[calim_cfd]

Originally Posted by sh.d

hi dear mauricio
thanks for your answer.
But I did not answer my question:
What is the difference between value and tangential velocity?Is this value scalar or vector?

hi
i cannot access OF right now but i guess that this value is a scalar . The tangential velocity might be a scalar or a vector depending on what OF is asking. i cant check the files atm. when i reach them ill try to post a better reply.
l8r

[kornickel]

Originally Posted by calim_cfd

hi
pressureinletoutletvelocity (in) bcs are to be used with inletoutlet (out) bcs for the u field

and you use totalpressure(in) and fixedvalue(out) for the p field

these bcs guarantee a well-posed problem in case the user has only pressure measures and backflow expected

try that
l8r and gl

Hey, regarding calim_cfd's post, what if I just have the static pressure and definitely need this pressure on my inlet surface (not calculated backwards from velocity), is there a suitable and clean way to make the inlet patch fixedValue in the pressure field? Using the other bcs above?

I also use simpleFoam, so I want to keep rho out of my calculation until postprocessing.

[hz283]

Hi All,

About the boundary condition presureinletoutletvelocity, I have a question:

for outflow, zero gradient, ok, it is clear.

for inflow, from the description we can see that for inflow the velocity is obtained from the patch-face normal component of the internal-cell value. Actually it is also zero gradient! So what is the difference between this case and outflow?

Any comments?

Originally Posted by calim_cfd

the bcs i mentioned they kinda form a consistent pair and regarding the usage,, i guess you can use it for outlets, but then you have to handle the signs..

here's the description, guess you've seen it already.. i haven't tried it thou

pressureInletOutletVelocity

Description
    Velocity inlet/outlet boundary condition patches for where the pressure is
    specified.  zero-gradient is applied for outflow (as defined by the flux)
    and for inflow the velocity is obtained from the patch-face normal
    component of the internal-cell value.

pls give it a try if u have the time and keep us post!
ty

[skyinventorbt]

Velocity is a vector quantity.
Use it as shown below...

tangentialVelocity uniform (0 0 0); // this is an additional condition that you can specify on a patch
--
KANNAN

[nash]

Originally Posted by Aadhavan

Hi Fomers and Calim;

I am simulating a fan using MRFSimpleFoam,
I have given the boundary condition as follows,
0/U

inlet
{
type flowRateInletVelocity;
flowRate 2;
value uniform (0 0 0);
}
outlet
{
type zeroGradient;
}

0/P

inlet
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 101325;
}

the simulation ran upto 10000 Iteration,
I have attached the Residual plot as well, please have a look.
but the result is not matching with experimental result.

actually inlet pressure should be less than outlet pressure but I an getting other way around.

I am trying to fix this issue by giving different BC as follows,

0/U

outlet
{
type zeroGradient;
}
inlet
{
type pressureInletOutletVelocity;
value uniform (0 0 0)

0/p

inlet
{
type totalPressure;
gamma 0;
p0 uniform 101325; // total pressure
value uniform 101325;
}

outlet
{
type fixedValue;
value uniform 101260.5; // static pressure
}

while execute the solver, I am getting the following error,

Create mesh for time = 0

Reading field p

Reading field U



--> FOAM FATAL IO ERROR:
Cannot find patchField entry for cyclic ILR0
Is your field uptodate with split cyclics?
Run foamUpgradeCyclics to convert mesh and fields to split cyclics.

file: /home/cerecam/OpenFOAM/OpenFOAM-2.0.1/tutorials/incompressible/MRFSimpleFoam/exCompDomain/onlyPressure/0/U::boundaryField from line 25 to line 76.

From function GeometricField<Type, PatchField, GeoMesh>::
GeometricBoundaryField::GeometricBoundaryField
(
const BoundaryMesh&,
const DimensionedField<Type, GeoMesh>&,
const dictionary&
)
in file /home/cerecam/OpenFOAM/OpenFOAM-2.0.1/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 271.

FOAM exiting


please guide me how to approach this problem,
I am really struggling to solve this problem.
please help me,

thanks,
Aadhavn

Hi Aadhavn,
i simulate the centrifugal fan as well and get higher static pressure at inlet and lower static pressure at outlet. I set the massflow at inlet with zeroGradient pressure and at outlet zeroGradient velocity and fixedValue pressure zero.

have you or anyone now how to fix this ?

thanks
-nash

[openfoammaofnepo]

Hi All,

If the inlet and outlet are very far from the flow of interest like the airfoil here, I mean the computational domain is large compared to the airfoil, Can I use pressureinletoutletvelocity (for U) and totalPressure (for p) for both inlet and outlet?

Because I use the above options but near the inlet BC there are always unphysical solutions like very large velocity, sometimes like a vortex (positive and negative appearing at the same time there). I am not sure if this is caused by the not reason BC setting.

Thank you for any comments.

Originally Posted by calim_cfd

hi
pressureinletoutletvelocity (in) bcs are to be used with inletoutlet (out) bcs for the u field

and you use totalpressure(in) and fixedvalue(out) for the p field

these bcs guarantee a well-posed problem in case the user has only pressure measures and backflow expected

try that
l8r and gl

[giack]

It is possible that your boundary condition setting give you unphysical results. In my work I tried this kind of boundary condition setting (pressureInletOutletvelocity for inlet and outlet) and they give me wrong results as you.

what is your physical inlet boundary condition? If is a flux that enter in the domain there isn't reason to set a pressureInletOutletVelocity in the inlet for U.

