CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Some Problems about the Boundary Conditions in OpenFoam

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

Like Tree3Likes
  • 2 Post By Axel_T
  • 1 Post By Axel_T

Reply
 
LinkBack Thread Tools Display Modes
Old   January 4, 2010, 10:29
Question Some Problems about the Boundary Conditions in OpenFoam
  #1
Member
 
Join Date: Jun 2009
Posts: 34
Rep Power: 7
lzgwhy is on a distinguished road
Dear all,

How many kinds of boundary conditions (BCs) in OpenFoam? What are they? And how can I denote them in a BCs file of OpenFoam?

The above are some general problems I want to know. However, I faced a specific problem in practice. When I calculated the 2D flow over a 2D cylinder, I did not how to denote the boundary conditions for the cylinder wall and the external boundary which enclose the physical domain, though I knew the meaning of these BCs mathematically and how to set them in commercial software. In particular, how can I set pressure BC for a wall in OpenFoam, if there is no need to set value pressure or pressure gradient to the wall in advance? And how can I set velocity BC for a pressure outlet boundary, if there is no need to set value velocity to it in advance?

Thanks in advance!

Why
lzgwhy is offline   Reply With Quote

Old   January 5, 2010, 16:56
Default
  #2
New Member
 
Axel Tietjen
Join Date: Dec 2009
Location: Hamburg, Germany
Posts: 19
Rep Power: 7
Axel_T is on a distinguished road
Hi Why,

there are many types of BC, right. But they are all set in the fieldvariables in your first time-dictionary.

A simple pipe for example would have a inlet, outlet and fixed walls, when you defined the boundaries right during mesh-generation.
In the time-dictionary /0 must be for example the file of the pressure variable: /0/p
In that file there is a entry for the initial state:
internalField uniform 100000;
and a sub-dictionary for the boundaries:
boundaryField
{
inlet
{
type fixedValue;
value uniform 1.1e5;
}

fixedWalls
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 1e5;
}
}
For the velocity at the inlet, there is a BC called pressureInletOutletVelocity which calculates the velocity depending on the pressure.

Take a look at the OF-UserGuide chapter 5.2 especially page U-133

bye
Axel
Annier and Arjun Jayakumar like this.
Axel_T is offline   Reply With Quote

Old   January 7, 2010, 07:48
Post
  #3
Member
 
Join Date: Jun 2009
Posts: 34
Rep Power: 7
lzgwhy is on a distinguished road
Hi,Axel.

Thank you for your help. However, I tried to set new boundary conditions (BCs) again and re-calculate my problem with icoFoam solver. In these cases, OpenFoam could not conduct calculation correctly. I read the chaper you suggested, and I have some questions. Firstly, there is one kind of boundary, on which mathematically just one quantity is needed to set, for example, just velocity is needed to set and pressure will be calculated by the velocity field. How can I set this kind boundary condition for pressure and velocity boundary files in OpenFoam, i.e. p file and U file? The second question is about the selection of the solver in OpenFoam. Do you think I am right if I choose the icoFoam solver for the problem of fluid flow over a 2D cylinder, which is a classical external fluid flow problem? If not, which one solver would you like to suggest to me?

Thanks.

Why
lzgwhy is offline   Reply With Quote

Old   January 7, 2010, 13:10
Default
  #4
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 6
openfoam1 is on a distinguished road
yes , me too , i have the same problem ,, I have a velocity data and i want to put them in the inlet of my domain as a boundary condition
any one can help
thanks
openfoam1 is offline   Reply With Quote

Old   January 7, 2010, 22:57
Default
  #5
New Member
 
Axel Tietjen
Join Date: Dec 2009
Location: Hamburg, Germany
Posts: 19
Rep Power: 7
Axel_T is on a distinguished road
Hello Why,

I don't know if it would help a lot, but I show you the way I solved it at my problem: A chamber with only one inlet, where the pressure raises over time.

The pressure-boundary is in the file "p"
dimensions [1 -1 -2 0 0 0 0];

internalField uniform 400000;

boundaryField
{
inlet
{
type timeVaryingUniformFixedValue;
fileName "inlet_p.dat";
outOfBounds warn;
}

fixedWalls
{
type zeroGradient;
}
}
There used the timeVaryingUniformFixedValue to get the pressure growing over time. It loads the file "inlet_p.dat", which I created in this syntax:
(
(t0 p0)
(t1 p1)
...
(tn pn)
)

This file needs a strikt format, I think. So don't insert extra spaces or something like that. Just time and pressure.
The keyword outOfBounds says what to do when you enter a timestep which is not listet in the dat-file. There "warn" will hold the last value of the specified range and give you a warning message. Other options are error, clamp and repeat.


