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

Strange issue with OF v1906 and pointDisplacement

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 8, 2020, 23:42
Default Strange issue with OF v1906 and pointDisplacement
  #1
Senior Member
 
TWB
Join Date: Mar 2009
Posts: 357
Rep Power: 16
quarkz is on a distinguished road
Hi,

I tried to run decomposePar and renumberMesh (parallel) before running the simulation as usual in OF v1906

However, when I run 'mpirun pimpleFoam -parallel', I got the error:

[3] --> FOAM FATAL IO ERROR:
[3] [0]
Essential entry 'value' missing
[3]
[3] file: /scratch/users/nus/tsltaywb/OpenFOAM/naca0012_naca0008_200x51_test_err/processor3/0/pointDisplacement.boundaryField.flap_wall
[3]
[3] From function Foam::valuePointPatchField<Type>::valuePointPatchF ield(const Foam:ointPatch&, const Foam:imensionedField<Type, Foam:ointMesh>&, const Foam::dictionary&, bool) [with Type = Foam::Vector<double>]
[3] in file /home/project/11000324/OpenFOAM/OpenFOAM-v1906/src/OpenFOAM/lnInclude/valuePointPatchField.C at line [0]

On inspection, I found that the entry:

value uniform (0 0 0);

is removed in pointDisplacement

The orginal pointDisplacement is:

boundaryField
{

flap_wall
{
type angularOscillatingDisplacement;
value uniform (0 0 0);
axis (0 0 1);
origin (1.02 0.0 0.02);
angle0 0;
amplitude 0.358; //units of rad
omega 6.28; //units of rad/s

}

I found that either running decomposePar or renumberMesh will remove the value statement, preventing pimpleFoam from working.

Even running in serial with renumberMesh will give the error. v1812 seems to be working though.

Does anyone has the same experience?

Thanks.
quarkz is offline   Reply With Quote

Old   May 9, 2020, 06:13
Default
  #2
HPE
Senior Member
 
HPE's Avatar
 
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 932
Rep Power: 11
HPE is on a distinguished road
Hi,

Is there any tutorial you can provide or indicate that we can try to reproduce the error?

Thanks
HPE is offline   Reply With Quote

Old   September 16, 2020, 03:56
Default
  #3
Senior Member
 
TWB
Join Date: Mar 2009
Posts: 357
Rep Power: 16
quarkz is on a distinguished road
Hi,

Sorry for the delay. I have shared a link to the error case. It is a naca0012 airfoil with a naca008 flap behind. The flap is supposed to rotate.

Error appears with v1906.

https://app.box.com/s/s968xxa6pyfum8esjjs50ttfpr3h7a7o

I tested v2006 and it seems to have been resolved.
quarkz is offline   Reply With Quote

Old   October 24, 2020, 05:32
Default
  #4
New Member
 
Ali
Join Date: May 2016
Location: Sydney, Australia
Posts: 15
Rep Power: 8
AliVali is on a distinguished road
Hi quarkz.



I have a similar problem. I can run the model with single cpu but get the following error and using decomposerPar.
Time = 0
Selecting solid-body motion function tabulated6DoFMotion

Processor 0: field transfer


--> FOAM FATAL IO ERROR:
keyword solidBodyMotionFunction is undefined in dictionary "/mnt/e/DHI/Work/surfLake/New_CFD/floatingObject/test_rigidBody/0/pointDisplacement.boundaryField.floatingObject.tab ulated6DoFMotionCoeffs"

file: /mnt/e/DHI/Work/surfLake/New_CFD/floatingObject/test_rigidBody/0/pointDisplacement.boundaryField.floatingObject.tab ulated6DoFMotionCoeffs from line 43 to line 45.

From function const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, bool, bool) const
in file db/dictionary/dictionary.C at line 573.

FOAM exiting


in pointDisplacement

floatingObject
{
type solidBodyMotionDisplacement;
solidBodyMotionFunction tabulated6DoFMotion;
tabulated6DoFMotionCoeffs
{
CofG (0.5 0.5 0.5);
// timeDataFileName "<constant>/6DoF.dat";
timeDataFileName "$FOAM_CASE/constant/6DoF.dat";
}
}





and dynamicMeshDict is as follows


FoamFile
{
version 2.0;
format ascii;
class dictionary;
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh dynamicMotionSolverFvMesh;
motionSolverLibs (fvMotionSolvers);

solver displacementLaplacian;

displacementLaplacianCoeffs
{
diffusivity inverseDistance (floatingObject);
// diffusivity quadratic inverseDistance (floatingObject);
}





I checked with of2006 and openFOAm7, get the similar error.
Any help would be highly appreciated.


