Fluids

Fluids

Interpolating species fractions from nearby cells during pressure outlet backflow?

    • julia.hartig
      Subscriber

      Hey all,

      I'm running a transient simulation where backflow occurs periodically through the outlet (a "pressure outflow" BC) due to domain vibration. Since the species fractions near the outlet are time-dependent, there is no appropriate constant mole fraction to set for backflow - at the start of the simulation (i.e t=0s), the backflow condition is most appropriately described by ambient conditions (i.e. n2~0.78, o2~0.22) but as the simulation progresses and product gases reach the outlet, we would expect a more complex stream also containing our byproducts (methane, etc.). I've noticed this is introducing oscillations at the outlet and other unphysical behavior.

      I would like to have Fluent assign backflow species concentrations based on the nearest neighboring cell or collection of cells (i.e. closest "downstream" cell) which I should be able to do with a UDF, but I only see options for a constant, parameter-based or expression-based assignment in the species dialog box of the pressure BC. It seems like maybe this would be possible with an expression, since this has a "Locations" dropdown containing my outlet (i.e. 'outlet-top') but I don't know how to reference specific properties/simulation values at this location.

      Any advice on how to tackle this issue would be greatly appreciated! I'm leafing through the Users Guide but not seeing any examples relevant to what I'm trying to do so far.

    • Rob
      Ansys Employee
      Expressions ought to do it, but you may need to use the average value from the near boundary region. The facet value on the boundary should include the boundary setting in the calculation so may not be what you want.
    • julia.hartig
      Subscriber
      Rob Okay that makes sense. I'm really close... but I can't figure out how to make a near-outlet region that will actually appear in the "Locations -> Boundary Zones/Surfaces" dropdown. I created a surface, "outlet_line", but it's not recognized by the expressions utility. If I override it (hardcode the location to "outlet_line") it says that region is invalid.
      I guess one way to do this would be to split the outlet tube into two pieces, mesh the interface, and then use that interface as the species averaging location? I hate to do this because it requires reimporting the mesh and redoing the case, and won't be very flexible if I find a better location to extrapolate species fractions from, but maybe this is the only option? What do you think?
    • Rob
      Ansys Employee
      You need to split the mesh to get a "proper" surface, but try with a plane too as some of the tools work on those but not iso-surfaces. If the mesh is fairly well aligned near the outlet you can use a register to split the mesh in Fluent. No need to re-mesh.
    • julia.hartig
      Subscriber
      I didn't realize you could split the mesh inside Fluent directly, your suggestion is a much easier approach :) Unfortunately the "Surfaces -> New -> Plane" option is greyed out since I'm working in 2D, so I tried splitting with a register. So far it's running without issues, I'll have to see how the results look when it finishes.
    • DrAmine
      Ansys Employee
      Using udf and providing the t0 value on the face profile.
    • julia.hartig
      Subscriber
      The simulation just finished and the backflow results look good so I think this worked. Thanks for the help Rob! :)
Viewing 6 reply threads
  • You must be logged in to reply to this topic.