skin frition and separation flow

  • 34 Views
  • Last Post 13 November 2018
  • Topic Is Solved
abd fs posted this 13 November 2018

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 ?

Order By: Standard | Newest | Votes
abenhadj posted this 13 November 2018

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. 

Best regards,

Amine

abd fs posted this 13 November 2018

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

Best regards,

SERARE

seeta gunti posted this 13 November 2018

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.

abenhadj posted this 13 November 2018

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

Best regards,

Amine

abd fs posted this 13 November 2018

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 posted this 13 November 2018

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

abenhadj posted this 13 November 2018

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?

Best regards,

Amine

abenhadj posted this 13 November 2018

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. 

 

Best regards,

Amine

abd fs posted this 13 November 2018

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

abenhadj posted this 13 November 2018

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!

 

 

Best regards,

Amine

abd fs posted this 13 November 2018

Thank you so mush Sir AMINE 

I will try this and post here the results

Best regards,

SERRARE

Kremella posted this 13 November 2018

Hello,

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

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

https://studentcommunity.ansys.com/thread/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 posted this 13 November 2018

 Thank you so much  Sir Kremella

Close