Ali
AliVali is offline   Reply With Quote

Old   September 16, 2021, 18:26
Default
  #5
New Member
 
William Lambert
Join Date: Dec 2020
Posts: 1
Rep Power: 0
wblambert is on a distinguished road
Hi AliVali,
I am getting this exact error. Did you find a solution to this problem?

Thanks
wblambert is offline   Reply With Quote

Old   June 29, 2022, 09:08
Default
  #6
New Member
 
Cristóbal
Join Date: Jan 2022
Location: Sweden
Posts: 6
Rep Power: 2
cibanez is on a distinguished road
Hi,

I'm also getting the same error as AliVali, but with oscillatingRotatingMotion instead. Does anyone know the cause or have a fix for it?

/Cristóbal
cibanez is offline   Reply With Quote

Old   June 29, 2022, 12:17
Default
  #7
Senior Member
 
TWB
Join Date: Mar 2009
Posts: 357
Rep Power: 16
quarkz is on a distinguished road
Hi all, I suggest getting an example from the tutorials which is similar to your problem. Make sure it's working 1st. Then replace it with your mesh and some other impt parameters step by step. Testing along the way. Somehow I think it worked for me.
quarkz is offline   Reply With Quote

Old   June 30, 2022, 10:04
Default
  #8
New Member
 
Cristóbal
Join Date: Jan 2022
Location: Sweden
Posts: 6
Rep Power: 2
cibanez is on a distinguished road
Hi,

I was able to decompose that pointDisplacement field. As said before the case was running in serial but I could not get it to decompose.

The following boundary condition for pointDisplacement runs in serial but does not decompose the field:

Code:
wing
    {
        type        solidBodyMotionDisplacement;
        solidBodyMotionFunction oscillatingRotatingMotion;
        oscillatingRotatingMotionCoeffs
        {
           origin      (0 0.1 0);
           axis        (1 0 0);
           omega       50;          // rad/s, 1rad/s=9.5rpm
           amplitude   (0.15 0 0);    // max amplitude (degrees)
        }
    }
The fix for it is to include solidBodyMotionFunction oscillatingRotatingMotion inside oscillatingRotatingMotionCoeffs, which is a rather strange way of writting the coefficients.

Code:
wing
    {
        type        solidBodyMotionDisplacement;
        solidBodyMotionFunction oscillatingRotatingMotion;
        oscillatingRotatingMotionCoeffs
        {
           solidBodyMotionFunction oscillatingRotatingMotion;
           origin      (0 0.1 0);
           axis        (1 0 0);
           omega       50;          // rad/s, 1rad/s=9.5rpm
           amplitude   (0.15 0 0);    // max amplitude (degrees)
        }
    }
I think this might be a bug as the same error can be replicated in the tutorial case "box2D_moveDynamicMesh" when trying to decompose it.

/C
cibanez is offline   Reply With Quote

Old   July 14, 2022, 11:38
Default Bug reported and fixed
  #9
New Member
 
Cristóbal
Join Date: Jan 2022
Location: Sweden
Posts: 6
Rep Power: 2
cibanez is on a distinguished road
Hi,

This bug has been reported and recently closed.

Here you can find the closed ticket. https://develop.openfoam.com/Develop.../-/issues/2526
And here you can find the commit with the changes made to Foam::solidBodyMotionFunction::solidBodyMotionFunc tion https://develop.openfoam.com/Develop...bd61c1c1d93c65

/C
cibanez is offline   Reply With Quote

Old   August 12, 2022, 02:28
Default
  #10
New Member
 
Ali
Join Date: May 2016
Location: Sydney, Australia
Posts: 15
Rep Power: 8
AliVali is on a distinguished road
Quote:
Originally Posted by wblambert View Post
Hi AliVali,
I am getting this exact error. Did you find a solution to this problem?

Thanks

Hi William,



No I couldn't solve it. Unfortunately in OF2112 also fails. My workaround is to decompose it using OF/8, then run it with OF/2006. I know this is a silly solution, but it works most the times. It sounds there is solution at



https://develop.openfoam.com/Develop...bd61c1c1d93c65


I haven't checked it, yet
AliVali 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



All times are GMT -4. The time now is 19:25.