[syuico]

Hi all and dear Foamers,

I want to read the subdict "initialPoints" in the boundaryFieid of pointVectorField "pointDisplacement".

In sixDoFRigidBodyDisplacementPointPatchVectorField.C , it is read as

if (dict.found("initialPoints"))
{
    initialPoints_ = vectorField("initialPoints", dict , p.size());
}

I output the name of dict:
dict.name()=".../test/1/pointDisplacement.boundaryField.object"

I also find out that there is a dict in fixedValuePointPatchField.C, so I believe there must be a way to create a dictionary from pointVectorField.

This problem is quite similar to: Accessing boundary patch dictionary within thermodynamic library and given a volScalarField object, how to read inputs from its dictionary, but I failed to figure it out.

My question: How can I get the patch-dictionary of a pointVectorField?

Thank you in advance.

[olesen]

Originally Posted by syuico

Hi all and dear Foamers,

I want to read the subdict "initialPoints" in the boundaryFieid of pointVectorField "pointDisplacement".

In sixDoFRigidBodyDisplacementPointPatchVectorField.C , it is read as

if (dict.found("initialPoints"))
{
    initialPoints_ = vectorField("initialPoints", dict , p.size());
}

I output the name of dict:
dict.name()=".../test/1/pointDisplacement.boundaryField.object"

I also find out that there is a dict in fixedValuePointPatchField.C, so I believe there must be a way to create a dictionary from pointVectorField.

This problem is quite similar to: Accessing boundary patch dictionary within thermodynamic library and given a volScalarField object, how to read inputs from its dictionary, but I failed to figure it out.

My question: How can I get the patch-dictionary of a pointVectorField?

Thank you in advance.

You will have to either rethink what you are trying to do, or need to re-explain here, but what you describe is not generally possible at.


When OpenFOAM constructs a GeometricField (volume, surface, point, etc) from a file, it does so by using the IOobject information (name, path, repository) combined with a given "instance" (eg, the time "0.02") to find a file and open it as an input stream. The contents of the input stream are parsed/tokenized as a general dictionary (in memory). From this dictionary, entries such as dimensions, internalField, boundaryField are used to populate the different field components. This is normally termed "de-serialization".
What you see in the code snippet you provided is part of that de-serialization for a specific boundary patch, using its respective parsed sub-dictionary.
Since all of these dictionaries only exist temporarily in memory (constructed from the stream), there are no dictionaries that you can get at later on.
Another way to think about it: if the field is generated on the fly, for example as the result of adding two fields, there would also be no dictionary for the result of that operation.


If you really need to get at the raw dictionary contents, you will need to replicate part of what I described above: get a path to a location (eg, 0.02/myField) open the contents and parse as plain dictionary. Then walk to the entry of interest and get the values you need.
If you only need the boundary information, take a look at the polyBoundaryMeshEntries class for some ideas.

[syuico]

Originally Posted by olesen

You will have to either rethink what you are trying to do, or need to re-explain here, but what you describe is not generally possible at.


When OpenFOAM constructs a GeometricField (volume, surface, point, etc) from a file, it does so by using the IOobject information (name, path, repository) combined with a given "instance" (eg, the time "0.02") to find a file and open it as an input stream. The contents of the input stream are parsed/tokenized as a general dictionary (in memory). From this dictionary, entries such as dimensions, internalField, boundaryField are used to populate the different field components. This is normally termed "de-serialization".
What you see in the code snippet you provided is part of that de-serialization for a specific boundary patch, using its respective parsed sub-dictionary.
Since all of these dictionaries only exist temporarily in memory (constructed from the stream), there are no dictionaries that you can get at later on.
Another way to think about it: if the field is generated on the fly, for example as the result of adding two fields, there would also be no dictionary for the result of that operation.


If you really need to get at the raw dictionary contents, you will need to replicate part of what I described above: get a path to a location (eg, 0.02/myField) open the contents and parse as plain dictionary. Then walk to the entry of interest and get the values you need.
If you only need the boundary information, take a look at the polyBoundaryMeshEntries class for some ideas.

Thanks for your reply! You really answer my doubts. I can finally give up trying to convert the pointVectorField to a dictionary.

As for the solution, I do think about copying the file and changing the class to "dictionary" to read the values. But it seems a little dirty.
About the "polyBoundaryMeshEntries" class, it seems that I can only get the information of boundary mesh instead of boundary field values?
Please correct me if I'm wrong.

Thanks for your reply again!

[olesen]

The fastest explanation - just try something like is already done in the code:

https://develop.openfoam.com/Develop...type=heads#L78


Can use with a specified type-name, or (see comments in IOobject typeHeaderOk) without checks for the "class" in the header.

[syuico]

Originally Posted by olesen

The fastest explanation - just try something like is already done in the code:

https://develop.openfoam.com/Develop...type=heads#L78


Can use with a specified type-name, or (see comments in IOobject typeHeaderOk) without checks for the "class" in the header.

It works! THANK U SO MUCH!