Fluids

Fluids

Different behavior of boundary conditions with dynamic mesh in Fluent

    • jfonken
      Subscriber

      Hi all,

      I experience a problem with my pressure-outlet boundary conditions when executing FSI with Ansys Fluent and Ansys Mechanical APDL. I'm modeling an abdominal aortic aneurysm including the aorto-illiac bifurcation. At both outlets (called LCI and RCI), I'm applying a pressure-outlet boundary condition. After each time step, the boundary pressure for the next time step is calculated using a Windkessel model and a 'define_execute_at_end' UDF. At each iteration, I'm using a 'define_profile' UDF to couple the calculated pressure to the right boundary. One pressure is calculated for the entire outlet (since the pressure is based on the flow through the surface).

      When I use these UDFs and monitor the pressure in a Fluent-only (rigid mesh) model, the pressures behave as expected. The pressure for all iterations within one timestep is the same and corresponds to the results visualized in CFDpost (see figure below). The pressure is constant along the entire outlet, with only small differences at the borders.

    • DrAmine
      Ansys Employee
      A thought: Within a coupling iteration Mechanical and Fluent will exchange the information. Fluent will not only run say 5 iteration per time steps but 5 iterations for the time step per coupling iteration. DEFINE_PROFILE is executed may times at time step even before the time steps starts. I would rather use a DEFINE_ADJUST which gets executed every iteration and to check whether at the end of the time step the pressure prescribed corresponds to the pressure received and reported in Fluent. It might be possible too that one would require more iteration per time steps so that things stabilizes.
    • jfonken
      Subscriber
      Hi Amine Thanks for your suggestion! I started to use the DEFINE_ADJUST function to output the current pressure at each face at the LCI and RCI outlet boundaries, such that I could compare the current and prescribed pressures. I would expect that the current pressure corresponds to the prescribed pressure, since the DEFINE_PROFILE is executed before DEFINE_ADJUST. However, this is not the case for my model, as also seen in the figure in my first post.
      If I understand you correctly, you suggest that I use DEFINE_ADJUST to adjust the pressure at the boundary faces instead of using DEFINE_PROFILE?

    • JeroenFeher
      Ansys Employee
      Hi there. I'd like to chime in on this as well. The define profile is (almost always) required to prescribe your pressure. I think what was suggested by DrAmine is to define a variable which you update, either using your define_execute_at_end or your define_adjust. Then that variable is used in your define_profile. From what I understood, you are already doing this , but using a define_execute_at_end but it will allow you exact control on what's being prescribed.
      However, this brings me to point 2, namely the results from those figures. Let's start with the second figure. I can see you have backflow on 100% of your outlet surface in this case. What is the backflow specification you have there? The equations used for generic windkessel models provide you with a static pressure and prescribing total pressure during backflow is incorrect.
      You mentioned you have outlets which are free to move in radial direction. When your vessel expands or contracts, you will have fluid movement at the wall, in radial direction, but not necessarily at the center of your vessel. In fact if the vessel is perfectly symetrical there is no radial velocity at the exact center. So basically a pressure gradient should exist in radial direction or you would have no radial velocity and no movement of the wall. However, I'm not sure what magnitude that gradient should be.
    • DrAmine
      Ansys Employee
      Hello: yesis correct. Reversal flow might spoil the strategy. I did not say that the ADJUST will be used to setup the pressure at the boundary but to get the right pressure which should be then applied via the DEFINE_PROFILE.

      So back to the reversal flow: bear in mind that if back-flow occurs the pressure you are prescribing will be (in general) interpreted as stagnation pressure (total pressure).
    • jfonken
      Subscriber
      That worked Jeroen, thanks!!
Viewing 5 reply threads
  • You must be logged in to reply to this topic.