[openfoammaofnepo]

Actually it is an open atomshperic inlet (or strictly it is not an inlet). Sometimes the flow can enter the domain but sometimes it will flow out. How does your unphysical look like? Mine is always: unphysical pressure (very large) and so unphysical velocity. Actually the flow there should be very 'quiet'. Thank you.

[giack]

I had an unphysical reverse flow but the value of p and U are ok.

What is your outlet?The same of the inlet?

[openfoammaofnepo]

When I use the same condition for inlet and outlet, i.e. pressureinletOutletVelocity for U and totalPressure for p, the flow near the outlet is correct. The unphysical problem lies near the inlet.

I think reverse flow from this kind of BC is normal......

[giack]

not in my case, but my simulation had also mesh problem so I'm not sure that the problem is the boundary condition setting.. In any case, for a well posed problem you have to set the pressure in one side and the U in the other.. With your boundary condition setting you set the pressure both in inlet and outlet...Try to change, if possible, the outlet boundary condition

[openfoammaofnepo]

Thank you for your suggestions.

Now I am trying:

for inlet:

U: pressureinletOutletVelocity
p: totalPressure

for outlet:
U: inletOutlet
p: zeroGradient

The case is running and not sure this will improve it. Theoretically speaking this should be fine. Did you try the above options in your simulations?

[giack]

I didn't try their because I decided to change the boundary and put a wall on one hand (I haven't the necessity tho have two open side in my simulation). I'm not sure that your new setting work properly beacause when there is outflow in both boundaries the soler setted the pressure in both side.

Say me if with this setting the solver work without problem

[openfoammaofnepo]

Hi giack,

If I use the following setting for the totalPressure:

 //        type            totalPressure;
//        p0              uniform 0;
//        U               U;
//        phi             phi;
//        rho             none;
//        psi             none;
//        gamma           1.4;
//        value           uniform 0;

So this options correspond to the following operation in the source code:

operator==(p0p - 0.5*(1.0 - pos(phip))*magSqr(Up));

Here what is pos(phip)? I am a little confused about this.

[ThomasV]

Originally Posted by openfoammaofnepo

operator==(p0p - 0.5*(1.0 - pos(phip))*magSqr(Up));

Here what is pos(phip)? I am a little confused about this.

It is meant to act like a boolean. It checks for the sign of phip - i.e. the flux on the patch. If the flux is positive or zero pos(phip) will become "1" otherwise it'll be "0". So depending on the direction of the flux it's either...



... or ...



As a positive flux should indicate a flux out of the domain it'll just apply while if there's a flux into the domain it'll subtract the term from . I guess that's why this BC is suitable for being used for a velocity inlet as it changes the pressure according to U for an inward flux...

[openfoammaofnepo]

Thank you. I got the reply one year later!

[cleoo]

Originally Posted by calim_cfd

hi
pressureinletoutletvelocity (in) bcs are to be used with inletoutlet (out) bcs for the u field

and you use totalpressure(in) and fixedvalue(out) for the p field

these bcs guarantee a well-posed problem in case the user has only pressure measures and backflow expected

try that
l8r and gl

does this have to be used with a multiphase case or with just one?

[eb19]

Originally Posted by hz283

Hi All,

About the boundary condition presureinletoutletvelocity, I have a question:

for outflow, zero gradient, ok, it is clear.

for inflow, from the description we can see that for inflow the velocity is obtained from the patch-face normal component of the internal-cell value. Actually it is also zero gradient! So what is the difference between this case and outflow?

Any comments?

Hi,

Have you got an answer to your question? I also think the same.
I am just thinking, could it be the boundary conditions of velocity are not always zero gradient, but is a fixed gradient. Only in the case of zero gradient, then regardless inflow or outflow, the two conditions are actually the same.

What do you think?

[Raza Javed]

Hello Everyone,


I am modelling a fluid flow from a rectangular pipe. You can see in the figure attached.
(yellow region is fluid, and green region is pipe).


I know the Pressure, Velocity and Temperature of the fluid at the inlet.



Now, if due to some reason, some temperature rise from the outside of the pipe occurs, that will also raise the temperature of the fluid, then at the outlet the temperature of the fluid will be different. How can I find the temperature at the outlet?


And what boundary conditions for pressure, velocity and temperature would be suitable at inlet and outlet?


I shall be very thankful if someone can help me out in this.


Thank you

[JoshWilliams1996]

Originally Posted by sh.d

hi dear mauricio
thanks for your answer.
But I did not answer my question:
What is the difference between value and tangential velocity?Is this value scalar or vector?

Still doesn't answer your question but I hope this helps, from the .H file.

This velocity inlet/outlet boundary condition is applied to pressure
    boundaries where the pressure is specified.  A zero-gradient condtion is
    applied for outflow (as defined by the flux); for inflow, the velocity is
    obtained from the patch-face normal component of the internal-cell value.

    The tangential patch velocity can be optionally specified.

    \heading Patch usage

    \table
        Property     | Description             | Required    | Default value
        phi          | flux field name         | no          | phi
        tangentialVelocity | tangential velocity field | no  |
    \endtable

The key thing for you is perhaps that tangential velocity is a vector, but it is optional. I guess it relates to 'for inflow, the velocity is obtained from the patch-face normal component of the internal-cell value.'. i.e. it is up to the user to specify an additional component if necessary.