CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Pressure outlet v.s Outlet

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 9, 2020, 15:34
Default Pressure outlet v.s Outlet
  #1
New Member
 
Guoxing
Join Date: Oct 2018
Posts: 7
Rep Power: 5
Guoxing Chen is on a distinguished road
Hi,

I am modeling the urban wind environment with Starccm+.
I am using SKE and Boussinesq Model.
If I used Pressure outlet boundary, it would have reverse flow and the residual might not reach 10-4. While switch to Outlet boundary, the reverse flow is gone and the convergence is really nice.
Is there any differences in the final results between boundary types of Pressure outlet and Outlet?

Best regards,
G

Last edited by Guoxing Chen; May 9, 2020 at 18:53. Reason: adding a word
Guoxing Chen is offline   Reply With Quote

Old   May 10, 2020, 06:33
Default
  #2
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 555
Rep Power: 17
ping is on a distinguished road
if there is positive flow out of a pressure bc then there will no difference in the results assuming the pressure value setting is not influencing the flow and thus that you have identical mass flows.
if you have reverse flow with the pressure bc then you have a poorly setup model and a common mistake newbies make is to position the outlet too close to some disturbance in the model eg a bend, and you should have typically 10x the diameter of straight duct etc downstream of such a feature - easy to add using the meshing extruder.
ping is offline   Reply With Quote

Old   May 10, 2020, 11:26
Default
  #3
New Member
 
Guoxing
Join Date: Oct 2018
Posts: 7
Rep Power: 5
Guoxing Chen is on a distinguished road
Quote:
Originally Posted by ping View Post
if there is positive flow out of a pressure bc then there will no difference in the results assuming the pressure value setting is not influencing the flow and thus that you have identical mass flows.
if you have reverse flow with the pressure bc then you have a poorly setup model and a common mistake newbies make is to position the outlet too close to some disturbance in the model eg a bend, and you should have typically 10x the diameter of straight duct etc downstream of such a feature - easy to add using the meshing extruder.
Hi Ping,

Thanks for the reply.
I guess it was not the problems of distance. In the recommendation document of CFD simulation of urban wind environment, the distance from building edge to the downstream should longer than 15H, where H is the building height.
For my setup, I extend the distance to 45H, and the problems still existed (reverse flow and the convergence).
Meanwhile, in the recommendation, the flow shall be fully developed at the outlet. Is it the bc type of OUTLET is used for fully developed flow?

Best regards,
G
Guoxing Chen is offline   Reply With Quote

Old   May 10, 2020, 21:39
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,448
Rep Power: 53
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
By Outlet boundary do you mean Outflow Boundary condition?

The pressure outlet BC fixes the pressure and sets the gradient of velocity to 0.

The outflow BC sets only the diffusive flux to zero. This constraint is a little weaker and allows stuff advect out.

The implications of the differences between these are really subtle.
LuckyTran is offline   Reply With Quote

Old   May 11, 2020, 03:19
Default
  #5
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 555
Rep Power: 17
ping is on a distinguished road
so this is what we call an external cfd case and so my mentioning a duct was for internal flow cfd. cases like this can be tricky for a few reasons one being the temperature and pressure gradient in the vertical direction so take a close look at velocity vectors on several vertical section planes across the domain and parallel to the wind direction and look for clues to the source of reverse flow.
and it is common for unsteady eddies etc to occur around buildings and this can cause residuals to plateau and so prevent steady state convergence. so look for these local effects and if they are small and repeatable then you can consider the case converged. otherwise you need to do some additional solving in unsteady mode and average results.
ping is offline   Reply With Quote

Old   May 14, 2020, 18:14
Default
  #6
New Member
 
Guoxing
Join Date: Oct 2018
Posts: 7
Rep Power: 5
Guoxing Chen is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
By Outlet boundary do you mean Outflow Boundary condition?

The pressure outlet BC fixes the pressure and sets the gradient of velocity to 0.

The outflow BC sets only the diffusive flux to zero. This constraint is a little weaker and allows stuff advect out.

The implications of the differences between these are really subtle.
Thanks for the inspired reply.
The OUTLET BC in starccm+ may be the same as OUTFLOW bc in ansys.
Guoxing Chen is offline   Reply With Quote

Old   May 14, 2020, 18:18
Default
  #7
New Member
 
Guoxing
Join Date: Oct 2018
Posts: 7
Rep Power: 5
Guoxing Chen is on a distinguished road
Quote:
Originally Posted by ping View Post
so this is what we call an external cfd case and so my mentioning a duct was for internal flow cfd. cases like this can be tricky for a few reasons one being the temperature and pressure gradient in the vertical direction so take a close look at velocity vectors on several vertical section planes across the domain and parallel to the wind direction and look for clues to the source of reverse flow.
and it is common for unsteady eddies etc to occur around buildings and this can cause residuals to plateau and so prevent steady state convergence. so look for these local effects and if they are small and repeatable then you can consider the case converged. otherwise you need to do some additional solving in unsteady mode and average results.
Thanks for the inspired reply.
I have found that most of the CFD simulation on urban wind environment were set it as outlow bc in ansys, which might be the same as outlet bc in starccm+. It was assumed that the flow was fully developed at the outlet, so using outlet bc in starccm+ is ok for my cases.
Guoxing Chen is offline   Reply With Quote

Old   May 15, 2020, 03:47
Default
  #8
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,448
Rep Power: 53
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Interesting... I was under the impression that there is no outlet BC in Star. But after verifying it, indeed there is a typo/error in drop down menu for the BC's. The outlet BC in star is actually a Flow Split Outlet which is not at all like the outflow BC.

The Flow Split Outlet BC extrapolates values from the interior to the boundary. This is equivalent to like a 0th order upwind scheme.

I don't know why Star doesn't have the outflow/fully developed BC as a boundary condition (because it does have the fully developed interface). Hopefully someone tells this to the Star bois.
LuckyTran is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind tunnel Boundary Conditions in Fluent metmet FLUENT 6 October 30, 2019 13:23
Getting divergence while increasing the back pressure at pressure outlet greenfields15 FLUENT 0 March 19, 2018 00:39
pressure outlet condition setup halfblood@SYSU Main CFD Forum 0 March 15, 2013 23:35
Pressure outlet BC help! eishinsnsayshin FLUENT 7 December 4, 2012 00:36
Unsteady pressure differential between inlet and outlet of the pipe for single phase joshi20h FLUENT 0 September 26, 2012 13:41


All times are GMT -4. The time now is 15:44.