March 8, 2018 at 6:59 amVenkatesh ArivazhaganSubscriber
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
March 8, 2018 at 2:40 pmRaef.KobeissiSubscriber
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.
March 8, 2018 at 3:20 pmVenkatesh ArivazhaganSubscriber
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.
March 11, 2018 at 10:53 pmRaef.KobeissiSubscriber
did You try to use pressure outlet with a specific pressure?
March 12, 2018 at 11:38 amVishal GanoreAnsys Employee
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.
March 12, 2018 at 12:54 pmVenkatesh ArivazhaganSubscriber
Thak you so much Vishal ganore
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- The solver failed with a non-zero exit code of : 2
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2022 Copyright ANSYS, Inc. All rights reserved.