Fluids

Fluids

Topics relate to Fluent, CFX, Turbogrid and more

DPM Non-continuous particle tracks

    • Aayushya Agarwal
      Subscriber

      I'm trying to simulate a multi phase flow of the following geometry, where discrete particles are being injected from the surface on the left

       

      I have inserted a Rosin-Rammler distribution of particle diameters with anywhere from 100-100000 streams and randomized the initial starting point. However, when I plot the particle trajectories, they seems to be non-continuous. Below I've attached two examples of the particle traces near the outlet. The two examples are of 1000 streams and 100,000 streams

       

      When I sample the dpm on the outlet boundary, the plot looks like particles are clumped rather than spread evenly. This geometry models a printer where I expect the particles to deposit in all regions of the outlet (however with a distribution). I see in the simulation that even with more streams I am getting the same areas with no particles depositing. I'd appreciate the help. Thanks

       

    • Rob
      Forum Moderator

      Have a look at the flow field. Is gravity on, and are you modelling 3d, 2d or 2d axisymmetric? 

    • Aayushya Agarwal
      Subscriber

      This is a contour of our flow field. We are using a 2D axisymmetric model:

    • Rob
      Forum Moderator

      OK. Now, if particles are funnelled to the axis through the domain, why would they not remain in the centre? 

    • Aayushya Agarwal
      Subscriber

      I agree the particles should remain in the center. My question is regarding the discrete nature of where the particles land. You can notice that there are gaps between where the particles land, as shown in the figure below. And no matter how many particles I inject, or I randomize the initial starting points on the surface, this gap remains. I would expect with a large number of particles there should be a continuous deposition

       

       

    • Rob
      Forum Moderator

      Please can you overlay the particle tracks with velocity contour and mesh? You may need two images, one with contour node values on, and a second with them off. 

       

    • Aayushya Agarwal
      Subscriber

       

       

      I’ve attached plots of the particles tracks with the velocity contour and the mesh below. Thanks

       

       

       

    • Rob
      Forum Moderator

      Thanks. It looks like you've got some particles outside of the jet core, the remainder are not seeing enough radial force (or stocastic kick) to spread out. 

    • Aayushya Agarwal
      Subscriber

      Would the answer then to be have a higher fluid flow rate, or maybe a better initial velocity for the particles?

    • Rob
      Forum Moderator

      To spread the particles out? 

      Initial velocity may not do much as their trajectory by the outlet is pretty much entirely determined by the nozzle and entrainment inlet. 

      I would check the flow near the outlet in more detail - in the two velocity images it looks like the fluid jet is very diffuse. Is that mesh or convergence related? How "good" are the backflow conditions? 

    • Aayushya Agarwal
      Subscriber

      I want to remove the discreteness of the particle trajectories near the outlet as shown below

       

      Here are the boundary condition settings for the outlet:

       

      And here is the mesh near the outlet:

       

      Here is the velocity magnitude and radial velocity of the fluid near the outlet:

       

       

    • Rob
      Forum Moderator

      Try "neighbouring cell" on the backflow direction. The radial velocity looks very odd on the last image. 

      To clarify, you're running 100k particle tracks and displaying those? Have you got stochastic tries turned on? 

       

    • Aayushya Agarwal
      Subscriber

      I have tried making the backflow direction specification method as "From Neighboring Cell". Here is the particle trajectories and radial velocity contour now:

       

       

      Also yes I am displaying the 1000 particle tracks. I have the randomize starting points on, but I don't have turbulent dispersion so I'm not able to do the stochastic tries

       

       

    • Rob
      Forum Moderator

      No turbulence? 

    • Aayushya Agarwal
      Subscriber

      I have the fluid model set to laminar:

      And in the discrete particle settings, I'm unable to select turbulent dispersion. If I understand correctly that's where I select stochastic tries

    • Rob
      Forum Moderator

      OK, no turbulence so no stochastic tracking: it uses the turbulent values to kick the trajectories in a random way. 

      In your case the streams are released from the inlet face,and will then follow the flow. I'd then expect some discrete particle tracks. Remember we're tracking parcels rather than particles. 

Viewing 15 reply threads
  • The topic ‘DPM Non-continuous particle tracks’ is closed to new replies.