Fluids

Fluids

Topics related to Fluent, CFX, Turbogrid and more.

Multiphase flow – Free surface jet deviation to analytic solution

    • christian.scheffler
      Subscriber

      Hi all,

      I have an issue regarding the propagation of a free surface jet in ANSYS CFX.
      The trajectory length of the jet does not fit to the analytic value of the horizontal throw.
      There seems to be a kind of damping or energy loss.
      What might be the problem?

      Settings are:
      1st phase = Jet: Water, 2nd phase: Air
      Steady State
      Advection Scheme: High resolution
      Isothermal 25°C
      Laminar flow
      Morphology: Continuous Fluid
      Buoyant: Gravity y-direction: 9.81m/s
      Fluid Models: Multiphase Free Surface Model: Standard (i.e. Homogeneous Model not activated)
      Fluid Specific Models: Fluid Buoyancy Model: Density Difference
      Fluid Pair Models: Interphase Transfer: Free Surface
      Fluid Pair Models: Momentum Transfer: Drag Coefficient 0.44
      Fluid Pair Models: Surface tension not activated
      Solver Control: Advanced Options: Multiphase Control - Volume Fraction Coupling: Segregated
      Inflow: Normal velocity 4m/s, 1.0 water, 0.0 Air

      Could somebody help??

      Comparison between free surface jet and anayltic trajectory

    • Rob
      Forum Moderator

      I assume you've resolved the jet and converged the solution. Where is the drag/viscosity term in the theoretical correlation?

    • christian.scheffler
      Subscriber

      Convergence more or less, at least the Pressure and Momentum RMS residuals for the water fraction are below 1e-4. Do you consider this as a problem?

      Convergence

      I set the drag coefficient to 0.0 and it seems to have a great influence; however, there is still a difference to the analytical solution.

      Comparison Free surface jet with drag coefficient 0.0
      Regarding your question: No, there is no drag force considered in the simple analytical throw trajectory equation.

      I would like to understand which parameters influence the solution.
      Any ideas?I will try to test air with very low density and pressure and see if the orgin of the "loss" problem could be there.

    • Rob
      Forum Moderator

      I didn't think there was a drag coefficient for the VOF model? Convergence isn't good, but I don't use CFX so am unsure how bad it is. The person I'd usually ask isn't back in yet, but another colleague looks to be in. 

      We can't model vacuum, but see what dropping the gas density and viscosity does. 

    • Rob
      Forum Moderator

      OK, having spoken to someone who covers CFX. You're using the drag coefficient to adjust momentum exchange between the two fluids so as the analytical model has no drag the result will be different. 

      Convergence isn't good either. 

    • christian.scheffler
      Subscriber

      I tested air pressure/density at 20000m level -> no visible influence. 

      Convergence is almost below 1e-4 RMS for all momentums. But I am not sure if RMS assessment is correct for such a large area where only a small number of cells contain the water jet.
      Any ideas how to improve convergence for the steady state analysis? Timescale settings? Note: The distance of the jet in x is about 1m, that means a travel duration of about 0.25s for one fluid particle.

      Convergence Momentums and Volume Fractions

      I will test to increase jet size in order to minimize interface losses between the two fractions air/water and increase the cell number trying to improve convergence.

      Reducing the drag coefficient from 0.44 to 0.0 seems to had the biggest impact.

      Any other ideas are welcome.

       

    • Rob
      Forum Moderator

      Check the fluid model too - you're dragging air with the jet, hence the significant difference when you reduce the drag coefficient. 

      How well refined is the mesh in the jet?  Reducing the time scale should help improve convergence too. 

    • christian.scheffler
      Subscriber

      Now the free surface jet and the analytic solution is more or less equal. The model needed the following changes compared to the above settings:

      • use openings for left and right wall instead of wall left and outlet/wall right
      • setting a physical timescale of 0.05

      This improved significantly the convergence.
      Neither one of the settings alone did the trick.
      The timescale value (time step) is just a guess, I didn’t calculated it based on the Solver Theory Guide. But it is certainly a better option to calc it according to 1.273, 1.274, 1.275 (2023R1). Just to mention it here: the jet velocity is 4m/s, the dimension of the jet in x about 1m, the cell size 1.5mm x 1.5 mm x 1.0 mm. The jet width is resolved by about 10 cells.

      Comparison free surface jet to analytical solution

      Convergence

Viewing 7 reply threads
  • The topic ‘Multiphase flow – Free surface jet deviation to analytic solution’ is closed to new replies.