CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

MSHArequest for surfaceScalarField phi from objectRegistry

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 23, 2007, 01:57
Default My blockmeshdict is :
  #1
Member
 
Mojtaba Shahmohammadian
Join Date: Mar 2009
Posts: 73
Rep Power: 7
msha is on a distinguished road
My blockmeshdict is :





/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.3 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "";
case "";
instance "";
local "";

class dictionary;
object blockMeshDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
(-0.5 0.33377906 0.01457311)
(-0.45 0.31030427 0.01354818)
(-0.4 0.28768137 0.01256044)
(-0.35 0.26612769 0.01161939)
(-0.3 0.24592454 0.0107373)
(-0.25 0.22743209 0.0099299)
(-0.2 0.21110041 0.00921684)
(-0.15 0.19746635 0.00862157)
(-0.1 0.18712052 0.00816986)
(-0.05 0.1806288 0.00788642)
(0 0.17841241 0.00778965)
(0.05 0.1806288 0.00788642)
(0.1 0.18712052 0.00816986)
(0.15 0.19746635 0.00862157)
(0.2 0.21110041 0.00921684)
(0.25 0.22743209 0.0099299)
(0.3 0.24592454 0.0107373)
(0.35 0.26612769 0.01161939)
(0.4 0.28768137 0.01256044)
(0.45 0.31030427 0.01354818)
(0.5 0.33377906 0.01457311)

(-0.5 0.33377906 -0.01457311)
(-0.45 0.31030427 -0.01354818)
(-0.4 0.28768137 -0.01256044)
(-0.35 0.26612769 -0.01161939)
(-0.3 0.24592454 -0.0107373)
(-0.25 0.22743209 -0.0099299)
(-0.2 0.21110041 -0.00921684)
(-0.15 0.19746635 -0.00862157)
(-0.1 0.18712052 -0.00816986)
(-0.05 0.1806288 -0.00788642)
(0 0.17841241 -0.00778965)
(0.05 0.1806288 -0.00788642)
(0.1 0.18712052 -0.00816986)
(0.15 0.19746635 -0.00862157)
(0.2 0.21110041 -0.00921684)
(0.25 0.22743209 -0.0099299)
(0.3 0.24592454 -0.0107373)
(0.35 0.26612769 -0.01161939)
(0.4 0.28768137 -0.01256044)
(0.45 0.31030427 -0.01354818)
(0.5 0.33377906 -0.01457311)

( -0.5 0 0)
(-0.45 0 0)
(-0.4 0 0)
(-0.35 0 0)
(-0.3 0 0)
(-0.25 0 0)
(-0.2 0 0)
(-0.15 0 0)
(-0.1 0 0)
(-0.05 0 0)
(0 0 0)
(0.05 0 0)
(0.1 0 0)
(0.15 0 0)
(0.2 0 0)
(0.25 0 0)
(0.3 0 0)
(0.35 0 0)
(0.4 0 0)
(0.45 0 0)
(0.5 0 0)

);

blocks
(

hex (42 43 22 21 42 43 1 0) (5 20 1) simpleGrading (1 1 1)
hex (43 44 23 22 43 44 2 1) (5 20 1) simpleGrading (1 1 1)
hex (44 45 24 23 44 45 3 2) (5 20 1) simpleGrading (1 1 1)
hex (45 46 25 24 45 46 4 3) (5 20 1) simpleGrading (1 1 1)
hex (46 47 26 25 46 47 5 4) (5 20 1) simpleGrading (1 1 1)
hex (47 48 27 26 47 48 6 5) (5 20 1) simpleGrading (1 1 1)
hex (48 49 28 27 48 49 7 6) (5 20 1) simpleGrading (1 1 1)
hex (49 50 29 28 49 50 8 7) (5 20 1) simpleGrading (1 1 1)
hex (50 51 30 29 50 51 9 8) (5 20 1) simpleGrading (1 1 1)
hex (51 52 31 30 51 52 10 9) (5 20 1) simpleGrading (1 1 1)
hex (52 53 32 31 52 53 11 10) (5 20 1) simpleGrading (1 1 1)
hex (53 54 33 32 53 54 12 11) (5 20 1) simpleGrading (1 1 1)
hex (54 55 34 33 54 55 13 12) (5 20 1) simpleGrading (1 1 1)
hex (55 56 35 34 55 56 14 13) (5 20 1) simpleGrading (1 1 1)
hex (56 57 36 35 56 57 15 14) (5 20 1) simpleGrading (1 1 1)
hex (57 58 37 36 57 58 16 15) (5 20 1) simpleGrading (1 1 1)
hex (58 59 38 37 58 59 17 16) (5 20 1) simpleGrading (1 1 1)
hex (59 60 39 38 59 60 18 17) (5 20 1) simpleGrading (1 1 1)
hex (60 61 40 39 60 61 19 18) (5 20 1) simpleGrading (1 1 1)
hex (61 62 41 40 61 62 20 19) (5 20 1) simpleGrading (1 1 1)
);