Then I defined my "U"-file in this way:
dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}

fixedWalls
{
type fixedValue;
value uniform (0 0 0);
}
}

ThepressureInletOutletVelocity can also be used when the flux can change direction, when you are shure that you will always have a inflow, the pressureInletVelocity would do it either.
I don't know why there must be specified a value for the inlet, because it's calculated, but it won't run without.

I hope I was able to point you in the right direction about that.

Good luck!

Axel
shininiu likes this.
Axel_T is offline   Reply With Quote

Old   February 8, 2010, 07:35
Default normal velocity
  #6
Member
 
hamdi
Join Date: Mar 2009
Posts: 72
Rep Power: 7
hamcer is on a distinguished road
hello,

I try to determine the normal velocity at each point on the boundary which declared as zerogradient, how can I do that?

Thanks in advance.
hamcer is offline   Reply With Quote

Old   February 8, 2010, 11:57
Default fixed value + alternating BC boundary condition = ??
  #7
Senior Member
 
Join Date: Dec 2009
Posts: 112
Rep Power: 7
heavy_user is on a distinguished road
Hi Folks,

i am running a case with reactingFoam.
I use steady BC, but the BC vary with each time Step ..
WHHYYY ??

My BC are:

Code:
pressure:

    inlet           
    {
        type            fixedValue;
        value           uniform 100000;
    }

T:
    inlet           
    {
        type            fixedValue;
     value         uniform 296;
    }
U:

 inlet
    {
        type            fixedValue;
        value           nonuniform List<vector> 
100
(
(0 0 67.552)
(0 0 67.77)
(0 0 67.035)
(0 0 65.8686)
(0 0 64.7974)
(0 0 63.5496)
(0 0 61.7962)
(0 0 59.7163)
(0 0 57.5885)
(0 0 54.9667)
(0 0 50.2231)
(0 0 36.2949)
(0 0 0.315833)
(0 0 6.57834)
(0 0 7.44999)
(0 0 7.96628)
(0 0 8.26225)
(0 0 8.49278)
(0 0 8.65498)
(0 0 8.76455)
(0 0 8.83736)
(0 0 8.88867)
(0 0 8.932)
(0 0 8.97775)
(0 0 9.03216)
(0 0 9.0771)
(0 0 9.2)
(0 0 9.2)
.
.
.
)
;
    }

Species:
C3H8 for r/R<1.
"AIR" for r/R>1.
so NOT time dependent BC.

When I check velocity with sample i get different results for each timstep:
(I use sample from (0 0 0) to (0 0.15 0) which should be exactly my (2D) inlet)

The Geometry is a box, with 2 adverce faces asigned the inlet and outlet, 2 adverse faces are declared empty, one face assigned symmetry and the other "wall"(here all BCs are assiged zeroGradient)

One of my favourite results:
(location Ux Uy Uz)

Code:
0 2.31962e-20    -0.308472    65.1918    
0.00015015 3.18149e-21    -0.0180087    67.4434    
0.0003003 -9.95544e-36    1.46518e-16    67.481    
0.00045045 0    0    66.9175    
0.000600601 0    0    66.1129    
0.000750751 0    0    65.2443    
0.000900901 0    0    64.3746    
0.00105105 0    5.15872e-16    63.3375    
0.0012012 0    -3.35738e-16    62.151    
0.00135135 0    -3.35738e-16    60.8089    
0.0015015 0    0    59.3887    
0.00165165 0    -6.66706e-16    57.9029    
0.0018018 0    1.33341e-15    56.3505    
0.00195195 0    0    54.0607    
0.0021021 0    0    50.486    
0.00225225 0    0    44.7908    
0.0024024 0    0    32.4953    
0.00255255 0    0    18.0146    
0.0027027 0    0    9.53493    
0.00285285 0    0    3.99707    
0.003003 0    0    5.9627    
0.00315315 0    0    7.18547    
0.0033033 1.54684e-34    5.29596e-15    7.55476    
0.00345345 0    0    7.83008    
0.0036036 0    0    8.0389    
0.00375375 0    0    8.19776    
0.0039039 0    0    8.32852    
0.00405405 -2.80758e-34    -4.26399e-15    8.4364    
0.0042042 -2.80758e-34    -4.26399e-15    8.53066    
0.00435435 2.75369e-34    -1.57786e-15    8.60796    
0.0045045 0    0    8.67098    
0.00465465 2.73743e-34    2.24416e-15    8.72545    
0.0048048 0    0    8.76632    
0.00495495 -1.36664e-34    -1.67595e-15    8.80503    
0.00510511 0    0    8.8319    
0.00525526 0    0    8.85877    
0.00540541 0    0    8.87967    
0.00555556 -2.68723e-34    5.9232e-15    8.89947    
0.00570571 -2.61375e-34    7.59204e-15    8.91845    
0.00585586 -2.61375e-34    7.59204e-15    8.93644    
0.00600601 0    0    8.95444    
0.00615616 -3.70648e-37    6.9118e-15    8.97396    
0.00630631 -3.70648e-37    6.9118e-15    8.99351    
0.00645646 0    0    9.01273    
0.00660661 0    0    9.03147    
0.00675676 0    0    9.05022    
0.00690691 4.66049e-34    -3.62717e-15    9.07803    
0.00705706 0    0    9.10858    
0.00720721 0    0    9.13892    
0.00735736 4.50919e-34    1.7008e-15    9.16062    
0.00750751 0    0    9.18232    
0.00765766 2.14111e-34    1.03588e-16    9.2    
0.00780781 0    0    9.2    
0.00795796 0    0    9.2    
0.00810811 0    0    9.2    
0.00825826 0    0    9.2    
0.00840841 0    0    9.2    
0.00855856 -4.06648e-34    5.09e-15    9.2    
0.00870871 0    0    9.2    
0.00885886 0    0    9.2    
  
