Fluids

Fluids

Topics related to Fluent, CFX, Turbogrid and more.

Boundary Condition Issue

    • Housermanj
      Subscriber

      I am attempting to simulate the flow of resin through a rectangular porous domain using Ansys Fluent. The flow is driven by a pressure difference, with atmospheric pressure at the inlet and a very low pressure at the outlet. Initially, the velocity throughout the domain is zero. The inlet pressure is set to 101,325 Pa (atmospheric pressure), while the outlet pressure is set to 2 Pa. This pressure gradient initiates the flow through the porous medium.

       

      However, when I specify pressure inlet and pressure outlet boundary conditions, Fluent crashes. I have tried various pressure initializations within the domain, including:

      1. Atmospheric pressure,
      2. Exit pressure (2 Pa),
      3. A linear variation from the inlet to the outlet.

      Unfortunately, none of these approaches worked.

       

      Interestingly, when I specify a velocity inlet condition (with the inlet velocity calculated based on Darcy's law), the simulation runs successfully. However, the inlet velocity is not constant in reality, as it should vary based on the pressure gradient. Therefore, I would prefer to model the flow using specified inlet and outlet pressures rather than a constant velocity.

       

      The mesh employed is a Cartesian mesh. Any advice or pointers on how to properly model flows with specified inlet and outlet pressures in Fluent would be greatly appreciated.

       

       

       

       

    • Rob
      Forum Moderator

      What operating pressure did you set? Is this single phase?  

      Note, models with pressure inlet and outlet can be sensitive to the initial condition as mass flow is part of the solution. If you also have porous media the calculation can become more complicated as velocity and pressure become very tightly coupled. 

      • Housermanj
        Subscriber

        The operating pressure is set to zero. It is mutliphase (VoF) with 2 phases. 

    • Rob
      Forum Moderator

      And the gas density is? What time step are you using?

      • Housermanj
        Subscriber

        The density for both fluids are set to constant values. The time step is .05 secs.

    • Rob
      Forum Moderator

      So you have a 1 bar pressure drop over the domain, VOF and fixed density. If you use a very simple dP=0.5 rho v^2  how fast is the liquid going to try and move? How does that relate to the time it'll take to cross one cell (ie a residence time)?  What is the resin viscosity?

      • Housermanj
        Subscriber

        Based on the Darcy’s equation, the velocity magnitude comes up to 8.0E-05 m/s.  The cells are perfect squares in the flow direction, with side 5.0E-3 m.  So, the residence time is approximately 62 seconds.

        viscosity is 0.1 Pa.s 

    • Rob
      Forum Moderator

      Try patching a layer or two of cells at the inlet with the resin. With a viscosity that high you're potentially seeing a result of the gas density (to find the velocity) and not the liquid. 

Viewing 4 reply threads
  • You must be logged in to reply to this topic.