edges
(
);

patches
(
patch inlet
(
(42 42 0 21)
)
patch outlet
(
(62 62 41 20)
)
wall wall
(
(0 1 22 21)
(1 2 23 22)
(2 3 24 23)
(3 4 25 24)
(4 5 26 25)
(5 6 27 26)
(6 7 28 27)
(7 8 29 28)
(8 9 30 29)
(9 10 31 30)
(10 11 32 31)
(11 12 33 32)
(12 13 34 33)
(13 14 35 34)
(14 15 36 35)
(15 16 37 36)
(16 17 38 37)
(17 18 39 38)
(18 19 40 39)
(19 20 41 40)
)
wedge front
(

(42 43 1 0)
(43 44 2 1)
(44 45 3 2)
(45 46 4 3)
(46 47 5 4)
(47 48 6 5)
(48 49 7 6)
(49 50 8 7)
(50 51 9 8)
(51 52 10 9)
(52 53 11 10)
(53 54 12 11)
(54 55 13 12)
(55 56 14 13)
(56 57 15 14)
(57 58 16 15)
(58 59 17 16)
(59 60 18 17)
(60 61 19 18)
(61 62 20 19)
)

wedge back

(

(21 22 43 42)
(22 23 44 43)
(23 24 45 44)
(24 25 46 45)
(25 26 47 46)
(26 27 48 47)
(27 28 49 48)
(28 29 50 49)
(29 30 51 50)
(30 31 52 51)
(31 32 53 52)
(32 33 54 53)
(33 34 55 54)
(34 35 56 55)
(35 36 57 56)
(36 37 58 57)
(37 38 59 58)
(38 39 60 59)
(39 40 61 60)
(40 41 62 61)
)

empty axis

(

(42 43 43 42)
(43 44 44 43)
(44 45 45 44)
(45 46 46 45)
(46 47 47 46)
(47 48 48 47)
(48 49 49 48)
(49 50 50 49)
(50 51 51 50)
(51 52 52 51)
(52 53 53 52)
(53 54 54 53)
(54 55 55 54)
(55 56 56 55)
(56 57 57 56)
(57 58 58 57)
(58 59 59 58)
(59 60 60 59)
(60 61 61 60)
(61 62 62 61)
)


);

mergePatchPairs
(
);

// ************************************************** *********************** //




this is a 2d axis-symmetry nozzle . The solver is rhoSonicFoam ,when I run the case this error appears:







Root : /home/msha/OpenFOAM/msha-1.3/run/tutorials/rhoSonicFoam
Case : nozzle
Nprocs : 1
Create time

Create mesh for time = 0

Reading thermodynamicProperties

Reading field p

Reading field T

Reading field U


Starting time loop

Time = 1e-05

Lookup interpolationScheme for interpolate(rho)
Lookup interpolationScheme for interpolate(rhoU)

Max Courant Number = 0.120569
Lookup divScheme for div(phiv,rho)
Lookup gradScheme for grad(rho)


--> FOAM FATAL ERROR :
request for surfaceScalarField phi from objectRegistry region0 failed
available objects of type surfaceScalarField are

4
(
weightingFactors
limiter
differenceFactors_
phiv
)


From function objectRegistry::lookupObject<type>(const word&) const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude/objectRegistryTempl ates.C at line 122.

FOAM aborting

Foam::error::printStack(Foam:stream&)
Foam::error::abort()
Foam::GeometricField<double,> const& Foam::objectRegistry::lookupObject<foam::geometric field<double,> >(Foam::word const&) const
Foam::totalPressureFvPatchScalarField::updateCoeff s()
Foam::GeometricField<double,>::GeometricBoundaryFi eld::updateCoeffs()
Foam::fvMatrix<double>::fvMatrix(Foam::GeometricFi eld<double,>&, Foam::dimensionSet const&)
Foam::fv::gaussConvectionScheme<double>::fvmDiv(Fo am::GeometricField<double,> const&, Foam::GeometricField<double,>&) const
Foam::tmp<foam::fvmatrix<double> > Foam::fvm::div<double>(Foam::GeometricField<double ,> const&, Foam::GeometricField<double,>&, Foam::word const&)
Foam::tmp<foam::fvmatrix<double> > Foam::fvm::div<double>(Foam::GeometricField<double ,> const&, Foam::GeometricField<double,>&)
rhoSonicFoam [0x8059060]
__libc_start_main
__gxx_personality_v0
Aborted



what can I do?
msha is offline   Reply With Quote

Old   October 15, 2007, 12:06
Default Isn't any one for help in this
  #2
Member
 
Mojtaba Shahmohammadian
Join Date: Mar 2009
Posts: 73
Rep Power: 7
msha is on a distinguished road
Isn't any one for help in this subject

Please help any way.

