How to retrieve MAPDL matids for each body in a custom result?

Pierre Thieffry

Customer wants to retrieve the MatID associated to selected bodies in a custom result in 2020R2. How can he do this?

Pierre Thieffry

the solver_data structure would be useful in such a case, as it now has a .GetMaterialSolverId(geoBodyId) function. But... this was not available in 2020R2.

I found out that the information is written to the ds.dat file in a comment block. So here is a sample code that will retrieve the information from the ds.dat file, write out a text file to user_files and display a message in Mechanical with the body ids corresponding to the ACT object selection. Not the most elegant solution, but it works...

# Custom Result Object Evaluation 
def EvaluateMatID(result,stepInfo,collector):      

    import os

    # Reader initialization 
    reader = result.Analysis.GetResultsData()     
    reader.CurrentResultSet = stepInfo.Set 

    solution=result.Parent.Solution

    matids_dict={}
    # Write a file with body names and corresponding APDL MatID
    f_out=open(os.path.join(result.Analysis.WorkingDir,'../../../user_files','matids.txt'),'w') # File to be written in user_files folder

    datfile=os.path.join(result.Analysis.WorkingDir,'ds.dat') # MAPDL input file to be parsed

    with open(datfile,'r') as f: # Parse MAPDL file
        line=f.readline()
        while line.find('!************************* Model Summary ********************')==-1: # This indicates where the correspondance between body names and matid are available
            line=f.readline()
        # read body names and matid
        line=f.readline()
        while line.find('!************************* End Model Summary ********************')==-1:  # Read in the comments
            splitline=line.split(',') # Split with "," to separate information in the comments
            f_out.write(splitline[0].strip('!')+'\t'+splitline[-1])  # Write out first part of line (body name) and last part (matid)
            matids_dict[splitline[0].strip('!')]=int(splitline[-1]) # create dictionary with material ids
            line=f.readline()
        
    f_out.close()   

    # display message with matid for selected body(ies) for the ACT object
    propGeo = result.Properties["Geometry"]
    refIds = propGeo.Value.Ids

    mat_ids=[]
    for bodyId in refIds:
        bodyName=ExtAPI.DataModel.GeoData.GeoEntityById(bodyId).Name
        mat_ids.append(matids_dict[bodyName])

    msg = Ansys.Mechanical.Application.Message('Found the following material Ids: '+str(mat_ids), MessageSeverityType.Warning)
    ExtAPI.Application.Messages.Add(msg)

Pierre Thieffry

The above script only works if all bodies have different names. I had to adapt it so we don't rely on body names but just on their order in the tree

def EvaluateMatID(result,stepInfo,collector): 
    '''Evaluates Normal Stress as a custom result, with different averaging options.''' 

    import os

    # Reader initialization 
    reader = result.Analysis.GetResultsData()     
    reader.CurrentResultSet = stepInfo.Set 

    solution=result.Parent.Solution

    matids_dict={}
    body_index=0
    # Write a file with body names and corresponding APDL MatID
    f_out=open(os.path.join(result.Analysis.WorkingDir,'../../../user_files','matids.txt'),'w') # File to be written in user_files folder

    datfile=os.path.join(result.Analysis.WorkingDir,'ds.dat') # MAPDL input file to be parsed

    with open(datfile,'r') as f: # Parse MAPDL file
        line=f.readline()
        while line.find('!************************* Model Summary ********************')==-1: # This indicates where the correspondance between body names and matid are available
            line=f.readline()
        # read body names and matid
        line=f.readline()
        while line.find('!************************* End Model Summary ********************')==-1:  # Read in the comments
            splitline=line.split(',') # Split with "," to separate information in the comments
            f_out.write(splitline[0].strip('!')+'\t'+splitline[-1])  # Write out first part of line (body name) and last part (matid)
            matids_dict[body_index]=[splitline[0].strip('!'),int(splitline[-1])] # create dictionary with material ids
            body_index+=1
            line=f.readline()
        
    f_out.close()   

    # display message with matid for selected body(ies) for the ACT object
    propGeo = result.Properties["Geometry"]
    refIds = propGeo.Value.Ids

    # as we can have duplicate body names, running through body Ids in order they appear 
    # in the tree
    mat_ids=[]
    body_index=0
    bodies=ExtAPI.DataModel.GetObjectsByType(DataModelObjectCategory.Body) # retrieve all bodies
    for body in bodies:
        geo_body_id=body.GetGeoBody().Id        
        if geo_body_id in refIds:
            mat_ids.append(matids_dict[body_index][1])
        body_index+=1

        
    msg = Ansys.Mechanical.Application.Message('Found the following material Ids: '+str(mat_ids), MessageSeverityType.Warning)
    ExtAPI.Application.Messages.Add(msg)
        

CollinsJnr

@Pierre Thieffry
Thank you for these code

I wanted to ask about the

Ansys.ACT.Interfaces.Analysis.ISolverData.GetMaterialSolverId(geoID)

the documentation says only one parameter is required (int32)

But shell shows this

Ansys.ACT.Interfaces.Analysis.ISolverData.GetMaterialSolverId(26)
GetMaterialSolverId() takes exactly 2 arguments (1 given)

And when I try to give a second parameter it shows this

Ansys.ACT.Interfaces.Analysis.ISolverData.GetMaterialSolverId(ISolverData,26)
expected ISolverData, got type

What is this second parameter (ISolerData) and how can I find it?

Thank you in advance

Mike.Thompson

If you are trying to get this information for post processing after the solution is done, you should look at the solution object: Solution.SolverData

If you are trying to get this before the solve while, the input file is being written. The solver data is passed as an argument to the get solved commands Call Back.

Pierre Thieffry

@CollinsJnr to follow up on @Mike.Thompson ' s reply, you can use this in a Python Code with "Get Solve commands" callback:

geobody_id=741
matid_for_a_body=Ansys.ACT.Interfaces.Analysis.ISolverData.GetMaterialSolverId(solver_data,geobody_id)

As Mike mentioned, the 'solver_data' info is an argument passed to the callback as you can see from the comments in the Python Code:

solver_data -- data stucture that allows you to access information from the model such as current step, contact pair ids, etc.

Using the function as is in the console will lead to the message on the required argument. Nevertheless, the documentation is indeed misleading. I will report internally.