General Mechanical

General Mechanical

Use an output as input for the next timestep

    • dario.guarino
      Subscriber

      Hello,

      I am solving a transient thermal problem.

      I would like to use the calculated temperature of certain node o surface, at a timestep N, as input for the step N+1. I want to compare the temperature at timestep N with a certain reference temperature at timestep N+1.

      In function of the outcome ( T(N) bigger or smaller wrt the reference) I want to use a certain coefficient at timestep N+1 instead of another.

      Is it possible to do such a thing? maybe via APDL or python script?

      Thank you

      Regards

    • Sheldon Imaoka
      Ansys Employee

      Sorry that I don't quite understand your question, but are you trying to define temperature-dependent film coefficients? If so, this can be directly done via the "Convection" object.
      If this is not the case, can you clarify what is meant by "certain coefficient at timestep N+1"? What coefficient are you referencing?
      Generally speaking, you can have temperature-dependent material properties or temperature-dependent thermal loads and boundary conditions. Ansys Mechanical does not evaluate the temperature-dependency based on the previous timestep - instead, Newton-Raphson method is used to iterate to ensure that the temperature-dependency is evaluated at the current temperature. This is more accurate than using the previous temperature for the current timestep (if you evaluated based on temperature of previous timestep, then accuracy would be dependent on timestep size).
      Regards Sheldon

    • dario.guarino
      Subscriber

      Thank you for your answer. Indeed my message was not really clear, I will try to reformulate.
      With a transient thermal I am simulating a steam flow that invests a surface. The surface is initially cold.
      I have prepared an excel file, that I use as input to define the convection coefficient and the ambient temperature, that change over time. Those values have been pre-defined via a script external to Ansys and condensation is not taken into account. Now I would like to improve my model by considering the condensation phenomenon.
      Initially I expect condensation, since my surface is going to be colder than the saturation temperature. As the time passes, my surface will warm and become hotter than the saturation temperature. At this point there will not be condensation anymore.
      I would like to do that by checking each step the temperature of my surface and compare it to the saturation temperature, that needs to be calculated each step.
      I am trying to find out how this can be done. The temperature of my surface at step N, should be used at timestep N+1 to be compared with the saturation temperature (calculated at timestep N+1).
      In function of the outcome of the check, a certain convection coefficient will be used. (coefficient X if T < Tsat and coefficient Y if T >Tsat).
      I hope it is a bit more clear
      Thank you again!
      Kind regards

    • Sheldon Imaoka
      Ansys Employee

      Thanks for your clarification.
      If only your bulk temperature is a function of time, in the Details view of your "Convection" object, you can change "Edit Data for: Ambient Temperature" and specify it to be a function of time. Then, you can switch "Edit Data for: Film Coefficient" and set it as a function of temperature. The "Coefficient Type: Surface Temperature" allows you to define that the temperature-dependency is based on the surface temperature. A perfect step function cannot be used since you need unique values for a given surface temperature, but you can then define film coefficient changing before and after Tsat.
      If both your bulk temperature and film coefficient change as a function of time, then you will need to define the Convection loading via a "Commands (APDL)" object since film coefficient would be a function of both time and surface temperature. Section 3.5.16. "Applying Loads Using Tabular Input" and the Thermal Analysis Guide of the Mechanical APDL help documentation could be a starting point to understand how to define such loads in APDL.
      Regards Sheldon


Viewing 3 reply threads
  • You must be logged in to reply to this topic.