THANK YOU ALL

MSHA
msha is offline   Reply With Quote

Old   November 9, 2007, 04:07
Default I have encountered the same pr
  #3
New Member
 
N S Prasad
Join Date: Mar 2009
Posts: 15
Rep Power: 7
nsp82 is on a distinguished road
I have encountered the same problem of

--> FOAM FATAL ERROR :
request for surfaceScalarField phi from objectRegistry region0 failed
available objects of type surfaceScalarField are

4
(
weightingFactors
differenceFactors_
phiv
vanLeerLimiter(rhoU)
)

for a 2d flow over an afoil with rhoSonicFoam

Can some one point out my mistakes ...?

Regards,
nsp82 is offline   Reply With Quote

Old   September 9, 2009, 06:19
Default
  #4
New Member
 
Join Date: Sep 2009
Posts: 4
Rep Power: 7
sandrak is on a distinguished road
I know this thread is old, but I'm encountering the same problem with OpenFoam Version 1.6. It's the rhoSonicFoam as well and it happens when calling
fvm::div(phiv, rho);

The error message is the same, I'll post it anyway:

request for surfaceScalarField phi from objectRegistry region0 failed
available objects of type surfaceScalarField are

4
(
phiv
limitedLinearLimiter(rho)
differenceFactors_
weightingFactors
)

I looked through all my files. There is never a phi used, only phiv. It still works well on the shockTube tutorial, but not on my case and I don't know, what I'm doing wrong.
sandrak is offline   Reply With Quote

Old   June 20, 2010, 06:57
Default
  #5
New Member
 
Yu
Join Date: May 2010
Location: Cambridge, MA
Posts: 11
Rep Power: 6
Ruehri is on a distinguished road
Although this thread may seem a little bit old I think it might help if I share my thoughts on this. I found an error in my BC when using waveTransmissive, which uses the field phi, whereas rhoSonicFoam uses phiv.

A simple workaround was for me to simply recompile the solver for using phi (changing every phiv to phi). It might be possible to change waveTransmissive to use phiv, but I didn't try that.
Ruehri is offline   Reply With Quote

Old   February 28, 2011, 08:41
Default LaplacianFoam
  #6
Member
 
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 5
sixwp is on a distinguished road
As none of the members above could get an answer and as I am pretty much in the same situation, I'm digging out (don't know if it's valuable in English ^^) this thread.

I have trouble with a laplacianFoam simulation where I got this Error message when running:
Code:
--> FOAM FATAL ERROR: 

    request for surfaceScalarField phi from objectRegistry region0 failed
    available objects of type surfaceScalarField are

4
(
DT
differenceFactors_
weightingFactors
(DT*magSf)
)


    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /usr/local/OpenFOAM/OpenFOAM-1.7.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 139.
Maybe people from previous posts have found out where the problem is located

Thank you for your time

[Edit]: I already tried to replace in fvSchemes "phi" by "DT" (DT defined in transportProperties) but still

Last edited by sixwp; February 28, 2011 at 10:17.
sixwp is offline   Reply With Quote

Old   October 9, 2013, 22:37
Default
  #7
Senior Member
 
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 7
ziad is on a distinguished road
Three year old thread but hey, it doesn't hurt to post a fix, right?

Create a phi initial and boundary conditions file in folder 0/ and you're set. I haven't figured out why bubbleFoam doesn't create phi automatically as it is supposed to and does in most cases but if you create the file for it everything runs smoothly.
ziad is offline   Reply With Quote

Old   January 20, 2014, 06:00
Default I have encountered the same problem, but no posted advice works
  #8
New Member
 
Steven
Join Date: Dec 2013
Location: Perth
Posts: 15
Rep Power: 3
crst15 is on a distinguished road
Hi,

I got a similar problem when trying to run potentialFoam. I have tried to apply Ziad suggestion by creating phi initial and boundary conditions file in folder 0/. However, it doesn't work and the terminal window displays the following:


--> FOAM FATAL ERROR:

request for surfaceScalarField phiHbyA from objectRegistry region0 failed
available objects of type surfaceScalarField are

3
(
(1*magSf)
phi
1
)


From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 164.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2 Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const& Foam:bjectRegistry::lookupObject<Foam::Geometric Field<double, Foam::fvsPatchField, Foam::surfaceMesh> >(Foam::word const&) const in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#3 Foam::fixedFluxPressureFvPatchScalarField::updateC oeffs() in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#4 at gaussLaplacianSchemes.C:0
#5 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricFi eld<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#6 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#7
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
#8
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
#9
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
#10 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#11
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
Aborted (core dumped)


As in my case the error message says "phiHbyA" rather than "phi", I also made a file for "phiHbyA" in 0/ folder. But it still can't work and the error message I receive is always the same.

