How to postprocess a Mechanical model with PyDPF-Core?

Question

I have a model built in Mechanical that has contacts and fixed supports.

I would like to perform the post-processing outside of Mechanical using PyDPF-Core and get contact pressure and reaction forces, for specific contact regions or fixed support regions. How can I do that ?

Pernelle Marone-Hitz · Answer

To extract the reaction force on the fixed support, we can use several methods:

Using reaction_force operator:

This operator will return the reaction forces, we can then sum them and take the norm to obtain the total reaction force:

reaction = dpf.operators.result.reaction_force(data_sources=datasources)

reaction_fc = reaction.outputs.fields_container()

print("Reaction force data:")

#print(reaction_fc[0].data)

rf_sum = dpf.operators.math.accumulate_over_label_fc(reaction)

rfsum = dpf.operators.math.norm(rf_sum)

rfsum_val = rfsum.outputs.field.get_data().data[0]

print("RFSUM:")

print(rfsum_val)

Which will return in my case:

Using force_summation operator:

That approach is quite convenient as is offers easy filtering of the contact elements.

fsum_op = dpf.operators.averaging.force_summation() 

fsum_op.inputs.nodal_scoping.connect(fs_scoping)

fsum_op.inputs.data_sources.connect(datasources)

fsum_op.inputs.scoping_filter.connect(0) # 0: sum all nodal forces excluding contact elements, 1: sum all nodal forces for contact nodes only, 2: sum all nodal forces for all selected nodes including contact elements

print("Force accumulation:")

my_force_accumulation = fsum_op.outputs.force_accumulation()

print(my_force_accumulation[0].data)

fsum_norm = dpf.operators.math.norm(my_force_accumulation)

fsum_normal_val = fsum_norm.outputs.field.get_data().data[0]

print("Total force:")

print(fsum_normal_val)

print("Force on nodes:")

my_forces_on_nodes = fsum_op.outputs.forces_on_nodes()

print(my_forces_on_nodes[0].data)

This returns:

Pernelle Marone-Hitz · Answer

To extract the contact pressure result on one contact region, we can then adapt the following code:

# Extract the contact pressure result

contact_pressure_op = dpf.operators.result.contact_pressure() 

contact_pressure_op.inputs.mesh_scoping.connect(ns_scoping)

contact_pressure_op.inputs.data_sources.connect(datasources)

contact_pressure_op.inputs.requested_location.connect('Nodal')

contact_pressure_fc = contact_pressure_op.outputs.fields_container()

print("Contact pressure data:")

print(contact_pressure_fc[0].data)

Which returns:

Pernelle Marone-Hitz · Answer

Now that the named selections exist, we can create several scopings to filter the results on specific named selections.

The code below creates one scoping for the first contact region, and another scoping for the fixed support:

# Create a named selection scoping

contact_ns = contact_named_selections[0]

ns_scoping_op = dpf.operators.scoping.on_named_selection() 

ns_scoping_op.inputs.requested_location.connect('Elemental')

ns_scoping_op.inputs.named_selection_name.connect(contact_ns)

ns_scoping_op.inputs.data_sources.connect(datasources)

ns_scoping = ns_scoping_op.outputs.mesh_scoping()
# Create a scoping for the fixed support
fs_scoping_op = dpf.operators.scoping.on_named_selection() 

fs_scoping_op.inputs.requested_location.connect('Nodal')

fs_scoping_op.inputs.named_selection_name.connect('_FIXEDSU')

fs_scoping_op.inputs.data_sources.connect(datasources)

fs_scoping = fs_scoping_op.outputs.mesh_scoping()