CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Using outlet values as inlet BC

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 8, 2011, 07:37
Default Using outlet values as inlet BC
  #1
Member
 
Join Date: Apr 2010
Posts: 53
Rep Power: 8
bephi is on a distinguished road
Hello everybody,

my question is whether there is a possibility in OpenFOAM to use values from a calculation in a simple geometry as boundary conditions at the inlet of a complex geometry.

In my case, I need a fully developed velocity profile as a inlet boundary condition so at first I want to develop this profile in a straight pipe and use the outlet values.

Unfortunately I have no idea how to put them on the inlet of the other mesh!
With regards!
Philipp
bephi is offline   Reply With Quote

Old   February 8, 2011, 07:56
Default
  #2
New Member
 
Francisco Cortés
Join Date: Sep 2010
Location: Santiago, Chile
Posts: 7
Rep Power: 7
fcortes is on a distinguished road
I don't know if that can be done, but perhaps you could use groovyBC approximate the profile of your simple geometry solution…. Just an idea
Best regards,
Francisco.
fcortes is offline   Reply With Quote

Old   February 8, 2011, 08:05
Default
  #3
Member
 
Join Date: Apr 2010
Posts: 53
Rep Power: 8
bephi is on a distinguished road
Hello Francisco,
thank you for the quick reply! I thought of using groovyBC but the formula that I have to calculate the velocity is just for a circle. Unfortunately my inlet is not a perfect circle.
Maybe there is a way to map the values but I have no idea how to realize this...

Does someone else has an idea how to get the velocity profile at the inlet of the complex geometry?
bephi is offline   Reply With Quote

Old   February 8, 2011, 08:16
Default
  #4
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 12
MartinB is on a distinguished road
Hi Philipp,

to use a fully developed velocity profile on the inlet have a look at the directMapped boundary condition. You must define the BC in your 0/U file, as well as in the constant/polyMesh/boundary file. Here are some snippets:

Code:
0/U    File:
    inlet
    {
        //type            fixedValue;
        //value           uniform (0 0 0.063111);
	type            directMapped;
        value           uniform (0 0 0.063111);
        setAverage      true;
        average         (0 0 0.063111);
    }
Code:
constant/polyMesh/boundary file:
    inlet
    {
        type            directMappedPatch;
        nFaces          342; // <--- your values untouched here
        startFace       2804297;  // <--- your values untouched here
	sampleMode      nearestCell;
	sampleRegion    region0;
	samplePatch     none;
	offset          ( 0 0 0.01 );
    }
Another way as you suggest in your first post would be: use the mapFields tool and define in system/mapFieldsDict:
Code:
patchMap        ( outlet_from_one_simulation inlet_from_other_simulation );
(The last one might be the other way round, too, don't remember right now...).

Martin
MartinB is offline   Reply With Quote

Old   February 8, 2011, 08:38
Default
  #5
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 14
maddalena is on a distinguished road
Quote:
Originally Posted by bephi View Post
my question is whether there is a possibility in OpenFOAM to use values from a calculation in a simple geometry as boundary conditions at the inlet of a complex geometry.
I have done it using the timeVaryingMappedFixedValue on U.
Search in the forum for it, there should be something about it (this is what I get: http://www.cfd-online.com/Forums/ope...tml#post245855)

mad
maddalena is offline   Reply With Quote

Old   February 8, 2011, 10:01
Default
  #6
Member
 
Join Date: Apr 2010
Posts: 53
Rep Power: 8
bephi is on a distinguished road
Thank you all so much for your help!

@Martin:
Both suggestions seem to be a good idea! In the following days I try to realize those.
One important question is the following: How can I make sure that the mesh at the outlet (simple geometry) knows the mesh at the inlet (complex geometry). Does it have to be the same mesh with the same coordinates? Or can I map outletvalues to "every" inlet independent from cell number and coordinates?

@mad:
I will search for timeVaryingMappedFixedValue! But is it possible to achieve a velocity profile that is dependent on time and space or just a fixed value for U at different time steps (block profile).
bephi is offline   Reply With Quote

Old   February 8, 2011, 10:33
Default
  #7
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 252
Rep Power: 12
MartinB is on a distinguished road
Quote:
How can I make sure that the mesh at the outlet (simple geometry) knows the mesh at the inlet (complex geometry). Does it have to be the same mesh with the same coordinates? Or can I map outletvalues to "every" inlet independent from cell number and coordinates?
The outlet of the simple geometry must be at the same position in space as the inlet of the complex geometry. However, it's not necessary that the meshes are the same (have the same coordinates for the cells). The values will be interpolated, if the meshes are different.

Martin
MartinB 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
Boundary conditions: inlet and outlet aline OpenFOAM 7 June 29, 2010 03:45
Inlet and outlet boundary condition David Baker FLUENT 3 June 22, 2005 00:42
Inlet and outlet flow rate Neser CFX 1 March 2, 2004 17:02
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13
inlet and outlet boundary you FLUENT 2 May 10, 2001 17:10


All times are GMT -4. The time now is 17:53.