.....
....
....
0.142492 0    0    9.2    
0.142643 0    0    9.2    
0.142793 0    0    9.2    
0.142943 0    0    9.2    
0.143093 0    0    9.2    
0.143243 0    0    9.2    
0.143393 0    0    9.2    
0.143544 0    0    9.2    
0.143694 0    -1.13922e-14    9.2    
0.143844 0    0    9.2    
0.143994 0    0    9.2    
0.144144 0    0    9.2    
0.144294 0    0    9.2    
0.144444 0    0    9.2    
0.144595 0    0    9.2    
0.144745 0    -1.13922e-14    9.2    
0.144895 0    -0.0605795    6.54958    
0.145045 0    -0.130931    3.47163    
0.145195 0    -0.201282    0.393675    
0.145345 0    -0.271634    -2.68428    
0.145495 0    -0.341985    -5.76223    
0.145646 0    -0.412336    -8.84018    
0.145796 0    -0.482688    -11.9181    
0.145946 0    -0.553039    -14.9961    
0.146096 0    -0.623391    -18.074    
0.146246 0    -0.693742    -21.152    
0.146396 0    -0.764093    -24.2299    
0.146547 0    -0.834445    -27.3079    
0.146697 0    -0.904796    -30.3858    
0.146847 0    -0.975147    -33.4638    
0.146997 0    -1.0455    -36.5418    
0.147147 0    -1.11585    -39.6197    
0.147297 0    -1.1862    -42.6977    
0.147447 0    -1.25655    -45.7756    
0.147598 0    -1.3269    -48.8536    
0.147748 0    -1.39726    -51.9315    
0.147898 0    -1.46761    -55.0095    
0.148048 0    -1.53796    -58.0874    
0.148198 0    -1.60831    -61.1654    
0.148348 0    -1.67866    -64.2433    
0.148498 0    -1.74901    -67.3213    
0.148649 0    -1.81936    -70.3992    
0.148799 0    -1.88972    -73.4772    
0.148949 0    -1.96007    -76.5551    
0.149099 0    -2.03042    -79.6331    
0.149249 0    -2.10077    -82.711    
0.149399 0    -2.17112    -85.789    
0.14955 0    -2.24147    -88.8669    
0.1497 0    -2.31182    -91.9449    
0.14985 0    -2.38217    -95.0228
I have no clue why it is doing this!
It does not go along with my understanding of "fixedValue" used for BC.

When I use calcMassflow on that Patch i get corresponding(same cracyness) results.

can anyone give me a hint on that, plz!?

regards !
heavy_user is offline   Reply With Quote

Old   February 6, 2012, 12:58
Default hi openfoamers
  #8
Member
 
Jignesh
Join Date: Aug 2011
Location: India
Posts: 68
Rep Power: 5
jignesh_thaker2007 is on a distinguished road
Send a message via Yahoo to jignesh_thaker2007
i have doubt in my problem like that

I have pipe flow problem ok so i enter the fluid inside the pipe so i give the velocity inlet values now i know that at inlet pressure is 1 pascal so and at the outlet pressure outlet condition is there so plz tel me at inlet how can i set the pressure?
jignesh_thaker2007 is offline   Reply With Quote

Old   February 28, 2012, 10:28
Default
  #9
New Member
 
Join Date: Sep 2011
Posts: 10
Rep Power: 5
yipiyaya8 is on a distinguished road
Quote:
Originally Posted by Axel_T View Post

Then I defined my "U"-file in this way:
dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}

fixedWalls
{
type fixedValue;
value uniform (0 0 0);
}
}

ThepressureInletOutletVelocity can also be used when the flux can change direction, when you are shure that you will always have a inflow, the pressureInletVelocity would do it either.

Hi Axel

My case is i know inlet T, P...also outlet P....

