CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   problems about surfaceNormalFixedValue (http://www.cfd-online.com/Forums/openfoam-solving/64719-problems-about-surfacenormalfixedvalue.html)

chiven May 21, 2009 01:17

problems about surfaceNormalFixedValue
 
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::pump-in"
file: /home/g2/e090012/OpenFOAM/e090012-1.5/run/tutorials/simpleFoam/stratification/0/U::pump-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 May 21, 2009 03:57

Hi Jiejin,

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

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

instead of

Code:

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

Regards,

Gijsbert

chiven May 21, 2009 04:24

Thanks for the comments
 
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 May 21, 2009 06:56

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 May 21, 2009 07:14

it is OK, thank you
 
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 May 21, 2009 07:45

U is a vector
 
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 May 21, 2009 08:36

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

Sherlock_1812 June 5, 2014 09:52

trouble with sporadic velocities
 
3 Attachment(s)
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


All times are GMT -4. The time now is 00:45.