CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Highly negative pressure value for outlet with specified pressure

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 26, 2014, 16:49
Post Highly negative pressure value for outlet with specified pressure
  #1
Member
 
Behrooz Jamshidi
Join Date: Apr 2013
Posts: 75
Rep Power: 4
CFD-fellow is on a distinguished road
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.

Any help would be appreciated
CFD-fellow is offline   Reply With Quote

Old   April 27, 2014, 06:34
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   April 27, 2014, 09:31
Default
  #3
Member
 
Behrooz Jamshidi
Join Date: Apr 2013
Posts: 75
Rep Power: 4
CFD-fellow is on a distinguished road
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
CFD-fellow is offline   Reply With Quote

Old   April 27, 2014, 18:32
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What have you set the boundary as? An outlet or opening? And which option of outlet or opening?
ghorrocks is offline   Reply With Quote

Old   April 28, 2014, 05:17
Post
  #5
Member
 
Behrooz Jamshidi
Join Date: Apr 2013
Posts: 75
Rep Power: 4
CFD-fellow is on a distinguished road
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.
Attached Images
File Type: png 1_full.png (24.8 KB, 3 views)
File Type: png 10_full.png (22.8 KB, 3 views)
CFD-fellow is offline   Reply With Quote

Old   April 28, 2014, 07:01
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,937
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
static vs. total pressure auf dem feld FLUENT 14 February 3, 2015 06:08
sonicFoam - pressure driven pipe: flow continuity violation and waveTransmissive BC Endel OpenFOAM Running, Solving & CFD 3 September 11, 2014 16:29
negative pressure in cfx flar.t CFX 1 December 19, 2006 00:20
negative pressure mAx FLUENT 0 January 25, 2006 15:31
Negative Pressure S Christopher CFX 2 October 6, 2005 18:14


All times are GMT -4. The time now is 11:24.