Hoever i want to let the openfoam to calculate the Inlet Velocity ...I tried to use

oulet
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}


but i dont know if this information is enough?!
}

Last edited by yipiyaya8; March 8, 2012 at 17:45.
yipiyaya8 is offline   Reply With Quote

Old   December 23, 2012, 04:34
Default
  #10
New Member
 
Gregory Paladin
Join Date: Jul 2012
Posts: 10
Rep Power: 4
paladin is on a distinguished road
Hi foamers !

Sorry to dig up this post, but i'm facing the same problem here..

I have a flame in the open, where i've imposed inlet velocity (because i have the velocity datas) and outlet pressure (atm. pressure, because it's in the open)

At first i've put a zeroGradient condition on the outlet velocity, but my domain is too short so the solver can't respect both conditions, a zerogradient velocity and a pressure that still have a gradient at the outlet.. So it seems like i also have to let openfoam calculate outlet velocity based on the pressure gradient at the outlet.

Anyway, does anyone knows why we can't just put a "calculated" type for the outlet velocity and (0 0 0) for initial value?

I get

Quote:
--> FOAM FATAL ERROR:

gradientInternalCoeffs cannot be called for a calculatedFvPatchField
on patch Outer of field U in file ".../SwirlFlame_kEps_calculatedVelocity/0/U"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::gradientInternalCoef fs() const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.

FOAM exiting

I've tried type pressureInletOutletVelocity and pressureInletVelocity types, but it doesn't change anything. (I use OF 2.0.x)

Last edited by paladin; December 23, 2012 at 05:52.
paladin is offline   Reply With Quote

Old   January 14, 2013, 01:15
Default urgent help
  #11
Member
 
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 87
Rep Power: 3
shipman is on a distinguished road
Hi eveybody,

I am the new user of the openFoam and nowadays tried to learn how i can use it. For one example i have used multiphase solver and apllied it to the 2-D symmetric nozzle which surface has been created in Star-CD and converted to OpenFoam. My question is that how can change the velocity values. You can see P and V BC are set as follow.

Thanks in advance for help.

object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [1 -1 -2 0 0];

internalField uniform 300e5;

boundaryField
{
Default
{
type totalPressure;
U U;
phi phiv;
rho rho;
psi none;
gamma 1;
p0 uniform 2e5;
}

Default_5
{
type fixedValue;
value uniform 1e5;
}

Default_10
{
type zeroGradient;
}
}

object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0];

internalField uniform (0 0 0);

boundaryField
{
Default
{
type zeroGradient;
value uniform (0 0 0);
}

Default_5
{
type zeroGradient;
value uniform (0 0 0);
}

Default_10
{
type fixedValue;
value uniform (0 0 0);
}

Default corresponds to Inlet
default_5 ==> outlet
Default?10==> walls
shipman is offline   Reply With Quote

Old   April 11, 2013, 12:31
Default
  #12
Member
 
Join Date: Mar 2013
Posts: 82
Rep Power: 3
giack is on a distinguished road
Hi to all
Someone know how velocity is obtained from pressure in pressureInletOutletVelocity?

thank to all
giack is offline   Reply With Quote

Old   May 16, 2014, 13:55
Default Boundary condition for sphere in OpenFOAM
  #13
New Member
 
sammasum
Join Date: May 2014
Posts: 1
Rep Power: 0
samice2008 is on a distinguished road
Hi,

I am trying to solve the sphere problem in the attachment. I have solved the problem with a fixedValue at the boundary but do not know what to do with this boundary conditions.

The challenge in the boundary is the direction of the normal vector. if it is in the positive X- direction then have a value of +1 but if it in the negative X-direction then the value is -1. Similarly for Y and Z axis.

FYI: The sphere is created from an .stl file and using blockMesh for a hexagon and the snappyHexMesh has been used to generate the mesh.

Desperatly looking for help

thanks
claire
Attached Images
File Type: jpg sphere with boundary condition.jpg (20.6 KB, 66 views)
samice2008 is offline   Reply With Quote

Old   July 8, 2014, 07:17
Default normal velocity
  #14
New Member
 
Ireneusz Czajka
Join Date: Nov 2013
Posts: 5
Rep Power: 3
iczajka is on a distinguished road
Is there possibility in openfoam to specify outlet velocity as normal ?
iczajka 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
Implementation of boundary conditions for FVM Tom Main CFD Forum 7 August 26, 2014 06:58
symmetry boundary conditions in cfx lost.identity CFX 41 May 22, 2013 08:21
LES of channel with cylic boundary mapping boundary conditions Thomas Baumann CD-adapco 0 August 24, 2009 10:53
compressible boundary conditions vivian Main CFD Forum 8 April 24, 2006 07:23
Boundary conditions? Tom Main CFD Forum 0 November 5, 2002 02:54


All times are GMT -4. The time now is 23:44.