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

Boundary Condition

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 10, 2006, 23:10
Default Hello, I have recently been
  #1
Member
 
Shaun Cooper
Join Date: Mar 2009
Posts: 54
Rep Power: 8
coops is on a distinguished road
Hello,

I have recently been playing with the forwardSetp case using the sonicFoam application. I have changed the meshing to suit the case I am interested in but when I do this I want to specify a zeroGradient boundary condition. I attempt to do this for U (changing the patch from symmetryPlane to zeroGradient) and I get the following:

Calculating field e from T

Reading field U



--> FOAM FATAL IO ERROR : inconsistent patch and patchField types for
patch type symmetryPlane and patchField type zeroGradient

file: /home/shaun/OpenFOAM/shaun-1.3/run/editting/forwardStepmeshing/0/U::top from line 52 to line 52.

From function fvPatchField<type>const fvPatch&, const Field<type>&, const dictionary&)
in file /home/shaun/OpenFOAM/OpenFOAM-1.3/src/finiteVolume/lnInclude/newFvPatchField.C at line 137.

FOAM exiting

What is happeing here and how can I fix this problem.

Thanks in advance,

Shaun
coops is offline   Reply With Quote

Old   October 12, 2006, 12:27
Default Simple: a symmetry plane patch
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Simple: a symmetry plane patch type needs a symmetry patch field type.
mattijs is offline   Reply With Quote

Old   October 12, 2006, 17:55
Default Hi Mattijs, What you have s
  #3
Member
 
Shaun Cooper
Join Date: Mar 2009
Posts: 54
Rep Power: 8
coops is on a distinguished road
Hi Mattijs,

What you have said makes sense, my question is, where is it in the case is it defined to be a symmetry plane patch type? Symmetry plane patch type is not mentioned in the blockmesh file, it is only in the initial fields files.

Does it have something to do with the application (sonicFoam) being used?

Thanks
coops is offline   Reply With Quote

Old   October 13, 2006, 03:49
Default Check your boundary file (cons
  #4
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Check your boundary file (constant/polyMesh/boundary). It might have preserved any settings from FoamX. Delete it and rerun blockMesh.
mattijs is offline   Reply With Quote

Old   October 15, 2006, 01:04
Default Hi Mattijs, Once I deleted
  #5
Member
 
Shaun Cooper
Join Date: Mar 2009
Posts: 54
Rep Power: 8
coops is on a distinguished road
Hi Mattijs,

Once I deleted the boundary file and rerun blockMesh it did allow other boundary conditions.

Thanks again

Shaun
coops is offline   Reply With Quote

Old   November 8, 2006, 06:00
Default Hello, I want to simulate the
  #6
Member
 
Ralph
Join Date: Mar 2009
Posts: 40
Rep Power: 8
ralph is on a distinguished road
Hello,
I want to simulate the flow around an airfoil.
The flow is incompressible.
The computational domain I used so far is of rectangular shape with the airfoil placed inside.
As boundary conditions I used:
inlet: fixed velocity
outlet: fixed pressure
airfoil: wall
sidewise domain bound: slip

The simulation showed that the domain was too small to model a farfield.

To avoid extending the domain I asked, if there is a kind of farfield boundary condition available.
Are the "freestream" and "freestreamPressure" boundary conditions suitable for that kind of problem (instead of using the slip condition)?
Is there a better choice as the fixed pressure at the outlet (in order to avoid extending the domain)?
Can anyone give me a hint?

Thanks in advance

Ralph
ralph is offline   Reply With Quote

Old   November 8, 2006, 06:45
Default Hi Ralph, Unless you don't ha
  #7
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Hi Ralph,
Unless you don't have a specific request for the solver, I would recomend you a different approach: a boundary layer method is much cheaper and usually more accurate than RANS.
An open source software that implements such a method is called XFOIL.

