Solid-Gas Multiphase System ERROR: Turbulent viscosity limited to viscosity ratio of 1.000000e+05

SundraSundra Member

Hello,

I am simulating a multiphase system (gas-solid using Eulerian Granular, Model: Realizable k-e, Standard Wall Function) with a air inlet velocity of 13 m/s. I want to simulate it as a fluidized packed bed reactor (without inlet and outlet flow of plastic pellets) and with "Adapt" - "Patch" I fill the reactor with plastic pellets (see image).

I have a problem during the calculation. I get a floating point exception error (turbulent viscosity limited to viscosity ratio of 1.000000e+05). I refined my mesh looking at skewness and orthogonal quality and it was really fine. I looked at some other forums and it seems that the k-epsilon model is probably calculating erroneously or my solver/controls setup is not right for my simulation.

Is there anyone who could help me with this problem? If you need more information I will immediately share it with you.

Thanks,

Sundra

Comments

  • RobRob UKForum Coordinator
    edited July 20

    Viscosity ratio is a warning, but you may then see the solver fail because of whatever is triggering this. 

    How are you adding the particles? 

  • SundraSundra Member
    edited July 20

    It´s seems to be that the viscosity ratio exceeds in every cell (800k) + it shows "reversed flow pressure outlet ". 

    I am following this tutorial 1:1 and just change my parameters.

    Basically I am creating a secondary "fluid" (plastic with its density, I don´t change the viscosity), adjust the secondary phase with "Granular", add the diameter and use syamlal-obrien for granular viscosity. After initializing I use the function "Refine/Coarse" and mark the cells where the plastic pellets should be. Than I patch the marked cells with volume fraction of plastic pellets, change my interaction phase with drag coefficient syamlal-obrien-para and then I start to simulate. 

  • RobRob UKForum Coordinator
    edited July 20

    What volume fraction did you use? If you patched at the packing limit it'll do interesting things: try 0.01 less than the packing limit. 

  • SundraSundra Member
    edited July 20

    I used a volume fraction of 0.578 and void of 0.422. The packing limit is 0.63 

  • SundraSundra Member
    edited July 20

    This error will appear at a certain point.

  • SundraSundra Member
    edited July 20

    I also reduced the time step size to 0.001s (tried 1s, 0.1s, 0.01s) and at the end I will get the same error but way later

  • SundraSundra Member
    edited July 20

    I did some research and probably my dt was  to big. With 0.001s I had the best "results" yet but in my case I might need to reduce dt even more. The minimum cell size is 2x10-5m and the maximal cell size is 0.065m. So I am trying to simulate with the "Adaptive Time Stepping" method and I am getting a physical dt varying between 1x10-5s to 5x10-5s (inlet velocity of air is 12.6m/s). At the end I will have a solution with a flow time of maybe 1s if I iterate 20 000 times... Not good not terrible

  • SundraSundra Member
    edited July 20

    I tried to make my cells bigger so that I can increase my dt without changing the inlet velocity (which should stay constant). The smallest cells I get are from the inflation layers at the walls of the vessel and pipe (approximately 0.004m). With these cell sizes I can "increase" my dt to 0.0003s which is anyway really small. 

  • RobRob UKForum Coordinator
    edited July 21

    Welcome to CFD multiphase. You've already started down one of the better paths. Depending on the size of the domain, how critical do you think the near wall flow is? 

  • SundraSundra Member
    edited July 21

    The whole vessel has a height of 10m and a diameter of 2.3m. The pipe has a diameter of 0.4m. The most critical parts is the air coming out of the pipe and colliding to the conical diffusor plates. My goal is to see how big does the pellets influence the velocity of the air close to the diffusor and lower vessel (4m height). I have done a lot of simulations without the pellets before just to see how the air behaves inside the vessel. My next step is to compare the 1phase and 2phase system without inflation layers. 

  • RobRob UKForum Coordinator
    edited July 22

    If you remove the inflation how does it look?  Very simply the finer the mesh the smaller the timestep and the more accurate the solution. Coarsening the mesh will speed things up, but reduce accuracy. You need to decide which you want. 

  • SundraSundra Member
    edited July 22

    Without inflation layer I got to the end of my simulation without any mayor troubles, just some cells where the turbulent ratio limit exceeded. I used a dt of 0.001s.

    That´s the question... I might need to try both (coarse/fine) and see how big the differences are. Do you have any tips for multiphase in general? What are the most critical parameters/controls/methods as a rule of thumb?

    Thanks for helping me out

  • RobRob UKForum Coordinator
    edited July 23

    I need to be careful here as giving detailed advice or using "my engineering knowledge" to any extent is beyond what we're allowed to cover on here.

    For multiphase you need to work out roughly what will happen (ie understand what you're modelling) before you start. You then choose the model(s) to do this before going away and getting the geometry & creating the mesh. The planning stage is also used to work out expected speeds, residence times etc to help with cell size and accuracy 

Sign In or Register to comment.