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/)
-   -   Inlet BC OpenFOAM 12 (http://www.cfd-online.com/Forums/openfoam-solving/60504-inlet-bc-openfoam-12-a.html)

ghanshyam August 30, 2005 05:04

It looks like in ver 1.2, tota
 
It looks like in ver 1.2, totalPressureInlet and inletOutlet bcs have been removed. In ver 1.1 at the inlet, three options were there, i.e. totalPressureInlet, inletOutlet, and pressureInlet. Now only pressureIlnet is available. Am I correct or something is wrong with my installation?

Regards
GS

henry August 30, 2005 05:14

No boundary conditions have be
 
No boundary conditions have been removed and some have been added. You will find the BC implementations in sub-directories of OpenFOAM-1.2/src/OpenFOAM/fields/fvPatchFields or in OpenFOAM-1.2/src/cfdTools/general/derivedFvPatchFields.

ghanshyam August 30, 2005 05:24

Thanks Henry. I am just going
 
Thanks Henry. I am just going through the new version. Now at the "outlet" many more options are available and an extra "inletOutlet" category has been added in ver 1.2. This will be very usefull for external flows.

Thanks and regards
GS

ghanshyam August 30, 2005 07:35

For k and epsilon wall BCs in
 
For k and epsilon wall BCs in ver 1.1 we had two options (a) k -> fixedValue, epsilon -> zeroGradient
(b) wall function (i.e. zero gradient for k and epsilon)

These two options are still available in 1.2, but when I use option (a) I get following message:

------------------------------------------
--> FOAM FATAL ERROR : fixedValue is the wrong k patchField type for wall-functi
ons on patch plate_wall
should be zeroGradient

From function wall-function evaluation
in file /data/OpenFOAM/OpenFOAM-1.2/src/cfdTools/general/lnInclude/checkPatc
hFieldTypes.H at line 3.

FOAM exiting
------------------------------------------

It looks like it is forcing to use wall function. In case I do not want to use wall function what do I do?

Regards
GS

henry August 30, 2005 07:45

All high-Re turbulence models
 
All high-Re turbulence models use wall-function of some kind because that is a requirement. For wall functions to work properly you must choose appropriate boundary conditions for the form of the implementation which in the case of OpenFOAM is zeroGradient on both k and epsilon. If you have been choosing otherwise your results will be wrong. To stop people making this error I have put in a check in 1.2.

If you don't want to use wall-functions choose a low-Re model with special near-wall modelling and run with a mesh fine enough in the near-wall region for it to be stable. There are several low-Re turbulence models to choose from.

If you don't like either of these options there are two others, either run with slip walls or implement the model and boundary conditions you think is best for your purpose.

ghanshyam August 30, 2005 08:16

Thanks Henry for the clarifica
 
Thanks Henry for the clarification. I will prefer to go for realizable k epsilon model with a two layer approach near the wall. Which you know I have already implemented. I will test and see how it works with this version.

Regards
GS

henry August 30, 2005 08:20

... and you should choose the
 
... and you should choose the k-epsilon BCs that are appropriate for your implementation of the two layer approach which may not be a standard option in FoamX so you might have to either edit the k-epsilon files by hand and specify the BCs that way or add the options you require to the FoamX configuration files.

ghanshyam August 30, 2005 08:44

Thats right. Basically it will
 
Thats right. Basically it will be same as the one for low Re models.

Regards
GS


All times are GMT -4. The time now is 16:08.