Using ACT, how can I create a result plot scoped to a path and a specific body?

Options
Pernelle Marone-Hitz
Pernelle Marone-Hitz Member, Moderator, Employee Posts: 831
First Comment First Anniversary Ansys Employee Solution Developer Community of Practice Member
edited June 2023 in Structures

Using ACT, how can I create a result plot scoped to a path and a specific body ?

Tagged:

Answers

  • Pernelle Marone-Hitz
    Pernelle Marone-Hitz Member, Moderator, Employee Posts: 831
    First Comment First Anniversary Ansys Employee Solution Developer Community of Practice Member
    Answer ✓
    Options

    The following code will create a maximum principal stress plot scoped to a path named "my_path" and to a body named "my_body":

        solu=ExtAPI.DataModel.Project.Model.Analyses[0].Solution # refer to solution
    my_stress_path=solu.AddMaximumPrincipalStress() # add maximum principal stress plot
    path=ExtAPI.DataModel.GetObjectsByName("my_path")[0] # obtain reference to path by name

    # obtain reference to body thanks to its display name 
    geo = ExtAPI.DataModel.GeoData
    for asm in geo.Assemblies:
        for part in asm.Parts:
            for body in part.Bodies: 
                if body.Name=="my_body":
                    my_body=body
                    
    # create temporary list of Ids for the body               
    temp_sel=ExtAPI.SelectionManager.CreateSelectionInfo(SelectionTypeEnum.GeometryEntities)
    temp_list=[my_body.Id]
    temp_sel.Ids=temp_list

    # modify result to define location (path and bodies)
    my_stress_path.Location = Ansys.Mechanical.Selection.PathLocation(path, temp_sel) # define location to selected path and bodies

Categories