CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Highly negative pressure value for outlet with specified pressure (https://www.cfd-online.com/Forums/cfx/134267-highly-negative-pressure-value-outlet-specified-pressure.html)

CFD-fellow April 26, 2014 16:49

Highly negative pressure value for outlet with specified pressure
 
Hi
Im modeling a free surface flow( air over water ).
>>>>>>>
Although Ive set the static pressure at outlet,after the third time step the cfx-post shows highly negative pressure for outlet (time step 1 and 2 was correct) but correct velocity as expected to be vise versa.:confused:

Any help would be appreciated

ghorrocks April 27, 2014 06:34

Your simulation is probably numerically unstable and is about the diverge. You need to improve numerical stability - do that by improving mesh quality, double precision, better initial conditions or other means.

CFD-fellow April 27, 2014 09:31

Thanks Glenn
My results are completely wrong but my residuals have a logical behavior (I mean its not near divergency).
According to my experience with Fluent, i think the solver doesnt have the right to change the specified variable in boundary condition under any condition (even divergency) and any step of the solution.
Is it possible that CFX-SOLVER has this right, to improve convergency or prevent divergency in early iterations? Or maybe i havent enough study on CFX boundary conditions.
Regards

ghorrocks April 27, 2014 18:32

What have you set the boundary as? An outlet or opening? And which option of outlet or opening?

CFD-fellow April 28, 2014 05:17

2 Attachment(s)
I use outlet with static pressure. Can opening boundary solve my problem?
I have attached the pressure contour for first and 10th time steps.My reference pressure is 1atm.

ghorrocks April 28, 2014 07:01

The pressure spots are spurious flows from the free surface model. These ae very common and hard to avoid. but careful choice of free surface model parameters and high mesh quality with tight convergence can reduce them.

But regarding your question on why the boundary is not fixed to the value you defined it to:

I think you will find the boundary face will be fixed to the value you defined. The values you are showing are the conservative values which represent the control volume inside the domain, and therefore are free to vary their value.


All times are GMT -4. The time now is 07:58.