Fluids

Fluids

what is the appropriate settings for the following cfd simulation?

    • neal312000
      Subscriber

      I am trying to simulate the cooling of a hot end of a 3d printer by the cooling fan. My mesh is good and every cell is below 0.85 in skewness. I am using sst k-w model with energy equation on.

      In cell zone conditions, I am using mesh motion for fan case and and I ticked the specified operating density in the variable density parameter in operating conditions.

      For boundary conditions, I have no inlets or outlets. Everything is wall. I have given heat flux to heater and convection boundary condition to the domain.(picture for reference below)

      My other settings solution methods and under relaxation factors are default.

      I use hybrid initialization and for calculations, time step=0.004s, no. of time step=250 and no. of iterations/time step= 20.

      I am getting warnings such as "turbulence viscosity ratio limited to 1.0e+05 in xx cells" and "divergence detected in amd solver: temperature" and "floating point exception" after about 260 iterations. After this warning the fluent closes on its own.

      I think I have to further reduce the time step and increase the no. of iterations/step from what I have read online.

      Please help with this. I attached pictures for reference

    • Kalyan Goparaju
      Ansys Employee
      Hello, nA couple of things that may helpnStart with a steady calculation and then switch over to a transient run. This should make the transient run more stable. nAny reason for having all the domain boundaries as walls? Is it a physical representation of your actual model? More often than not, when you have a fan cooling a heat source, the fan should be able to draw in air continuously from the surrounding. If you set all the domain faces to wall, you are in fact restricting this. nIf none of the above work, do try a smaller timestep to start the simulation off, and ramp it up later. nThanks,nKalyann
    • neal312000
      Subscriber
      I don't have outlets or inlets as it represents my physical model. Also if i keep any of the faces of my domain as outlet than I am getting a reversed flow as the fan has a small capacity of pushing air out.nFurther, I want to ask few questions.n1) What should be the origin of rotation in mesh motion and is it calculated from the origin of global coordinate system?n2) Is the error of turbulent viscosity ratio limited to 1e+05 in xx cells due to my geometry of fan case? If yes, how to resolve it?.Thank you, Neal
    • Rob
      Ansys Employee
      The origin of rotation is the centre point and then axis of the centre of the fan. For convenience most people try and put the fan on one of x, y or z axis. Rotation then follows the right hand rule. nViscosity ratio may mean you have a problem, or may mean your initial conditions are a bit too turbulent for the actual conditions. I wouldn't expect the fan to be in a sealed container though so review this. If it is sealed what is the fluid density? n
    • neal312000
      Subscriber
      I took your suggestion rob and gave an velocity inlet with zero velocity on one end of the domain and pressure outlet on the other end.nIn cell zone conditions , for mesh motion , I gave rotation direction as z=-1 but the fan is still rotating in positive direction. how can I rotate it towards the negative z direction?nI have attached images for reference.nThank you,nNealnn
    • Rob
      Ansys Employee
      Setting zero velocity isn't a good idea, zero pressure is OK, but zero velocity isn't. If the fan is spinning in the wrong direction you could use a negative angular velocity..... n
    • neal312000
      Subscriber
      The error of turbulent viscosity ratio limited to 1e+05 in xx cells was solved if I used second order implicit in transient formulation in solution methods and I made small rectangular vents at the ends of my fluid domain and gave them pressure outlets in boundary condition with zero gauge pressure. This appeared to solve my problem.nI do have one final question. The heater in my model is supposed to get heated to 250 degree Celsius. In my real physical model, it is done via a heater cartridge and it takes at least 60 seconds to heat it to 250 degree Celsius. I can only do a transient simulation of 1 second as my pc doesn't have high computing power. nSo what can be appropriate boundary condition for heater so, I can get it 250 degree Celsius in my simulation? Heater is made up of aluminum.nI have attached pictures for reference.nThank you,nNealnn
Viewing 6 reply threads
  • You must be logged in to reply to this topic.