Fluids

Fluids

How to model 2D Taylor-Couette flow using axisymetric boundary condition if Fluent

    • maggakahn
      Subscriber

      Hello,


      I am currently struggling to figure out how to model the classic Taylor-Couette problem in 2D using Fluent. 


      I want to simulate the problem in 2D using a crossection in the z-r plane (see bottom image for ref). Using the axissymetric option i thought i could set up a case as shown in the image below. Where the bottom line is the axis in the middle of the cylinders and the green square is the crossection of the cylinders (i.e fluid domain). Therefore by adding a azimuthal  velocity (normal to the screen) to the bottom wall of the square, it would  be similar to the taylor couette case.


      However i cannot find a way to set a rotating velocity on the inner cylinder in the azimuthal velocity. Fluent only shows x and y as available options for rotational velocity on a wall.


       



      Any suggestion on how to set up this case is greatly appreciated. Thank you very much for reading,


      Best regards,


      Magnus


       


       


       

    • Rob
      Ansys Employee

      You'll need 2d axi-symmetric with swirl. Does that give you any other options? If not you'll need a 3d (possibly periodic) model. 

    • maggakahn
      Subscriber

      Hmm i will try that. Any suggestions on how to properly include the axis line? Not sure if i have done something wrong, but i cant seem to mesh the geometry with the single line (axis) as shown in the first image I posted.


      Thank you very much for the quick respond. 

    • maggakahn
      Subscriber

      Is there a way for a wall to be defined as both a moving wall and a axis? If I create a square as in the picture and then define the lower line of the square as both a moving wall and a axis, i think that would work.


       


      Thank you!

    • Rob
      Ansys Employee

      Axis is defined (hard coded) as y=0.  The axis bc is there in case you model a cylinder and need something defined at the centreline. In your case you'll have walls at y=R1 and y=R2. 

    • Rob
      Ansys Employee

      For rotation, once 2d axi-swirl is set you should be able to give the wall an angular velocity. 

    • maggakahn
      Subscriber

      Yes indeed. When i turn on 2D axi-swirl i can indeed set a rotating angular velocity for the wall. In addition, I moved the axis to y=0, which helped Thank you!


      However, I have problems with stability and i think perhaps my mesh / geometry or the way I have created the geometry is sub optimal.


      The image above is the geometry i have created with SpaceClaim. Where i have detatched the two surfaces and called the bottom square "solid" (which is essentially just included to create the "axis" boundary condition for the lowest line of the square" ) and top square "fluid". This creates quite a few different bounderies when imported to Fluent.


       


      Do you have some tips on how to properly define these surfaces?


       


      Thank you very much for the help! Much appreciated


       

    • Rob
      Ansys Employee

      Just remove the lower square: it's not needed unless you want to include heat transfer.  As for the labels: read up on Named Selections in Workbench (Ansys) Meshing.

    • maggakahn
      Subscriber

      Okey. But how do i then include the axis of rotation? I tried to draw a line at y=0 and named (named selection) it as "axis" at one radii apart from the inner cylinder, but the mesher did not seem to like that and simply removed it. Is there a better way of defined this axis without needing to draw it?


      Thanks for the quick reply. 

    • Rob
      Ansys Employee

      You don't need to worry about it : the axis is y=0 that's hard coded into the solver. Just mesh the fluid part at R1 distance from the y=0 and try it. 

Viewing 9 reply threads
  • You must be logged in to reply to this topic.