CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Community Contributions

[IHFOAM] IHFOAM patch problem IH_Waves_InletVelocity

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

Like Tree1Likes
  • 1 Post By IHFOAM Team

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 22, 2018, 10:56
Default IHFOAM patch problem IH_Waves_InletVelocity
  #1
New Member
 
Jorge Molines
Join Date: Oct 2012
Posts: 11
Rep Power: 9
jormollo is on a distinguished road
Hi!
I have downloaded and installed OpenFoam and Ihfoam and I have a problem with the patchField type IH_Waves_InletVelocity. My versions are Ubuntu 16.04, OpenFoam 1706 and ihFoam 1706 downloaded from http://ihfoam.ihcantabria.com/source-download/.

Both installations of OpenFoam and ihFoam finished succesfully. I am running an example of a breakwater with porous media that I also downloaded from the web prepared for OF 230_240 and I modified some patches and the mode of the operating solver from PIMPLE to PISO. However, I do not know how to solve the new problem . Thanks in advance for any advise,
Jorge.


jorge@jorge-VirtualBox:~/OpenFOAM/OpenFOAM-v1706/tutorials/tutorials/OF230_240/breakwater$ ihFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v1706 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : v1706
Arch : "LSB;label=32;scalar=64"
Exec : ihFoam
Date : Feb 22 2018
Time : 16:49:22
Host : "jorge-VirtualBox"
PID : 26351
Case : /home/jorge/OpenFOAM/OpenFOAM-v1706/tutorials/tutorials/OF230_240/breakwater
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PIMPLE: Operating solver in PISO mode

Reading field porosityIndex

Porosity activated
Reading porosity variables

Number of materials: 4
a = 4(0 50 50 50)
b = 4(0 1.2 2 0.6)
c = 4(0 0.34 0.34 0.34)
D50 = 4(1 0.01 0.035 0.12)
porosity = 4(1 0.49 0.493 0.5)
Transient formulation is 0

Creating fields: porosity, aPor, bPor, cPor and D50Por

Reading field p_rgh

Reading field U



--> FOAM FATAL IO ERROR:
Unknown patchField type IH_Waves_InletVelocity for patch type patch

Valid patchField types are :

81
(
SRFFreestreamVelocity
SRFVelocity
SRFWallVelocity
activeBaffleVelocity
activePressureForceBaffleVelocity
advective
atmBoundaryLayerInletVelocity
calculated
codedFixedValue
codedMixed
cyclic
cyclicACMI
cyclicAMI
cyclicSlip
cylindricalInletVelocity
directionMixed
empty
extrapolatedCalculated
fixedGradient
fixedInternalValue
fixedJump
fixedJumpAMI
fixedMean
fixedNormalInletOutletVelocity
fixedNormalSlip
fixedProfile
fixedShearStress
fixedValue
flowRateInletVelocity
fluxCorrectedVelocity
freestream
inletOutlet
interstitialInletVelocity
kqRWallFunction
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mappedFlowRate
mappedVelocityFlux
mixed
movingWallVelocity
noSlip
nonuniformTransformCyclic
outletInlet
outletMappedUniformInlet
outletPhaseMeanVelocity
partialSlip
pressureDirectedInletOutletVelocity
pressureDirectedInletVelocity
pressureInletOutletParSlipVelocity
pressureInletOutletVelocity
pressureInletUniformVelocity
pressureInletVelocity
pressureNormalInletOutletVelocity
pressurePIDControlInletVelocity
processor
processorCyclic
rotatingPressureInletOutletVelocity
rotatingWallVelocity
sliced
slip
supersonicFreestream
surfaceNormalFixedValue
swirlFlowRateInletVelocity
symmetry
symmetryPlane
timeVaryingMappedFixedValue
translatingWallVelocity
turbulentDFSEMInlet
turbulentInlet
uniformFixedGradient
uniformFixedValue
uniformInletOutlet
uniformJump
uniformJumpAMI
variableHeightFlowRateInletVelocity
waveTransmissive
waveVelocity
wedge
zeroGradient
)


file: /home/jorge/OpenFOAM/OpenFOAM-v1706/tutorials/tutorials/OF230_240/breakwater/0/U.boundaryField.inlet from line 26 to line 28.

