Fluids

Fluids

Monitored values are stablized. But flow patterns are immature.How to fix flow patterns?

    • Sardar
      Subscriber

      Hi all.

      My simulation involves an agitator tank with two impellers.

      I am using steady, coupled psuedo transient with timescale factor of 1 to solve.

      Monitoring only the moments on impellers and volume average velocity throughout the tank suggests that the solution is "converged", because they are well stablized at sound values.

      But FLOW PATTERNS are nowhere near acceptable, they are not full fledged at all and my RESIDUALS are still high in the e-2 (continuity), e-3 levels(Albeit they are decreasing).

      What should I do to get flow patterns as expected? Letting everything continue as it goes does not look promising, primarily because flow patterns are way too slow to develop and coupled solver is too expensive. Should I resort to playing with URF and time scale factor of the pseudo solver (respectively default and 1)? If so, what exactly should I be lowering or increasing?

    • Rob
      Ansys Employee
      How long has the model been running? For a real problem it'll not converge in 20-150 iterations and with a timescale factor of 1 it'll be quite stiff. Dropping the time scale factor to around 0.1-0.5 tends to help with more complex flows, as will a good initial condition, mesh and physically appropriate bc's & material properties.
    • Sardar
      Subscriber
      The model has been running for 270 iterations (almost a whole day!) and flow patters are showing up, but still at quite low pace. Time scale factor of 0.5 has just started to help with flow patterns though.
    • Rob
      Ansys Employee
      270 iterations isn't very long. If it's struggling after 1500-5000 iterations then it's more of an issue. How many cells have you got, and how much RAM?
    • Sardar
      Subscriber
      I have 3.1 million cells (tank specs mentioned in my post here.)meshed via fluent meshing (surface mesh: min 0.0025 [m], Max 0.07 ||| volume mesh: min: 0.0025 max:0.04). I am running it with 8 GB RAM, and 8 cores (core-i 7).
      1500-5000 iterations means almost a week I guess, although a 68-m3 tank isn't a very common case as far as I have seen in videos.
      Do you think plugging close-to-reality values for turbulence in the standard initialization can help with simulation accuracy? (I don't remember where exactly I started thinking that standard is less accurate.)

    • Rob
      Ansys Employee
      Check the RAM usage on the PC. How many cores are you running on, and how many physical cores has the PC got?
    • Sardar
      Subscriber
      7.85 out of 8 GB RAM keeps touching the roof during the entire run I think. There are 8 physical cores and I am running on all of them.
    • Rob
      Ansys Employee
      I suspect you're paging to disc, or are very close to it. If you're using the Pressure Based Coupled Solver drop to SIMPLE. In theory it's slower, but as RAM may be causing the bottleneck it may improve the performance. Also turn off everything you can, eg no browsing the web!
    • DrAmine
      Ansys Employee
      Use a larger machine or reduce mesh count and adopt another Meshing strategy.
    • Sardar
      Subscriber
      Actually the replies given by Rob and DrAmine were spot on. I was using too fine a mesh leading to high computation expense and even worse divergence!! I believed mesh-induced divergence could be something quite rare!
      Now I have reduced my cell count to 600K and changed the mesh method to multizone. To say the least, the calculation pace is much much higher now. What would take a week is solved in 8 hours now, although there are still other adjustments I need to do. I will be back to add more info.
    • DrAmine
      Ansys Employee
      Great!
Viewing 10 reply threads
  • You must be logged in to reply to this topic.