CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

pressureGradient dictionary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 8, 2013, 12:11
Default pressureGradient dictionary
  #1
Member
 
Davide D.
Join Date: Oct 2012
Location: Birmingham (UK)
Posts: 44
Rep Power: 4
dav.dap83 is on a distinguished road
Hi,


I need to implement a pressureGradient force for spray parcels. I want to simulate gas parcels into a liquid using sprayFoam.

However, pressureGradient force needs a dictionary, and I have not been able to find an example of such a dictionary.
Can anyone provide an example, please?


Thanks
dav.dap83 is offline   Reply With Quote

Old   March 13, 2013, 23:53
Default
  #2
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 543
Rep Power: 18
chegdan will become famous soon enough
Voila!

Code:
    particleForces
    {
		gravity;
		pressureGradient
		{
			U	U;
		};

    }
Note: This works for 2.1.x
__________________
Dan

Find me on twitter @dancombest and LinkedIn
chegdan is offline   Reply With Quote

Old   October 4, 2014, 23:41
Default
  #3
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Quote:
Originally Posted by chegdan View Post
Voila!

Code:
    particleForces
    {
        gravity;
        pressureGradient
        {
            U    U;
        };

    }
Note: This works for 2.1.x
Hi,
It doesn't work with DPMFoam in 2.3.0
maysmech is offline   Reply With Quote

Old   October 5, 2014, 06:21
Default
  #4
Member
 
Davide D.
Join Date: Oct 2012
Location: Birmingham (UK)
Posts: 44
Rep Power: 4
dav.dap83 is on a distinguished road
Quote:
Originally Posted by maysmech View Post
Hi,
It doesn't work with DPMFoam in 2.3.0
In DPMFoam the velocity field of the fluid phase is named with Uc rather than U. So you just need to write:

Code:
    particleForces
    {
        gravity;
        pressureGradient
        {
            U    Uc;
        };

    }
dav.dap83 is offline   Reply With Quote

Old   October 5, 2014, 20:13
Default
  #5
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Quote:
Originally Posted by dav.dap83 View Post
In DPMFoam the velocity field of the fluid phase is named with Uc rather than U. So you just need to write:

Code:
    particleForces
    {
        gravity;
        pressureGradient
        {
            U    Uc;
        };

    }
Thanks, But it leads to this error:
Code:
--> FOAM FATAL ERROR: 

    request for volVectorField Uc from objectRegistry region0 failed
    available objects of type volVectorField are
1(U.air)

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/aut/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3  Foam::PressureGradientForce<Foam::KinematicCloud<Foam::Cloud<Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > > > >::cacheFields(bool) at ??:?
#4  
 at ??:?
#5  
 at ??:?
#6  
 at ??:?
#7  
 at ??:?
#8  
 at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 at ??:?
Aborted (core dumped)
DPMFoam uses U.air for velocity so using U.air instead of Uc leads to:

Code:
--> FOAM FATAL IO ERROR: 
keyword DUcDt is undefined in dictionary "/home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes"

file: /home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes from line 27 to line 29.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 437.

FOAM exiting
maysmech is offline   Reply With Quote

Old   January 11, 2015, 18:48
Default
  #6
Senior Member
 
Mojtaba.a's Avatar
 
Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 233
Rep Power: 7
Mojtaba.a is on a distinguished road
Send a message via Yahoo to Mojtaba.a
Quote:
Originally Posted by maysmech View Post
Thanks, But it leads to this error:
Code:
--> FOAM FATAL ERROR: 

    request for volVectorField Uc from objectRegistry region0 failed
    available objects of type volVectorField are
1(U.air)

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/aut/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3  Foam::PressureGradientForce<Foam::KinematicCloud<Foam::Cloud<Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > > > >::cacheFields(bool) at ??:?
#4  
 at ??:?
#5  
 at ??:?
#6  
 at ??:?
#7  
 at ??:?
#8  
 at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 at ??:?
Aborted (core dumped)
DPMFoam uses U.air for velocity so using U.air instead of Uc leads to:

Code:
--> FOAM FATAL IO ERROR: 
keyword DUcDt is undefined in dictionary "/home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes"

file: /home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes from line 27 to line 29.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 437.

FOAM exiting
Try
Code:
    interpolationSchemes
    {
        rho.air             cell;
        U.air               cellPoint;
        mu.air              cell;
        DUcDt            cellPoint;
    }
__________________
Complex Heat & Flow Simulation Research Group
If you can't explain it simply, you don't understand it well enough. "Richard Feynman"
Mojtaba.a 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
writing subDict in a dictionary ubaid OpenFOAM Programming & Development 3 October 25, 2014 17:17
New Boundary Condition: Reading Dictionary Problem Koga OpenFOAM Programming & Development 0 November 26, 2012 06:01
Reading from User Defined Dictionary File brosemu OpenFOAM Running, Solving & CFD 2 March 30, 2009 15:25
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51
FoamX error aachenBomb case Ervin Adorean (Adorean) OpenFOAM Pre-Processing 13 March 7, 2005 04:50


All times are GMT -4. The time now is 22:31.