[chiven]

The simpleFoam solver is used. And a problem is met.

The inlet velocity condition is set as follows.
--------------------------------------------------------------------
pump-in
{
type surfaceNormalFixedValue;
value uniform -0.9611;
}
-------------------------------------------------------------------
However, failed. The errors are reported:
.................................................. ............................................
keyword refValue is undefined in dictionary "/home/g2/e090012/OpenFOAM/e090012-1.5/run/tutorials/simpleFoam/stratification/0/U:ump-in"
file: /home/g2/e090012/OpenFOAM/e090012-1.5/run/tutorials/simpleFoam/stratification/0/U:ump-in from line 31 to line 32.
From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line 213.
FOAM exiting
.................................................. .............................................
Then I revised it as:
-------------------------------------------------------------------
pump-in
{
type surfaceNormalFixedValue;
value -0.9611;
}
-------------------------------------------------------------------
still failed, and the errors are the same.

But the case can successfully run with "fixedValue" type.

Any comments? Thanks in advance.

[gwierink]

Hi Jiejin,

Perhaps it is the sign of the value that is the problem. Try

pump-in      
    {
        type            surfaceNormalFixedValue;
        value           uniform 0.9611;
    }

instead of

pump-in      
    {
        type            surfaceNormalFixedValue;
        value           uniform -0.9611;
    }

Regards,

Gijsbert

[chiven]

thank you, Wierink.

from the userguide, there is description like,

"surfaceNormalFixedValue Specifies a vector boundary condition, normal to the patch, by its magnitude; +ve for vectors pointing out of the domain"

thus I use the sign of "-" to mean pointing in of the domain.


anyway, I shall try it and report the results. Thanks.

[gwierink]

Yes, you are very right, that's what I read as well ... . I tried surfaceNormalFixedValue on a sinpleFoam tutorial and got the same error message: OF complains that the keyword refValue is not defined in 0/U. I simply replaced "value" with "refValue" and it worked! When you write the refValue to be 10, the solver still works, but it draws fluid out of the inlet instead of pumping it in to the domain. So the recipe that should work is:

pump-in
{
type surfaceNormalFixedValue;
refValue uniform -10;
}

I don't know whether this is how it is supposed to be, but it works. Perhaps it's a 1.5 thing?

Regards,

Gijsbert

[chiven]

Hi, Wierink, I do following your suggestions, it does work well. It is insteresting. How can you know that? You are a great man!

Thank you very much.

[roth]

Sort of makes sense though, no? We're setting velocity U so value would expect a vector, hence the need for refValue, a scalar.

Michael

[chiven]

hi, Michael, thank you for your tip. Now I understand.It is interesting.

[Sherlock_1812]

Hi all,
This is a really old thread but is the most relevant one to place my question in.

I have a curved patch which is an inlet on which the surfaceNormalFixedValue velocity is imposed. The initial magnitude and direction of the vectors are correct.

The case is a buoyancy driven flow in the domain surrounding this inlet. Timestep - 1e-05. Once the simulation starts the first time step is fine. But at the 3rd time step, there is some backflow into this curved patch at the bottom showing abnormally high velocities (rescaled maximum velocity ~ 1m/s) (Snapshots are attached)

Is there a way that I can provide the surfaceNormalFixedValue + no back flow condition to this curved patch?

Thanks in advance

[fetc95]

Originally Posted by Sherlock_1812

Hi all,
This is a really old thread but is the most relevant one to place my question in.

I have a curved patch which is an inlet on which the surfaceNormalFixedValue velocity is imposed. The initial magnitude and direction of the vectors are correct.

The case is a buoyancy driven flow in the domain surrounding this inlet. Timestep - 1e-05. Once the simulation starts the first time step is fine. But at the 3rd time step, there is some backflow into this curved patch at the bottom showing abnormally high velocities (rescaled maximum velocity ~ 1m/s) (Snapshots are attached)

Is there a way that I can provide the surfaceNormalFixedValue + no back flow condition to this curved patch?

Thanks in advance

Hello. Did you solve this problem? In my case I have a patch at which the surface-normal component of the velocity is to be zero but the solution which I get from openfoam has incorrect behavior of the velocity near this surface and it seems to be like your problem.