[Michael@UW]

Dear FOAMers,

I was wondering if timeVaryingMappedFixedValue + pointDisplacement + parallel does not work in OpenFOAM v1906 or I did something wrong with my case.

I try to modify pitzDailyExptInlet case to test the moving boundary.
I add the following files
1. 0/pointDisplacement,
2. constant/boundaryData/inlet/0/pointDisplacement.
3. constant/dynamicMeshDict where displacementLaplacian is used.
The fvSolution file is also edited accordingly.

Then run in parallel.
mpirun -np 4 moveDynamicMesh -parallel

The error shows points file does not exist. But it is there, and it runs without any error in serial.

In addition, the original case without any modification runs well in parallel.

/////// Message Excerpt===========
Create mesh for time = 0

Selecting dynamicFvMesh dynamicMotionSolverFvMesh
Selecting motion solver: displacementLaplacian
[1]
[1]
[1] --> FOAM FATAL IO ERROR:
[1] file "../constant/boundaryData/inlet/points" does not exist
[1]
[1] file: ../constant/boundaryData/inlet/points at line 1.
[1]
[1] From function Foam::IFstream& Foam::IFstream:perator()() const
[1] in file db/IOstreams/Fstreams/IFstream.C at line 221.
[1]
FOAM parallel run exiting

Someone can confirm this? Any hints will be appreciated!

Michael

[HPE]

Hi,

- `points` file containing three-dimensional position data is required in order to map the corresponding boundary information onto the inlet patch.
- please search for an example within tutorials where `points` file is used in association with `timeVar*` boundary condition.

Hope this helps a bit.

[Michael@UW]

Originally Posted by HPE

Hi,

- `points` file containing three-dimensional position data is required in order to map the corresponding boundary information onto the inlet patch.
- please search for an example within tutorials where `points` file is used in association with `timeVar*` boundary condition.

Hope this helps a bit.

Hi HPE,

Thank you for your reply.
I am pretty sure 'point' file is there with correct formats. As the case is copied from the tutorial and it runs well in serial.

Strangely, I did nothing but switch to OpenFOAM 6, it runs without any issue in parallel. I was just wondering if it is a bug of OpenFOAM v1906 or something else was wrong with my environment.

[Michael@UW]

I attached my case. It would be appreciated if you could have a quick test.

[HPE]

Hi,

I will see what I can do - I will test your case. Please do not hesitate to poke me if I don't get back to it (sometimes, I lose the track of the posts that I promised to provide an answer).

[Michael@UW]

Originally Posted by HPE

Hi,

I will see what I can do - I will test your case. Please do not hesitate to poke me if I don't get back to it (sometimes, I lose the track of the posts that I promised to provide an answer).

Thank you for being willing to test my case! Looking forward to hearing from you.

By the way, in timeVaryingMappedFixedValue, is it possible to repeat the cycle like timeVaryingUniformFixedValue by setting outOfBounds repeat?

[HPE]

sorry, what cycle? (might be my IQ dropped to a single-digit ).

[Michael@UW]

Originally Posted by HPE

sorry, what cycle? (might be my IQ dropped to a single-digit ).

Sorry for the confusion. I want to run the simulation up to 10s but only provide the data up to 5s, because the boundary condition at inlet repeats during 6s~10s.
So I want to reuse the data in:
constant/boundaryData/inlet/0
constant/boundaryData/inlet/1
constant/boundaryData/inlet/2
...
constant/boundaryData/inlet/5

In short, I do not want to provide all the data for the second cycle.

Hopefully, it is clearer to state my problem.

[Michael@UW]

Originally Posted by HPE

Hi,

I will see what I can do - I will test your case. Please do not hesitate to poke me if I don't get back to it (sometimes, I lose the track of the posts that I promised to provide an answer).

Hi Dear HPE,
Just wondering if you have tested the case or any findings.

Regards,
Michael

[HPE]

I'm very sorry that I still couldn't touch it. Yet it is on my list.

[Michael@UW]

Originally Posted by HPE

I'm very sorry that I still couldn't touch it. Yet it is on my list.

No problem. I appreciate your time.

[Michael@UW]

Originally Posted by HPE

I'm very sorry that I still couldn't touch it. Yet it is on my list.

Dear HPE,

Did you have a chance to run the test case? I encountered this problem again. After upgrading to OpenFOAM v2006, I applied timeVaryingMappedFixedValue type on my moving wall (pointMotionU). It runs well in serial but gives an error regarding matchPoint. I think it is quite the same problem.

