Fluids

Fluids

Gas Mixture Nozzle Flow

    • MRMR
      Subscriber

      Hello

      I didnt find the solution for my problem in available CFX tutorials so I decided to try getting help here.

      I'm trying to simulate a steady state nozzle air flow with "holes" in the side wall as additional inlets for methane combustion exhaust fumes.

      A simplified solid is presented in a picture below.



      In fluid domain settings I would like to use "Air Ideal Gas" for the main Inlet (invisible in the picture, rectangular face from the side of coordinate arrows). The next aspect is is to define exhaust gases for side Inlets (in red circle): I used stoichiometric data from methane combustion, so I chose from the material library data four fluids:


      - CO2 Ideal Gas (Volume Fraction in Inlet Fluid Values - 0.095)
      - Water Ideal Gas (Vol. Fraction 0.19)
      - N2  Ideal Gas (Vol. Fraction 0.715)


      All of them as continuous Fluids; ref. pressure = 0; Non Buoyant Model; Stationary; None Mesh Deformation.


      And in Fluid Models I got the problems:
      From ANSYS Help I got the information: In homogeneous multiphase flow, a common flow field is shared by all fluids, as well as other relevant fields such as temperature and turbulence. 

      In my model the exhaust gases are joining the air flow and it's not all mixed from the beginning. So I didnt use this option.

      The second option: Homogeneous Model of Heat Transfer I also didnt use, but if someone could explain this to me I would be grateful. I included Viscous Work Term and Total Energy (due to Kinetic energy impact I cannot use the Thermal Energy model).

      In Turbulence I didnt use Homogeneous Model neither and no combustion or thermal radation is considered.
      I used the option "Fluid Dependent" Turbulence, so in Fluid Specific Models part I chose for all components  SST Turbulence Model with automatic wall function. 

      And in the next part there is my biggest issue: In Fluid Par Models I have one "Mixture Model" Interphase Transfer with basic 1 mm Interface Len. Scale a basic Drag Coefficiend of 0.44 in Drag Force. None Mass Transfer is included. How can I properly specify Heat Transfer between each Fluid Pair? 

      Boundary conditions
      Main Air Inlet - Static Pressure 0.18 MPa, Zero Gradient Flow, Temp 900C, Volume Fraction Air 1, rest fluids 0.
      Inlet 2 and 3 on the both sides of the nozzle: Static/Total pressure will be calculated later, but I need to get an ejection of fumes into the nozzle; flow - normal to boundary and static temperature of 1300C. I will repeat the Volume Fractions for these Inlets:
      - CO2  0.095
      - Water Ideal Gas 0.19
      - N2  Ideal Gas 0.715
      - Air 0

      Outlet Av. Static Pressure 0.11 MPa (Ref. Pressure = 0). Wall of the nozzle is heated, and its' fixed temperature is 1100C.
      Wall Contact Model: Use Volume Fraction.

       Archive file attached - "1". 


       

    • DrAmine
      Ansys Employee

      You do need to Gas Mixture and not Multiphase Model. Just define a custom material with variable composition / fixed composition and use that material as your fluid.

    • DrAmine
      Ansys Employee

      Moreover ANSYS Staff does not look into attachments but others can do.

    • MRMR
      Subscriber

      Hello Amine, thank you for your answer.

      I created the Fixed Composition Gas Mixture but in my Domain I still do have two fluids (air for the main Inlet, and Mixture for the Side Inlets) and due to this I still have this FLUID MODELS card with all "homogeneous model" options for Multiphase, Heat Transfer and Turbulence. When I will not use any of them I still have to define Heat Transfer (Coefficient or Nusselt Number or other) and Interface Len. Scae and Drag Force in Fluid Par Models part.

    • MRMR
      Subscriber

      Hello, does anybody have an idea how to specify this heat transfer coefficient (air vs exhaust methane fumes)?

    • DrAmine
      Ansys Employee

      So actually you require variable composition mixture including air.

    • MRMR
      Subscriber

      Thank you Amine for you help and commitment. Unfortunately I have to admit, that I'm a bit confused and probably got lost. 

      When I choose variable composition mixture, I use Calorically Perfect Ideal Gases Material Group and beneath I choose Air, CO2, N2 and Water - all ideal gases. 
      Then I choose the thermodynamic state of the mixture as a gas. I left Mixture Properties and didnt touch them. 
      In the next step I chose my mixture as Fluid in my Domain - Model SST with Viscous Heat Term and in Component Models I have all my fluids.
      Nonetheless I got an error "One constraint component is required for the component fluid models. When I change the option from "Transport Equation" to "Constraint" for one of them it disappear from one of the inlet boundary condition (in the main one or in the both side ones - depends which one I choose)

      Could you explain me what does this constraint option stand for? I cannot find it in ANSYS help or even in any other forum cases.

      As a reminder
      - my main inlet is an air one where I choose Mass Fraction 1 for Air and 0 for the rest
      - my side inlets are for combustion fumes, where I choose Mass Fraction 0 for Air and corresponding values for each fraction CO2, N2, Water

      Thank you again Amine for all your answers.

    • DrAmine
      Ansys Employee
      constraint specie is the blast one which will get algebraicly as 1-mass fraction of all other species which would be solved via dedicated transport equations.
    • DrAmine
      Ansys Employee
      usually one would make the most abundant specie as the constraint one.
    • MRMR
      Subscriber

      Thank you again Amine for your answers, especially that time. Unfortunately I'm afraid I'm not sure how it will work in my case, sorry. Could you try to explain one last time?

    • DrAmine
      Ansys Employee
      Don't worry. You have 4 species or components. One of the them should be a constraint. One generally take the abundant specie (like air in wet air) as constraint.

      Now at the boundary where air enters: you provide zero mass fraction for the other 3 species. This results in having mass fraction of air at that boundary to be equal to 1.
    • MRMR
      Subscriber

      Thank you very much - I got it. The problem is even funny, because when I changed all the options you said CFX showed me 3 mistakes for each inlet that "Air Ideal Gas is included" and should not.. And all I had to do is to go to each Inlet boundary again and approve the changes - that's all, that was what the hole incomprehension was about.. 

      Thank you again, now I will check what the simulation process will show me. 

      Regards

    • DrAmine
      Ansys Employee

      Welcome!

Viewing 12 reply threads
  • You must be logged in to reply to this topic.