How can I make displacement in a static structural analysis dependent on a geometric parameter ?

Rosse7 · October 2024

Hi,
when my optimization analysis runs some geometry dimensions (parameterized inside Design Modeler) change and I need my given displacement (in tabular form) proportionally change too.
How can I overcome this trouble?
Thank you

Jimmy He · October 2024

Hi Rosse7,

The value of a parameter in Workbench can be accessed within Mechanical scripting via the following:

import wbjn
# P1 is the name of the parameter in Workbench, change as needed.
value_string = wbjn.ExecuteCommand(ExtAPI,"""returnValue(str(Parameters.GetParameter(Name="P1").Value))""")
value_quantity = Quantity( value_string ) # Value of the parameter as a Quantity
print( value_quantity )

Once you have the current value of the parameter from Mechanical scripting, you can proceed with using it to change the boundary condition.

Best,
Jimmy

Erik Kostson · October 2024

@Rosse7

Below is a sample script that you can modify as needed - it is a python code (before solve target callback), and it updates the displacement imposed on a face, and based on the dimension of the geometry (this dim., changes for every design point). One can use the script parameter as below or use (commented away ) as mentioned the bounding box.

All the best

Erik

def before_solve(this, analysis):# Do not edit this line
    """
    Called before solving the parent analysis.
    Keyword Arguments : 
        this -- the datamodel object instance of the python code object you are currently editing in the tree
        analysis -- Static Structural
    """


    # To access properties created using the Property Provider, please use the following command.
    # this.GetCustomPropertyByPath("your_property_group_name/your_property_name")

    # To access scoping properties use the following to access geometry scoping and named selection respectively:
    # this.GetCustomPropertyByPath("your_property_group_name/your_property_name/Geometry Selection")
    # this.GetCustomPropertyByPath("your_property_group_name/your_property_name/Named Selection")
    import wbjn
    tbody=ExtAPI.DataModel.GetObjectsByName("Mysolidbody 1")[0]
    gbody =tbody.GetGeoBody()



    # P1 is the name of the parameter in Workbench, change as needed.
    xdim = float(wbjn.ExecuteCommand(ExtAPI,"""returnValue(str(Parameters.GetParameter(Name="P1").Value))""").split(' ')[0]) # geom. dim., changing for every design point


    #gbb=gbody.GetBoundingBox() # Bounding box method
    #xdim=gbb[3]-gbb[0]

    analysis=ExtAPI.DataModel.Project.Model.Analyses[0] # refer to analysis
    my_disp=ExtAPI.DataModel.GetObjectsByName("Displacement")[0]

    my_disp.Location=ExtAPI.DataModel.GetObjectsByName("Selection")[0] # scope boundary condition to named selection called "Selection"
    my_disp.XComponent.Inputs[0].DiscreteValues=[Quantity('0[s]'),Quantity('1[s]')] # define input values for tabular data
    my_disp.XComponent.Output.DiscreteValues=[Quantity('0[mm]'),Quantity(str(xdim*0.05)+'[m]')] # define output values for tabular data loading
    pass

Rosse7 · October 2024

Hi Jimmy He,

Thank you very much for your suggestion.
Could you tell me how to define/update displacement tabular data (e.g. in x) via scripting too, please?

Thank you,

Manu

Erik Kostson · October 2024

Hi

Another way is to use a python code (before solve target callback) that is updated for every design point.

One can use perhaps the bounding box of the body (see code below on how to do that), and then use that to scale the displacement. Or a Parameter as shown above can be scaled and used for the displacement.

See here how to define displacement:

https://discuss.ansys.com/discussion/151/activate-deactivate-boundary-conditions-through-scripting

All the best

Erik

    tbody=ExtAPI.DataModel.GetObjectsByName("Mysolidbody 1")[0] # tree body
    gbody =tbody.GetGeoBody() # geobody


    gbb=gbody.GetBoundingBox()
    xdim=gbb[3]-gbb[0] # x-dim