CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   asking about the dynamic pressure (http://www.cfd-online.com/Forums/main/112153-asking-about-dynamic-pressure.html)

yuhehuan January 23, 2013 01:07

asking about the dynamic pressure
 
Hi everyone. I simulated the pressure and velocity in an airflow 3-d area. I calculated the dynamic pressure at three outlets based on the equation :Pd=0.5*rho*v2. But the calculated results are different with the simulated results (dynamic pressure at the three outlets). I am not sure if my velocty simulated is wrong. I am appreciated with all your help! Many thanks!

yuhehuan January 23, 2013 13:56

Does anybody know? Thank you so so much!

cdegroot January 23, 2013 23:03

Your question is way too general to answer.

yuhehuan January 24, 2013 02:05

Quote:

Originally Posted by cdegroot (Post 403674)
Your question is way too general to answer.

what's your meaning?

cdegroot January 24, 2013 08:27

You haven't described what you are simulating or how you have set it up. Without more information it isn't possible to answer your question.

yuhehuan January 24, 2013 12:43

I simulated the airflow in a 3 dimensional space, there is one inlet at the bottom and three outlets at the side . I take velocity-inlet and outflow as the boundary conditions. There is reversed flow but it is still converged. I calculated the dynamic pressure at the outlets based on the eqution and compared the results with the simulated results from the report. It is not equal. I am so confused about that. Does anybody has the same problem?

cdegroot January 24, 2013 12:50

You haven't mentioned what software you are using. Is it Fluent? The backflow could be a problem. If it is turbulent, what are your backflow conditions? Do you expect that there would be backflow in the physical situation? How do you know it is converged? Did you check monitor points or just the residual? Since you are interested in dynamic pressures this would be an appropriate monitor. Have you checked grid independence?

yuhehuan January 24, 2013 13:15

Quote:

Originally Posted by cdegroot (Post 403829)
You haven't mentioned what software you are using. Is it Fluent? The backflow could be a problem. If it is turbulent, what are your backflow conditions? Do you expect that there would be backflow in the physical situation? How do you know it is converged? Did you check monitor points or just the residual? Since you are interested in dynamic pressures this would be an appropriate monitor. Have you checked grid independence?

Hi, thank you so much for your reply. It is turbulent. I guess the reason of backflow is that the distance between the inlet and outlets is very close. I used fluent. The residual solution is converged as the iteration finished. Sorry I don't understand the grid independence. The maximum aspect ratio is 9 and the maximum cell skewness is 0.58.

cdegroot January 24, 2013 14:00

The residual is not enough to declare convergence, especially if you are using the default convergence criteria in Fluent. Try dropping the convergence criteria by and order of magnitude and see if the solution changes. Keep dropping it if the solution changes.

Grid independence means to run the calculation on successively finer grids (recommend doubling total number of volumes each time) to make sure you are running a fine enough grid.

If the backflow persists you might need to modify your outlets. How you would do this depends on the physical situation you are modelling.

yuhehuan January 24, 2013 14:35

So you mean the reversed flow is not allowed to exist even if it is converged?

cdegroot January 24, 2013 14:46

It is possible to have reversed flow in a converged solution, but more often than not it is a sign of trouble. Plus if your backflow conditions are not reasonable there will be an impact on your solution. It could be that your outlet is not properly modelled. You'll have to think about the physics of the actual problem to figure this out. I think you probably actually want a pressure outlet not an outflow boundary since the outflow boundary condition assumes the flow is fully developed. Read the section of the User Guide "Using Outflow Boundaries". I think you will find it is not appropriate for your situation.

yuhehuan January 24, 2013 15:42

Because I don't know the pressure at the outlets and need to simulate using fluent, so i have to choose outflow as the boundary condition. It's impressible flow. Thank you so much for your explanation. I appreciate your help!

cdegroot January 24, 2013 15:50

Fair enough. Just make sure your outlets are located such that the outflow boundary condition is well-posed as describe in the User Guide. Maybe you need to simulate some of the space surrounding the box as well.


All times are GMT -4. The time now is 03:44.