Reversed flow problem

 Hello everyone,

  During 2D external flow analysis of car cavity in ansys fluent, the warning which i'm getting was  "reversed flow in 1 face of outflow 6" because of this warning, the solution is not at all converging. The mesh quality was also good and the extension of  outflow location will also be quite impossible. I have also kept the flow rate weighting as 1.

If somebody have a solution for this problem, please do reply

The files have been attached for the references

 

Comments

  • Raef.KobeissiRaef.Kobeissi United KingdomMember
    edited March 2018

    Reverse flow usually occurs when the outlet is not far enough from the car body and/or inlet. Make your fluid domain longer and away from the rear end of the car and it should work perfectly fine.

    Regards

  • Venkatesh ArivazhaganVenkatesh Arivazhagan IndiaMember
    edited March 2018

    Yeah i agree with you, but as per the problem statement which i'm having, i'm not allowed to increase the fluid domain. Is there any other chance to avoid this reversed flow problem.

      

  • Raef.KobeissiRaef.Kobeissi United KingdomMember
    edited March 2018

    did You try to use pressure outlet with a specific pressure?

  • vganorevganore Pune, IndiaAdmin
    edited March 2018

    I have couple of suggestions:

    1. You are using laminar model. Investigate your Reynolds number to understand what kind of flow it is. Naturally your flow should be turbulent (velocity of 28 m/s) so use turbulent model (I could get started with k-e).

    2. With above in mind, I could converge your solution below 1e-3 by initialising from inlet instead of hybrid initialisation and running it for 700 iterations. Flow reversal is not a problem here. Flow direction can change due to flow separation and recalculation effects.

     

    3. Focus on the value of Y+ plus your mesh is carrying. After performing certain iterations, Fluent could estimate Y+ value over a car body. Currently it is 5600, you need to bring it down between 30-300 by refining your mesh near the wall if possible. (ANSYS Student version may not able to produce such a fine mesh but research version can.)

    4. BCs: if this is a simple flow over a car just for an illustration purpose then its ok to have this demo model. In this case, your results (cd & Cl) will be highly sensitive to wind tunnel wall effects, as walls are placed very close to the car. To avoid this, you should allow sufficient space around the car so that computed flow variables should not be wall sensitive. Here is the tutorial that shows how to do this.

    http://user.engineering.uiowa.edu/~me_160/2017/CFD Labs/Lab4/Intermediate Lab 4 Manual.pdf

     

     

  • Venkatesh ArivazhaganVenkatesh Arivazhagan IndiaMember
    edited March 2018

    Thak you so much Vishal ganore 

Sign In or Register to comment.