Dragos
jiaojiao likes this.
dmoroian is offline   Reply With Quote

Old   November 8, 2006, 06:58
Default Thats not quite what Im look
  #8
Member
 
Ralph
Join Date: Mar 2009
Posts: 40
Rep Power: 8
ralph is on a distinguished road
Thats not quite what Im looking for Dragos.
But thanks for the hint.
I intend to further use OpenFOAM with a (U)RANS approach.
I got quite familiar with this code and am pleased with its capabilities.
The analysis of the airfoil should be the basis for further investigations with an (U)RANS approach.
Id be thankful for further hints concerning the boundary conditions.

Ralph
ralph is offline   Reply With Quote

Old   November 9, 2006, 07:58
Default Hi all, by further looking at
  #9
Member
 
Ralph
Join Date: Mar 2009
Posts: 40
Rep Power: 8
ralph is on a distinguished road
Hi all,
by further looking at the boundary conditions I got a little more insight.
But there are still two things I dont get.

1) I think to know what a inletOutlet is.
But what is the derived boundary condition freestream?

2) When an inletOutlet switches between inlet and outlet, what does a outletInlet? (isnt it the same?)

Is one of both BCs suitable for the farfield boundary of an external flow?

Ralph
ralph is offline   Reply With Quote

Old   November 9, 2006, 08:44
Default The idea of inletOutlet is tha
  #10
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
The idea of inletOutlet is that the boundary condition will change its behaviour based on the direction of the flux on the boundary. Thus, if the flux is going in on a face, the b.c. acts as fixed value; if it is going out, it acts as zero gradient.

outletInlet will (of course) do the exact opposite.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   November 9, 2006, 08:49
Default Thanks Hrvoje, could you also
  #11
Member
 
Ralph
Join Date: Mar 2009
Posts: 40
Rep Power: 8
ralph is on a distinguished road
Thanks Hrvoje,
could you also tell me what the freestream condition is?
It is derived from inletOutlet.

Ralph
ralph is offline   Reply With Quote

Old   January 5, 2007, 12:20
Default Base - numeric(primitive, deri
  #12
Senior Member
 
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 9
maka is on a distinguished road
Base - numeric(primitive, derived)- physical type b.c.

I went trough the documentation to understand the difference between the above boundary types. I came up with the following. I will be thankful if you can correct me:

1) physical type (optional): only affects the way FoamX works but has no effect if you are editing the files manually (as I do). I tried to specify any invalid name in front of physicalType and solver did not complain. Specified in boundary file.

2) base type: only affects geometrical or data communication functionality. Also wall is need by wall functions. Specified in blockMeshDict or boundary file.

3) numeric (primitive or derived): are needed by numerical algorithm that works on the fields. Specified in Field file.

4) base and numeric type has to match in case the base type was "symmetryPlane" or "empty". otherwise, they can be different.

Problem:
5) changing patch type in blockMeshDict and rerunning blockMesh will not update boundary file content (if the file already exist) but will update its access date. As a result the computation will not be affected by such change. blockMesh will print no warning about that and will not check the validity of new patch type.

The change is blockMeshDict is only effective if:
  1. we change, for example the number of cells and the patch type, then boundary file will be update successfully.
  2. we remembered to delete the existing boundary file.

Should this be reported as a bug?

Thanks in advance!
best regards,
Maka
maka is offline   Reply With Quote

Old   January 5, 2007, 15:11
Default Nope - it is done deliberately
  #13
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Nope - it is done deliberately to preserve boundary types in FoamX. Just delete the boundary file, run blockMesh and all will be well.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 8, 2007, 23:23
Default Both derived from basic symmet
  #14
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Both derived from basic symmetry, ie. doing the same thing. You can hook up slip on any kind of patch (e.g. for a slippery wall) whereas a symmetry plane is a geometrically enforced type.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 16, 2007, 11:39
Default Hello everyone One basic quas
  #15
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hello everyone
One basic quastion

In N.S equation we see laplacian of velocity and gradient of pressure .So with 3 boundry conditions (2 for velocity&1 for Pressure )the equation must be solved.

But in OpenFOAM the condition of Velocity&pressure in inlet&outlet must be realized.

This means 4 boundry conditoin for NSE.

