pressure much more than normally.

    Another fact u think should be mentioned is, I have gravity enabled. And in all the previous models it was such that the water duct was in South of PCM duct. I tried another model by placing the water duct north of PCM, but it still has the same backflow issue. I have attached a few SS for reference.

    Outlet pressure:

    Water pipe south of PCM (orientation of my model is 30deg to ground)


    Water pipe north of PCM

    Replaced PCM with water, this is outlet of all legs.


    Now I need to understand how exactly is the presence of PCM changing the pressure in water.

    The BC for PCM is, adiabatic for the faces, and three other faces are coupled with pipe.


    Please give me some insights.


    Thank you

  • radsrads Member Posts: 16

    I have done some newer modifications to the model, instead of having pressure outlet, I have an 'Outflow" boundary condition on water leg. This seems to have solved the reversed flow issue, and my average outlet temperature is higher than the entire water average temp (which was wrong in previous model, but now is physically correct).


    One thing that I did notice is that, the entire outlet is currently having negative pressure as seen below.


    And on top of that, even my inlet has negative pressure



    I want to understand if it is okay to have such pressure, because it seems to be quite low.

  • RobRob UKForum Coordinator Posts: 8,371

    Outflow rarely solves anything, it just doesn't report any of the problems: it's an old boundary condition (ie it was in Fluent v2.99) and shouldn't be used.

    Looking at the model, is the flow in the z direction? If so make the domain longer. If density is constant gravity won't do anything.

  • radsrads Member Posts: 16

    @Rob , Thanks for the input on outflow, will keep that in mind.

    As far as domain is concerned, yes there is a flow is in Z direction. I don't want to make the domain longer as the dimensions are according to a physical model. Is it possible to counter it with a change in velocity, like increase or decrease? Or should I move to a turbulent model of some kind? (currently it is a laminar flow).

  • RobRob UKForum Coordinator Posts: 8,371

    It's more that if you don't have enough up and down stream domain the flow is very much forced by the boundary condition: we want developed flow in most cases.

  • radsrads Member Posts: 16

    @Rob Yes that's correct. But what I fail to understand is, why was there no issue when I had a model with just water, with same dimensions and velocity.

  • RobRob UKForum Coordinator Posts: 8,371

    Some of the flow is now a function of the "other" channel. So the boundary conditions are different.

  • radsrads Member Posts: 16

    @Rob , Yeah that makes sense. So in order to check if the boundary condition of PCM was an issue, I made one simulation, wherein I had water replacing PCM, but all the boundary conditions intact. That is, I had shell conduction on the cross-sectional faces of PCM, and coupled BC for the faces in contact with Pipe. So I did not change these when I replaced PCM with water. And to my surprise, there was no backflow in this one too. The simulation ran smoothly and as expected. So, I feel that there is something wrong with my PCM modelling causing such an issue. I have some SS regarding the settings of my PCM and material properties. Please help me understand where the issue might be lying.



    Density : 810kg/m^3 @ 305K

    765kg/m^3 @ 315K

    Cp: 870kg/m^3 @ 305K

    1110kg/m^3 @ 315K


    Thank you

  • RobRob UKForum Coordinator Posts: 8,371

    Don't think anything is wrong. I do suspect it's linked to the heat transfer between the two zones. Talk to your supervisor regarding your model and compare to the experiment. We're limited in what advice we can give, and I think the model is OK but may not represent exactly what you're trying to replicate.

Sign In or Register to comment.