Fluids

Fluids

Topics relate to Fluent, CFX, Turbogrid and more

outlet type in boundary conditions

    • peppers
      Subscriber

      I want to know what the temperature is at the outlet when the air at the inlet is 270K convected so that the temperature will rise when it comes out at the outlet, the data I have is the air velocity. so i use velocity-inlet in the inlet. what type should i use in the outlet to know the temperature there? (the velocity at the inlet and outlet is the same, according to the law of continuity)

    • SRP
      Ansys Employee

      Hi,

      You can use the "Outlet" boundary condition in ANSYS Fluent. For more details please refer to fluent user's guide: 7.4. Boundary Conditions (ansys.com)

      By setting up the outlet boundary condition, ANSYS Fluent will calculate the flow properties at the outlet based on the specified static temperature, and you will be able to obtain the temperature distribution and other flow properties at the outlet during the simulation or in the post-processing stage.

      Thank you.

      • peppers
        Subscriber

        is there another name for the 'outlet' type in outlet? because i didn't find it in ansys student 2023

        • Rob
          Forum Moderator

          Pressure outlet. 

        • peppers
          Subscriber

          However, when using the "pressure-outlet" boundary condition, you need to input data such as pressure and back flow temperature. In my case, I only have velocity data, and I am trying to find the temperature at the outlet. If I input a value for the back flow temperature, let's say 300K, the outlet temperature becomes 300K. Is there a solution for this?

        • NickFL
          Subscriber

          What velocity data do you have? The CFD software will compute a velocity distribution across the outlet face. Do you have such a distribution or an "average" velocity? Typically, we like to use a velocity condition at the inlet or outlet and a pressure condition at other. Mathematically, this works best.

          As you said, the temperature that is specified at the outlet is a backflow temperature. But this means that the value will only be used IF the flow is re-entering the domain at this point. If all the flow is leaving the domain at the outlet (typically what we want) then the backflow temperature is not used. The computed outlet temperature would come from the convected fluid upstream. If you specify the backflow temperature of 300K, this does NOT mean the solution must have a temperature of 300K at the exit.

        • peppers
          Subscriber

          the data that I have is the average air velocity data from the blower as forced convection.

          How do I prevent the back flow temperature from being used so that I can find out the temperature at the outlet every certain time (transient) using the pressure-outlet? because I entered the velocity-inlet and pressure-outlet with a back flow temperature of 300K and the result is a temperature at the outlet of 300K (meaning the back flow temperature is active).

          btw does this also apply to the boundary condition outflow type? because I also tried using velocity-inlet and outflow and the result is that the temperature at the outlet follows the temperature that I input in the velocity-inlet

           

        • NickFL
          Subscriber

          How do I prevent the back flow temperature from being used so that I can find out the temperature at the outlet every certain time (transient) using the pressure-outlet? because I entered the velocity-inlet and pressure-outlet with a back flow temperature of 300K and the result is a temperature at the outlet of 300K (meaning the back flow temperature is active).

          Does it report a “Reversed Flow on ### of faces (X% area) of pressure-outlet” when solving? This is telling you how much of the outlet has flow returning to the domain. These numbers should be small or ideally not even reported because they are zero. One way to remove them is to extend your domain so that all the flow is leaving an not entering where you have an exit. 

          btw does this also apply to the boundary condition outflow type? because I also tried using velocity-inlet and outflow and the result is that the temperature at the outlet follows the temperature that I input in the velocity-inlet

          Generally it is a good practice to avoid the outlfow type boundary condition in Fluent. Read the link SRP provided above.

          I should mention that my statement above about have the pressure/velocity conditions at the outlet/inlet is for subsonic flow. The mathematics of compressible flow require the conditions upstream.

Viewing 1 reply thread
  • The topic ‘outlet type in boundary conditions’ is closed to new replies.