From function static Foam::tmp<Foam::fvPatchField<Type> > Foam::fvPatchField<Type>::New(const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = Foam::Vector<double>]
in file /home/jorge/OpenFOAM/OpenFOAM-v1706/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 134.

FOAM exiting
jormollo is offline   Reply With Quote

Old   February 26, 2018, 07:23
Default
  #2
Member
 
IHFOAM Team's Avatar
 
IHFOAM The Environmental Hydraulics Institute "IHCantabria"
Join Date: Sep 2017
Location: Santander (Spain)
Posts: 72
Rep Power: 4
IHFOAM Team is on a distinguished road
Hi Jorge,

I just add here the answer I already sent you in case anyone might need it:

IHFOAM boundary conditions are now implemented and released within OpenFOAM (since version v1612+) thanks to an agreement between ESI & IH-Cantabria.
(https://www.openfoam.com/releases/op...ave-generation)

You can find several tutorials in:
~/OpenFOAM-XXX/tutorials/multiphase/interFoam/laminar/waveExampleXX

If you want to use the old ihFOAM tutorials, you must just change and adapt the names of the BC's.

Best Regards,
IHFOAM Team.
jormollo likes this.
__________________
http://ihfoam.ihcantabria.com/
IHFOAM Team is offline   Reply With Quote

Old   February 28, 2018, 10:07
Default
  #3
New Member
 
Jorge Molines
Join Date: Oct 2012
Posts: 11
Rep Power: 9
jormollo is on a distinguished road
Thanks for your answer!
Regards,
Jorge.
jormollo is offline   Reply With Quote

Old   October 22, 2018, 23:26
Default IHFOAM patch problem IH_Waves_InletVelocity
  #4
New Member
 
Luo_Bingjun
Join Date: Oct 2018
Location: CHINA
Posts: 14
Rep Power: 3
Robin86 is on a distinguished road
Hello!I meet the same problem as you. The error "Unkown IHFOAM patch problem IH_Waves_InletVelocity" happens. My version is of v1806. How can I solve this problem. Thank you!
Robin86 is offline   Reply With Quote

Old   October 23, 2018, 03:08
Default
  #5
Member
 
IHFOAM Team's Avatar
 
IHFOAM The Environmental Hydraulics Institute "IHCantabria"
Join Date: Sep 2017
Location: Santander (Spain)
Posts: 72
Rep Power: 4
IHFOAM Team is on a distinguished road
Hi Robin86

Quote:
Originally Posted by Robin86 View Post
How can I solve this problem.?
Please, canyou tell me which version of IHFoam have you tried to used with OpenFOAM-v1806?

Regards,
IHFOAM Team
__________________
http://ihfoam.ihcantabria.com/
IHFOAM Team is offline   Reply With Quote

Old   October 23, 2018, 03:42
Default
  #6
New Member
 
Luo_Bingjun
Join Date: Oct 2018
Location: CHINA
Posts: 14
Rep Power: 3
Robin86 is on a distinguished road
I use OpenFoam v1806 and ihFoam v1806.
Robin86 is offline   Reply With Quote

Old   October 25, 2018, 21:52
Default
  #7
New Member
 
Luo_Bingjun
Join Date: Oct 2018
Location: CHINA
Posts: 14
Rep Power: 3
Robin86 is on a distinguished road
I use OpenFOAM 1806 to run the IHFOAM old version tutorials. The same problem "Unknown patchField type IH_Waves_InletVelocity" appears, just like the above problem. How can I solve it? Should I change the old version tutorials BC's? Which BC needs to be changed and how to change it? I am new OpenFOAM user. Thank you!
Robin86 is offline   Reply With Quote

Old   November 6, 2018, 09:32
Default
  #8
Member
 
IHFOAM Team's Avatar
 
IHFOAM The Environmental Hydraulics Institute "IHCantabria"
Join Date: Sep 2017
Location: Santander (Spain)
Posts: 72
Rep Power: 4
IHFOAM Team is on a distinguished road
Hi Robin86,

Quote:
Originally Posted by Robin86 View Post
I use OpenFOAM 1806 to run the IHFOAM old version tutorials.
There is no point in using the old version of IHFOAM with OpenFOAM-v1806.
Why? Because, IHFOAM boundary conditions are already implemented within OpenFOAM-v1806 in a more accurate and faster way than the first release.

