Fluids

Fluids

Topics relate to Fluent, CFX, Turbogrid and more

Transient pressure in ANSYS Post

    • Adriana Pinto
      Subscriber

      Hello, I am trying to do a transient plot of water pressure at a point as a function of time. But when I calculate the theoretical hydrostatic pressure on that same point it gives a huge difference. Can someone explain to me why?

    • Federico Alzamora Previtali
      Ansys Employee

      Hello, 

      can you provide more details as to what your model looks like and how are you calculating the theoretical values?

       

      • Adriana Pinto
        Subscriber

        Hello Federico, 

        Thank you for your attention. I am simulating a sloshing case, where I have the tank filled with water. I want to measure the damping so for that I need pressure charts. I am measuring that pressure on the basis of the tank.

        The hydrostatic pressure is calculated by the formula where you use the density and height of the liquid.

    • NickFL
      Bbp_participant
      Keep in mind that the pressure shown in Fluent/CFX does not have the hydrostatic component (meaning the depth of the water is not included in the pressure). If you want to visualize this, it would be best to create a CCF (if working in Fluent) to see how the depth of the water contributes to the pressure. Similar questions have been asked many times on here, so do a search of the forum.
      • Adriana Pinto
        Subscriber

        Hello Nick.

        Thank you so much for your attention and your response.

        What is the pressure given in ansys cfd-post? Is it static, or relative? I can't understand that. And how can I get a chart of the displacement of the free surface vs time at a point? What is a CCF?

        Thank you very much

        • NickFL
          Bbp_participant

          In Fluent post-processing, there are several pressures that are outputted that are often confuse young (and even experienced) users. There should be a sticky post on the top of the board that should explain it (ANSYS are you "listening"). There are some short notes below, but if you do a search in the forum there are better descriptions.

          Static Pressure - This is the pressure calculated by the solver. Keep in mind it is measured against to the operating pressure.

          Absolute Pressure - This is the combination of the static and the operating pressure.

          Total Pressure - This is the combination of the static and dynamic pressures.

          CCF? That is a very good question. I should have typed CFF (Custom Field Function), sorry. This allows you to create user variables. Using this you could create a variable MyPressure that is the combination of the Absolute Pressure + rho g * Z. Again if you search the forums there probably are examples.

          But above it sounds like do not have a fixed surface height. Then we have to measure Z against the water fluid interface. That leads to your good question of the free surface location, and that I would have to think about a bit. Are you using the VOF (Volume of Fluid) model?

        • Adriana Pinto
          Subscriber

          Thank you very much for your attention to my problem.

          Your answer was very detailed. However, when using post-processing it only appears the name pressure so I am a little confused on what pressure it is. 

          Yes, I am using VOF.

        • NickFL
          Bbp_participant

          It sounds like you are using CFD-Post for your post-processing. In that case, it is the static pressure in Fluent that is called pressure in CFX-Post.

          But based upon the problem that you have, you will likely want to start working with the post-processing tools directly in Fluent. Sending transient result files to Post just results in complications. Post-processing in Fluent has really improved in the last several years, so there is little need to go elsewhere.

        • Adriana Pinto
          Subscriber

          I followed your advice and I am using the tools in fluent. But the result is the same for the static pressure as in CFD Post. I will add that I am measuring the pressure as a function of time in a point and the pressure values can reach negative values. What can this mean?

        • NickFL
          Bbp_participant

          Because the static pressure is being measured against the operating pressure, a negative value means that it is simply less than this value. Example static pressure -10 kPa with operating pressure of 100 kPa, then the absolute pressure is 90 kPa.

          Again, this pressure does not include the hydrostatic component. For that, you will have to likely construct a new variable using either the CCF or a Named Expression. The best approach would be to incorporate the depth by using the VOF to determine how much liquid is "above" the bottom surface.

Viewing 2 reply threads
  • The topic ‘Transient pressure in ANSYS Post’ is closed to new replies.