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

nonreflective boudary conditions

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 15, 2011, 05:59
Default nonreflective boudary conditions
  #1
New Member
 
Matthias Finke
Join Date: Mar 2011
Posts: 12
Rep Power: 6
mfinke is on a distinguished road
Dear community members,

i working on a "displacement pump" model. The Fluid is defined as 1 phase compressibel flow (roh = f(p)) and a turbulence model is used.

Inlet and Outlet is defined as opening with pressure boundary condition with the nonreflective beta feature activated.

There are several GGIs defined to connect different parts of the pump (e.g. pistons with control journal).

Its a transient simulation with moving mesh regions.

Im using initial condtions from earlier simulation with reflective B.C. but large time step where the pressure wave propagation has no influence on flow behaviour.

Problem:
due to the constant pressure boundary conditions i have numeric pressure wave reflections at the Inlet and Outlet and later on propagation of this waves.

Therefore Im trying to use the nonreflective boundary condtion option in CFX-Pre but in the first Iteration i get the following error message:

"ERROR #001100279 has occurred in subroutine ErrAction.
Message:Signal caught: Segmentation violation"

"ERROR #001100279 has occurred in subroutine ErrAction.
Message: Stopped in routine SIG_HANDLER:"

any idea ?
Is there some limitation of this beta feature ?
I only know that nonreflective B.C. dont works together with multiphase flows.

best regards and thank you in advance

Matthias

Last edited by mfinke; March 16, 2011 at 06:05.
mfinke is offline   Reply With Quote

Old   March 18, 2011, 05:03
Default
  #2
New Member
 
Matthias Finke
Join Date: Mar 2011
Posts: 12
Rep Power: 6
mfinke is on a distinguished road
Dear members,
im still working on the problem. Meanwhile we find out that mesh motion has no influence on the error message.
Now im trying to figure out if grid Interfaces could be a source for the error. You are welcome to share your experience with me.

best regards

Matthias
mfinke is offline   Reply With Quote

Old   March 18, 2011, 07:22
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
That's probably why it is still in beta.

Just a wild idea, but try replacing the non-reflective boundary with a really coarse mesh just at the boundary. Connect it to the main domain with a GGI and put a normal pressure boundary at the exit. Very coarse meshes have high dissipation and you may be able to get a non-reflective (or at least not very reflective) boundary out of that.
ghorrocks is offline   Reply With Quote

Old   March 18, 2011, 15:16
Default
  #4
Senior Member
 
Join Date: Mar 2009
Location: Europe
Posts: 168
Rep Power: 8
joey2007 is on a distinguished road
Glenns approach is quite practical.

Do you use a turbulence resolving approach (LES, SAS, DES)? Then a coarse mesh may destroy also vortices flow upwards. Do not know if that is accurate. Unfortunately I do not have a better solution . If it is a scientific work, you may check:

A. Widenhorn, B. Noll, M. Aigner
Impedance boundary conditions for the numerical simulation of gas turbine combustion systems
ASME GT2008-50445, 2008
__________________
-
-
-
-
-
------------------------------------------------------------------------
Please do not forget: I am not paid for answering your questions.


Thousands of issues can cause a division by zero. Please do not capture a thread, with the argument: "I have the same issue ...."
joey2007 is offline   Reply With Quote

Old   March 21, 2011, 05:34
Default
  #5
New Member
 
Matthias Finke
Join Date: Mar 2011
Posts: 12
Rep Power: 6
mfinke is on a distinguished road
Dear members,

thank you for the suggestions made for my problem.

I have already tried to extrude the inlet and outlet (l=10m) of the pump. I used a bunching law for the extruded meshes (10 elements, 1st element hight 0,003m).

There reflection of the pressure wave were still there. I think i need to adapt the mesh density and pipe lenght and bondary condition type (see ghorrocks) to smooth/eliminate the pressure waves reflection. (a=1220 [m/s]@ high pressure pipe; a=200 [m/s] low pessure pipe; tsimulation = 2 x 0.033 [s])

Joey2007: thank you for the literature source. Hope your financial situation is ok ;-)

best regards

MAtthias
mfinke is offline   Reply With Quote

Old   March 21, 2011, 14:37
Default
  #6
Senior Member
 
Join Date: Mar 2009
Location: Europe
Posts: 168
Rep Power: 8
joey2007 is on a distinguished road
@Matthias: It is okay. I just wanted to remember some folks here, that you never have to look into the mouth of a gifted horse. Guess you may understand what I mean, if not it is not so important ....
__________________
-
-
-
-
-
------------------------------------------------------------------------
Please do not forget: I am not paid for answering your questions.


Thousands of issues can cause a division by zero. Please do not capture a thread, with the argument: "I have the same issue ...."
joey2007 is offline   Reply With Quote

Old   December 19, 2013, 16:23
Default
  #7
Senior Member
 
ali
Join Date: Oct 2009
Posts: 157
Rep Power: 7
alinik is on a distinguished road
Hey mfinke
were you able to resolve that error message?

Thanks
alinik is offline   Reply With Quote

Old   December 20, 2013, 03:47
Default
  #8
New Member
 
Matthias Finke
Join Date: Mar 2011
Posts: 12
Rep Power: 6
mfinke is on a distinguished road
Hey alinik,

yes i was, as i remember there were two possible reasons for the problem:
=> negative slope of density(p)-function ( while increasing pressure, density should increase also)
=> type of partition in distributed parallel runs

hope this helps

best regards
mfinke is offline   Reply With Quote

Old   December 20, 2013, 18:19
Default segmentation error
  #9
Senior Member
 
ali
Join Date: Oct 2009
Posts: 157
Rep Power: 7
alinik is on a distinguished road
Quote:
Originally Posted by mfinke View Post
Hey alinik,

yes i was, as i remember there were two possible reasons for the problem:
=> negative slope of density(p)-function ( while increasing pressure, density should increase also)
=> type of partition in distributed parallel runs

hope this helps

best regards
Thanks mfinke for your quick reply,

Since I am running it serial mode so it could not be a result of the second reason. Also I am modeling the flow around an airfoil at low Mach number so the flow could be assumed as incompressible(constrant density).
It has to be because of something else.
The fact is I am trying to impose the inlet BC using a fortran code. I am not sure if this is related to that fact. I receive absolutely no error while compiling the code and introducing the routine, function and inlet CEL. So it also seems that the fortran code and everything is fine.
I am desperatley looking for some solution to this error.

Any kind of information that might help is greatly appreciated.

Thanks

Ali,
alinik 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
HELP,how to define the periodic boudary conditions using the icem mesh? dada1204 FLUENT 2 May 1, 2012 17:06
Boudary conditions monochrome FLUENT 2 May 19, 2010 02:07
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24
Far field boudary conditions in FDM James Main CFD Forum 3 July 20, 2005 02:44
boudary conditions for flow past a sphere srijit goswami Main CFD Forum 3 January 27, 2001 08:28


All times are GMT -4. The time now is 11:05.