Can I ask you why do you want to do this strange thing?

Best Regrards,
IHFOAM Team
__________________
http://ihfoam.ihcantabria.com/
IHFOAM Team is offline   Reply With Quote

Old   November 6, 2018, 20:34
Default
  #9
New Member
 
Luo_Bingjun
Join Date: Oct 2018
Location: CHINA
Posts: 14
Rep Power: 3
Robin86 is on a distinguished road
Actually, I want to run the old tutorials to understand how to monitor free surface of wave. The old tutorials realize this while the tutorials in OpenFOAM 1806 do not. How to draw the curve of wave elevation and time in specified location? Thank you!
Robin86 is offline   Reply With Quote

Old   November 7, 2018, 02:49
Default
  #10
Member
 
IHFOAM Team's Avatar
 
IHFOAM The Environmental Hydraulics Institute "IHCantabria"
Join Date: Sep 2017
Location: Santander (Spain)
Posts: 72
Rep Power: 4
IHFOAM Team is on a distinguished road
Hi Robin86,

Quote:
The old tutorials realize this while the tutorials in OpenFOAM 1806 do not
We have added some monitoring tools in the controlDict (free surface sensors) to be able to track and draw the free surface elevation in time in a specific location.

Please, take a look to the end of the controlDict:

Code:
functions
{
    line
    {
        type            sets;
        libs            ("libsampling.so");
        enabled         true;
        writeControl    writeTime;
        writeInterval   1;

        interpolationScheme cellPoint;
        setFormat       raw;
        sets
        (
            line1
            {
                type    uniform;
                axis    distance;
                start   ( 1.0 0.02 0.0 );
                end     ( 1.0 0.02 0.55 );
                nPoints 1001;
            }
            line2
            {
                type    uniform;
                axis    distance;
                start   ( 2.0 0.02 0.0 );
                end     ( 2.0 0.02 0.55 );
                nPoints 1001;
            }
            line3
            {
                type    uniform;
                axis    distance;
                start   ( 3.0 0.02 0.0 );
                end     ( 3.0 0.02 0.55 );
                nPoints 1001;
            }
            line4
            {
                type    uniform;
                axis    distance;
                start   ( 5.0 0.02 0.0 );
                end     ( 5.0 0.02 0.55 );
                nPoints 1001;
            }
            line5
            {
                type    uniform;
                axis    distance;
                start   ( 7.5 0.02 0.0 );
                end     ( 7.5 0.02 0.55 );
                nPoints 1001;
            }

            line6
            {
                type    uniform;
                axis    distance;
                start   ( 10.0 0.02 0.0 );
                end     ( 10.0 0.02 0.55 );
                nPoints 1001;
            }
            line7
            {
                type    uniform;
                axis    distance;
                start   ( 12.0 0.005 0.0 );
                end     ( 12.0 0.005 0.55 );
                nPoints 1001;
            }
            line8
            {
                type    uniform;
                axis    distance;
                start   ( 14.0 0.005 0.0 );
                end     ( 14.0 0.005 0.55 );
                nPoints 1001;
            }
        );

        fixedLocations  false;
        fields
        (
            U alpha.water
        );
    }
}

Best Regards,
IHFOAM Team
__________________
http://ihfoam.ihcantabria.com/
IHFOAM Team is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with cyclic boundaries in Openfoam 1.5 fs82 OpenFOAM 36 January 7, 2015 00:31
[Gmsh] Single volume Mesh gmsh PeteH OpenFOAM Meshing & Mesh Conversion 9 August 6, 2013 08:54
Cyclic Boundary Condition Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Running, Solving & CFD 36 July 2, 2012 12:23
[Gmsh] Import gmsh msh to Foam adorean OpenFOAM Meshing & Mesh Conversion 24 April 27, 2005 08:19
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 08:33.