Pressure drop fluidized bed simulation

Hello, 

Using the multiphasic eulerian model, a simulation of fluidized bed with air and sand was made.

My issue is that I don´t have access to the pressure drop value in the post processing interface.

Indeed, nor the static and dynaçic pressure give the espected pressure drop (cf figure attached).

I know this is a specific question but science scientific progress lies in details, so : 

How can the pressure drop be obtained ? Or, how can we have access to the Gidaspow drag function which is required to calculate the interphase pressure term (cf equation below)?

Message in a bottle, may someone find the answer. Thanks

K_{sl} = 150\frac{\alpha_s (1-\alpha_l) \mu_l}{\alpha_l d_s^... ...5\frac{\rho_l \alpha_s \vert \vec v_s - \vec v_l \vert } {d_s}

«1

Comments

  • DrAmineDrAmine GermanyForum Coordinator
    edited October 2018

    There is no direct pressure drop value. You need to evaluate it on your own by creating some Report definitions in Fluent at the required locations (say inflow / outflow or above/below the bed) and then build-up the difference. 

  • maxime87maxime87 Member
    edited October 2018

    Hey Amine , thanks for your answer .

    at the outflow the pressure is atmospheric so I don't need to calculate the difference.

    I want to access the drag coefficient Ksl = Pressure drop/(Velocity*Height of the bed ) to reach the right drag pressure. That's what gives me headache

    Regards, 

    Maxime 

     

  • DrAmineDrAmine GermanyForum Coordinator
    edited October 2018

    There is no documented official way to access it. You can write your own drag function. 

  • maxime87maxime87 Member
    edited November 2018

    All right, maybe I can try to use the data in order to calculate this coefficient during the simulation but I don't know how.

    How can I do this : generate the Ks coefficient while the simulation is rolling ?

    Thanks

    Maxime 

     

  • DrAmineDrAmine GermanyForum Coordinator
    edited November 2018

    You need to use DEFINE_ADJUST Macro to write the whole formulation and write it into a cell UDMI (C_UDMI) to have it post-processed. 

    But why do you need to now it?  Actually one is interested to get the pressure drop as you highlighted but not the drag coefficient which is used in the modeling strategy. 

  • maxime87maxime87 Member
    edited November 2018

    Interesting,

    The pressure drop that I am looking for depends on this coefficient (Ksl = Pressure drop/(Velocity*Height of the bed ) ) and I don't have access to it.

    Indeed while I'm looking at the static pressure in the post-processing, it gives the value of the bed's weight not the pressure due to the gas-solid interactions which depends on the velocity (cf curve above). This pressure is the result of the gas phase force applied on the granular phase and unfortunately I don't see how I can obtain it in the Fluent's interface.

    But your proposal DEFINE_AJUST may be an answer.

    Thanks again 

     

    Maxime 

  • DrAmineDrAmine GermanyForum Coordinator
    edited November 2018

    Ksl is a part of drag after Ergun. Saying that the result what you get for pressure drop will be in line with it. Please have a look into the documentation.

  • maxime87maxime87 Member
    edited November 2018

    Yes, Fluent compute Ergun's Equation but the question is where is the result of this calculus?

    Best regards,

     Maxime

  • DrAmineDrAmine GermanyForum Coordinator
    edited November 2018

    The results is used to model the drag force. This is done in every cell and you want the information at global level between below and above the bed. Just post-process the pressure and you will have your pressure drop curve. That is what we did x times before.

  • maxime87maxime87 Member
    edited November 2018

    Ok, I did this at the beginning and it gives me a constant value equal to the bed's weight (no matter the velocity), not the curve above.

    Maybe you can give me an example of fluidized bed simulation involving this tecnique ? 

    Thks,

     

    Maxime 

  • RobRob UKForum Coordinator
    edited November 2018

    If the model is converged and you've not blown the bed out of the domain (you won't be the first person to do this) the pressure should increase with velocity. 

  • DrAmineDrAmine GermanyForum Coordinator
    edited November 2018

    Now we got your point: Ok, I did this at the beginning and it gives me a constant value equal to the bed's weight (no matter the velocity), not the curve above."

    As ANSYS Staff I cannot share any examples not stated as tutorials.  I can just tell you: a static bed is not only supported by the inlet. In reality, for static beds it is shown experimentally that the lateral walls contribute in supporting the bed mass. The particulate media creates some arches in contact which the lateral walls due to friction. This arches then support the particle mass above. Of course it depends on the ratio between the bed high and its diameter. A correction of fricitional pressure might allow the prediction of the pressure drop below the minimum fluidization velocity. I will update one more time whenever I have something to add.

  • maxime87maxime87 Member
    edited November 2018

    Hi again

     

    Thank you for your nice description of wall effects.

    The issue here is that I still don´t know how to acess the Ergun´s pressure drop that is computed in the Gidaspow model ( LINK removed)

    Maybe I have to recompute this by myself extracting the fluent´s data ?

     

    Best regards

    Maxime Taupiac 

     

  • maxime87maxime87 Member
    edited November 2018

    The simulation pressure curve (red) that I have for an inlet velocity equal to 0 (red) in function of the flow time is this one : 

  • DrAmineDrAmine GermanyForum Coordinator
    edited November 2018

    Recomputing the function itself is not the solution as the value will be cell dependent and you want to have a global variable. 

  • maxime87maxime87 Member
    edited November 2018

    Yes, I am trying to do averages in order to have the drag pressure but that's not really good. Maybe it like rwoolhou said is about the boundary and initial conditions.

    Thanks

     

    Maxime Taupiac

  • DrAmineDrAmine GermanyForum Coordinator
    edited November 2018

    Yes but as I said I remember that a correction of frictional pressure might allow the prediction of the pressure drop below the minimum fluidization velocity. 

    You can check if with DDPM + DEM you can obtain without any additional modification. But with DEM that would be expensive (based on the loading you have).

  • maxime87maxime87 Member
    edited November 2018

    Hello Mr rwoolhou,

    what do you mean by "blowing out the bed" ? Because, yes the simulation converges and the bed is moving between the boundaries quite normally.

     

    Thank you for your advice.

     

    Maxime

  • DrAmineDrAmine GermanyForum Coordinator
    edited November 2018

    blown down out =  No bed anymore in the domain

  • maxime87maxime87 Member
    edited December 2018

    Hi again Amine, 

    I tried like you said a 2D DEM-DDPM with collisions simulation with a manual injection (I did a rectangular pile of 92605 particles). Two main issues occured. Firstly the initial bed packing is very low (~10^-4-10^-5 and I want 0,5 (cf picture) ) and secondly the overlap is really important. 

    I keep the default collision parameters, the particle's diameter is 325um. During the calculation, a lot of particles escaped and there was a problem of tracking within the espected residence time... 

    Is there a way to solve both these issues ?

    Thanks

Sign In or Register to comment.