Fluids

Fluids

skin frition and separation flow

    • abd fs
      Subscriber

      Dear  all,


       I have been modeling turbulent flow around a ramp 25°  with a model model k-omeaga SST. I got y+<1 ,The Xr indicates the reattach length and for this case we get a Xr/h value equal Xr/h = 6.5. According with the experimental data the mean value of rettach length is Xr/h = 6,2and my velocity profile is:




      how can I lose the value of Xr to get 6.2 ?

    • DrAmine
      Ansys Employee

      Firs of all 6.5 to 6.2 is not really bad (less than 5%). Think about using some other turbulence model (what are you using here) and mesh sensitivity study and summarize the work. 100% concordance is almost not feasible. 

    • abd fs
      Subscriber

      sorry Sir Amine but I got 7.5  not 6.5 just typo.


      Best regards,


      SERARE

    • seeta gunti
      Ansys Employee

      Try with realizable k-e with enhanced wall treatment. You may get much closer result. RKE model is more suitable for shear flows involving rapid strain, moderate swirl, boundary layer separation and vortex shedding behind the bluff bodies etc. 


       


       


      Regards,


      Seeta.

    • DrAmine
      Ansys Employee

      Inflow quantities are very crucial here: Please check what has been set in the experiments!

    • abd fs
      Subscriber

      Thank you  seeta gunti,


       I have to use k-w SST to validate the results obtained with the same model and the same conditions


      Best regrads,


      SERRARE

    • abd fs
      Subscriber

      Dear all,


      in case I inject a velocity at the entrance Uref = 15m / s, I obtained an aerodynamic coefficient but the velocity profile at an abscise reference x = -8,9h is not correct in the opposite case if I inject a thoroughly developed turbulent velocity profile extracted from a tube I got a large recirculation zone with an Xr = 7.5h and the velocity profile at the reference point and just



      Someone can help me? With some tips, comments?


      Best regrads,


      SERRARE

    • DrAmine
      Ansys Employee

      Please be more precise and provide some information about the paper and experiments. You need to match the conditions in the experiments. 


      How did you generate the profiles? What are using in the running case only velocity or other properties?

    • DrAmine
      Ansys Employee

      1/Please generate fully developed profile by assuming periodicity for your tube.


      2/Actually almost all turbulence models obeying a simple formalism like the Boussinessq approach will predict good results whenever the flow is fully developed. Enhancement can be done through some advanced models or by changing the formalism.


      3/Form the experiment it is said 15 m/s but perhaps they are talking about the bulk and not providing any information about the inflow regions (disturbances, fluctuations). As someone who has done some experiments, I have seen runs done without flow straightener...without mentioning that in papers and books.


      4/SST model is fine. Same applies for Realizable with EWT or Menter et. al.


      5/Summarize all work and write your report: All results are good to be reported if they are well documented. 


       

    • abd fs
      Subscriber

      Dear AMINE thank you so much but how can generate fully developed profile by assuming periodicity for my tube?.


      I extracted the velocity profile from the tube :



      Best regards,


      SERARE

    • DrAmine
      Ansys Employee

      1/Read tube case


      2/if your inlet and outlet are matching then go in the console and type mesh/modify-zones/make-periodic text command give the ids of inlet and outlet and say no. Now in GUI under periodic conditions provide the mass flow rate.


      2/Change inlet and outlet to interface and crate mesh interface + periodic in the case you do not have conformal matching boundaries.


       


      Check 5.9.4. Creating Conformal Periodic Zones in User's guide and have fun!


       


       

    • abd fs
      Subscriber

      Thank you so mush Sir AMINE 


      I will try this and post here the results


      Best regards,


      SERRARE

    • Karthik R
      Administrator

      Hello,


      Here are some links which might help you understand Amine's suggestions better.


      https://forum.ansys.com/forums/topic/how-create-and-use-profile-txt-file-as-a-boundary-condition-in-fluent/?order=all#comment-4dd4894d-d983-4af6-af37-a95b0159630f


      https://forum.ansys.com/forums/topic/understanding-the-behavior-of-the-solution-results-by-fluent/?order=all#comment-48366633-3ecb-4988-a5a2-a94600ec630a


      These posts contain elaborate discussion on a problem similar to yours. I hope these help you understand the model better.


      Thank you.


      Best Regards,


      Karthik


       

    • abd fs
      Subscriber

       Thank you so much  Sir Kremella

Viewing 13 reply threads
  • You must be logged in to reply to this topic.