How this has justified?
marhamat is offline   Reply With Quote

Old   January 17, 2007, 10:12
Default I mean that for solution flows
  #16
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
I mean that for solution flows such as pipe flow by imposing velosity in inlet&wall and pressure in inlet we can reach to result(such az velociy in outlet and pressure in wall&outlet) .
But in OpenFOAM in each boundry the condition of velocity&pressure both must be realized.
For example if we impose wall to wall boundry condition then velocity is fixed & pressure gradient is zero.
How this has justified?
Really i want to know can i make new boundry condition that condition of pressure in wall be unknown ?(and in similar cases in other boundries)

Thanks alot
Marhamat
marhamat is offline   Reply With Quote

Old   January 19, 2007, 04:15
Default Hello everyone Sorry for freq
  #17
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hello everyone
Sorry for frequent questions

The conception of boundry condition in FOAM isn't clear for me.

For example when we impose wall to wall boundry condition then velocit value & pressure gradient are zero in this boundry .

What means zero pressure gradient.

What happens if we don't impose it to wall?

This means the result after convergence gives pressure and it's gradient in wall.

Assume that in pipe flow we make boundry conditions that in it only pressure&velocity in inlet &velocity in wall &velocity gradient in outlet are known.

And assume in another case we impose inlet to inlet boundry condition that in it velocity value is know & pressure grdient is zero and wall to wall and inltOutlet to outlet boundry condition that in it pressure value & velocity gradient is known.

1)Can we make the first case boundry conditions in OpenFOAM?
2)Do results differ in case 1and 2?How much and why?
any help is useful for me

Best regards
Marhamat
marhamat is offline   Reply With Quote

Old   March 23, 2007, 11:02
Default consistency check between patc
  #18
Senior Member
 
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 9
maka is on a distinguished road
consistency check between patch and patchField type:

such consistency check does not always work. There are two cases to consider:

a) when symmetryPlane, cyclic, empty (I have not tested wedge or processor) is specified in "blockMeshDict " but other type in field file (for example, Fixed value):

the check only works in case of symmetryPlane.

b) when symmetry, cyclic, empty (I have not tested wedge or processor) is specified in "field file" but other type in blockMeshDict (for example, patch):

The check works in all cases.

I tested that in cavity tutorial case.

IMPORTANT Note: Do not forget to remove "boundary" file every time you modify blockMeshDict if you want to test such effect.

As a result one can modify boundary condition in field file and run a computations that seems to ignore such modification. Actually, one can ask which of the two condition will override the other? I noticed that the geometrically enforced one (defined in blockMeshDict) does overrides the field b.c. Is that always the case?

Is that a big or it works this way for a reason that was not obvious to me. Thanks.

Best regards,
Maka
maka is offline   Reply With Quote

Old   March 26, 2007, 01:07
Default Hi, everyone I've find a
  #19
Member
 
Bobby
Join Date: Mar 2009
Location: wuhan, hubei, China
Posts: 33
Rep Power: 8
aderliner is on a distinguished road
Hi, everyone

I've find a "turbulence inlet" boundary condition in the solver oodles and Xoodles, but, if I want to use this boundary condition in another solver which does not have the choice,"turbulence inlet", in FoamX, what should I do?

Thanks~~!

Bobby
aderliner is offline   Reply With Quote

Old   March 26, 2007, 05:30
Default Is that a bug? In the above
  #20
Senior Member
 
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 9
maka is on a distinguished road
Is that a bug?

In the above message 23 March 2007,
"Is that a big or ...". :-) I meant is that a bug. Sorry for the typing mistake.

Best regards,
Maka.
maka 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 condition for UDS Tomik FLUENT 0 December 5, 2006 18:37
Boundary condition of the third kind or Danckwertz boundary condition plage OpenFOAM Running, Solving & CFD 4 October 3, 2006 12:21
Slip Boundary Condition for Moving Boundary Shukla Main CFD Forum 3 November 11, 2005 16:02
UDF boundary condition Jeff FLUENT 2 November 20, 2003 18:15
Boundary Condition in LES Zhang Tsiang Main CFD Forum 3 February 5, 2002 21:15


All times are GMT -4. The time now is 05:00.