In pointMotionU

    wall
    {
        type            timeVaryingMappedFixedValue;
        mapMethod       nearest;
        setAverage      off;
        offset          ( 0 0 0 );
        points          "points";
    }

The output (only in parallel):

[1] Cannot find point in pts1 matching point 284 coord:(0 0 0) in pts0 when using tolerance 1e+15
[0] Cannot find point in pts1 matching point 238 coord:(-0.00098 0 0) in pts0 when using tolerance 1e+15
[0] Searching started from:0 in pts1
[1] Searching started from:0 in pts1
[1] Cannot find point in pts1 matching point 286 coord:(0 1.313131313e-05 0) in pts0 when using tolerance 1e+15
....

And error message:

[0] --> FOAM FATAL ERROR: 
[0] Did not find a corresponding sourcePoint for every face centre
[0] 
[0]     From void Foam::pointToPointPlanarInterpolation::calcWeights(const pointField&, const pointField&)
[0]     in file triSurface/triSurfaceTools/pointToPointPlanarInterpolation.C at line 159.
[0] 
FOAM parallel run exiting
[0] 
[1] 
[1] 
[1] --> FOAM FATAL ERROR: 
[1] Did not find a corresponding sourcePoint for every face centre
[1] 
[1]     From void Foam::pointToPointPlanarInterpolation::calcWeights(const pointField&, const pointField&)
[1]     in file triSurface/triSurfaceTools/pointToPointPlanarInterpolation.C at line 159.
[1] 
FOAM parallel run exiting
[1] 
[cfd-me:24292] 1 more process has sent help message help-mpi-api.txt / mpi-abort
[cfd-me:24292] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages

All the points on the boundary with timeVaryingMappedFixedValue type are not matched

I'm sure all the data are correct which is confirmed by running in serial.

I tested the same case in OpenFOAM-7; there is no problem. But I need to use overset in ESI version.


Thank you!
Michael

[Michael@UW]

The problem has been (kind of) solved by modifying some codes in the source file:

/home/michael/OpenFOAM/OpenFOAM-v2006/src/fvMotionSolver/pointPatchFields/derived/timeVaryingMappedFixedValue/timeVaryingMappedFixedValuePointPatchField.C

1. time.caseConstant() -> time.constant(). The former returns ../constant and the latter gives constant

        const fileName samplePointsFile
        (
           //time.caseConstant()
           time.constant()
           /"boundaryData"
           /this->patch().name()
           /"points"
        );

2. It seems rawIOField is not initialized correctly, so I use IFstream read the data file.

        // IOobject io
        // (
        //     samplePointsFile,   // absolute path
        //     time,
        //     IOobject::MUST_READ,
        //     IOobject::NO_WRITE,
        //     false,              // no need to register
        //     true                // is global object (currently not used)
        // );

        // Read data
        // const rawIOField<point> samplePoints(io, false);


        pointField samplePoints((IFstream(samplePointsFile)()));

3. But this will cause vals.average() being not declared, because vals is not a rawIOField any more. So I copied and included the files AverageField.H and AverageField.C from OpenFOAM-7.

//#include "rawIOField.H"  // deleted

//# Copied from OpenFOAM-7
#include "AverageField.H"
#include "IFstream.H"

Then replaced the codes for "setAverage_" condition.

// replaced 
            // IOobject io
            // (
            //     valsFile,   // absolute path
            //     time,
            //     IOobject::MUST_READ,
            //     IOobject::NO_WRITE,
            //     false,              // no need to register
            //     true                // is global object (currently not used)
            // );

            // const rawIOField<Type> vals(io, setAverage_);

            // if (setAverage_)
            // {
            //     startAverage_ = vals.average();
            // }
//////////////////////////////////// 
// with

            Field<Type> vals;

            if (setAverage_)
            {
                AverageField<Type> avals((IFstream(valsFile)()));
                vals = avals;
                startAverage_ = avals.average();
            }
            else
            {
                IFstream(valsFile)() >> vals;
            }
//////////////////////////////////// End of Added

Otherwise, it will give the error:
"Number of values (0) differs from the number of points ( ) in file ...
when the data file has the format (uniform):

720{(0 0 0)}.

This file is generated by OpenFOAM API.

4. wmake, then it runs.

Hope someone can confirm this solution or propose a better one.