Any idea on how to fix this? I'll appreciate that so much.


Cheers
crst15 is offline   Reply With Quote

Old   January 24, 2014, 05:14
Default solution
  #9
Member
 
Ilya
Join Date: Dec 2011
Location: Russia
Posts: 65
Blog Entries: 35
Rep Power: 5
skeptik is on a distinguished road
In case of airfoil, rhoSonicFoam doesn't support BC such as waveTransmissive. It includes manipulation with phi field.

Good luck.
__________________
practice makes perfect
skeptik is offline   Reply With Quote

Old   March 1, 2014, 17:37
Default
  #10
Senior Member
 
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 7
ziad is on a distinguished road
Quote:
Originally Posted by crst15 View Post
Hi,

I got a similar problem when trying to run potentialFoam. I have tried to apply Ziad suggestion by creating phi initial and boundary conditions file in folder 0/. However, it doesn't work and the terminal window displays the following:


--> FOAM FATAL ERROR:

request for surfaceScalarField phiHbyA from objectRegistry region0 failed
available objects of type surfaceScalarField are

3
(
(1*magSf)
phi
1
)


From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 164.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2 Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const& Foam:bjectRegistry::lookupObject<Foam::Geometric Field<double, Foam::fvsPatchField, Foam::surfaceMesh> >(Foam::word const&) const in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#3 Foam::fixedFluxPressureFvPatchScalarField::updateC oeffs() in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#4 at gaussLaplacianSchemes.C:0
#5 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricFi eld<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#6 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam222/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#7
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
#8
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
#9
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
#10 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#11
in "/opt/openfoam222/platforms/linuxGccDPOpt/bin/potentialFoam"
Aborted (core dumped)


As in my case the error message says "phiHbyA" rather than "phi", I also made a file for "phiHbyA" in 0/ folder. But it still can't work and the error message I receive is always the same.

Any idea on how to fix this? I'll appreciate that so much.


Cheers
phiHbyA is computed by the code during the solution procedure. It is not a variable like U or p or phi. Not familiar with potentialFoam but can you post more info? What are you trying to simulate?
ziad is offline   Reply With Quote

Old   March 1, 2014, 17:44
Default
  #11
Senior Member
 
Ziad Boutanios
Join Date: Mar 2009
Location: Montréal, Canada
Posts: 113
Rep Power: 7
ziad is on a distinguished road
Quote:
Originally Posted by ziad View Post
Three year old thread but hey, it doesn't hurt to post a fix, right?

Create a phi initial and boundary conditions file in folder 0/ and you're set. I haven't figured out why bubbleFoam doesn't create phi automatically as it is supposed to and does in most cases but if you create the file for it everything runs smoothly.
The proper fix for this problem in bubbleFoam (and twoPhaseEulerFoam by proxy) is to make sure you have the following two lines in createFields.H between the part where you create your velocity fields and the part where you use phi for the first time.

Code:
    #include "createPhia.H"
    #include "createPhib.H"
In these header files phi will be computed based on U or read if already created from a previous iteration. Of course you'll also need these two header files as well. Single phase codes will probably use something like "createPhi.H". After this no need to create phi files in the time folders.
ziad is offline   Reply With Quote

Old   March 21, 2014, 05:35
Default
  #12
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 469
Rep Power: 12
vasava will become famous soon enough
I have openfoam 2.1.x installed on windows. My cases with single domains are running fine but when I run some case with multiple domains (e.g. conjugate heat transfer cases) I get the following error.

Code:
--> FOAM FATAL ERROR:

    request for objectRegistry topAir from objectRegistry cavity failed
    available objects of type objectRegistry are

3
(
innerfluid
outerfluid
pipe
)
Any clue or advise?
vasava 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
Visualisation of a surfaceScalarField with paraview sinusmontis OpenFOAM Paraview & paraFoam 3 July 9, 2010 05:09
Global variables or How to get a vector into an objectRegistry maddhi OpenFOAM Running, Solving & CFD 0 August 19, 2008 08:08
Register pointer to class in mesh objectRegistry kar OpenFOAM 1 June 3, 2008 05:57
SurfaceScalarField ghf in interFoam how does it look like mcchouffe OpenFOAM Running, Solving & CFD 11 July 3, 2007 11:33


All times are GMT -4. The time now is 22:30.