Is there any way to calculate deformed face area from apdl results file?

Rajesh Meena

I would like to calculate deformed face area of a crack face for comparing deformation or crack opening.
Is there a python way to do this?

Rajesh Meena

There are two solutions:

Mechanical DPF, using iron python:

import mech_dpf
import Ans.DataProcessing as dpf
mech_dpf.setExtAPI(ExtAPI)
import math

dataSource = dpf.DataSources(Model.Analyses[0].ResultFileName)
model = dpf.Model(dataSource)


whole_mesh = model.Mesh
face_scoping = model.GetNamedSelection("NS_SECRACK_BOTTOMFACE")

op = dpf.operators.mesh.skin(mesh=whole_mesh,
    mesh_scoping=face_scoping,
)

skin_mesh = op.outputs.mesh.GetData()
u = dpf.operators.result.displacement()
u.inputs.data_sources.Connect(dataSource)
u.inputs.mesh.Connect(skin_mesh)

op = dpf.operators.geo.elements_facets_surfaces_over_time() # operator instantiation
op.inputs.mesh.Connect(skin_mesh)
op.inputs.displacement.Connect(u)
my_fields_container = op.outputs.fields_container.GetData()
deformed_area = math.fsum(my_fields_container[0].Data)

print(deformed_area)

2. PyDPF using CPython

from ansys.dpf import core as dpf 

model =  dpf.Model(r"C:\Users\rmeena\AppData\Local\Temp\WB_rmeena_21364_2\wbnew_files\dp0\SYS\MECH\file.rst")

whole_mesh = model.metadata.meshed_region

face_scoping = model.metadata.named_selection("FACE_SET")

op = dpf.operators.mesh.skin(
    mesh=whole_mesh,
    mesh_scoping=face_scoping,
)

skin_mesh = op.outputs.mesh()

#undeformed_area
face_area = skin_mesh._as_vtk().area

# Deformed area
deformed_mesh = skin_mesh.deform_by(model.results.displacement.on_mesh_scoping(skin_mesh.nodes.scoping))
skin_mesh.nodes.coordinates_field.data = deformed_mesh.data
deformed_face_area = skin_mesh._as_vtk().area
print(face_area)

You could also covert the ironpython code to Cpython using same operator.

Rajesh Meena

There are two solutions:

Mechanical DPF, using iron python:

import mech_dpf
import Ans.DataProcessing as dpf
mech_dpf.setExtAPI(ExtAPI)
import math

dataSource = dpf.DataSources(Model.Analyses[0].ResultFileName)
model = dpf.Model(dataSource)


whole_mesh = model.Mesh
face_scoping = model.GetNamedSelection("NS_SECRACK_BOTTOMFACE")

op = dpf.operators.mesh.skin(mesh=whole_mesh,
    mesh_scoping=face_scoping,
)

skin_mesh = op.outputs.mesh.GetData()
u = dpf.operators.result.displacement()
u.inputs.data_sources.Connect(dataSource)
u.inputs.mesh.Connect(skin_mesh)

op = dpf.operators.geo.elements_facets_surfaces_over_time() # operator instantiation
op.inputs.mesh.Connect(skin_mesh)
op.inputs.displacement.Connect(u)
my_fields_container = op.outputs.fields_container.GetData()
deformed_area = math.fsum(my_fields_container[0].Data)

print(deformed_area)

2. PyDPF using CPython

from ansys.dpf import core as dpf 

model =  dpf.Model(r"C:\Users\rmeena\AppData\Local\Temp\WB_rmeena_21364_2\wbnew_files\dp0\SYS\MECH\file.rst")

whole_mesh = model.metadata.meshed_region

face_scoping = model.metadata.named_selection("FACE_SET")

op = dpf.operators.mesh.skin(
    mesh=whole_mesh,
    mesh_scoping=face_scoping,
)

skin_mesh = op.outputs.mesh()

#undeformed_area
face_area = skin_mesh._as_vtk().area

# Deformed area
deformed_mesh = skin_mesh.deform_by(model.results.displacement.on_mesh_scoping(skin_mesh.nodes.scoping))
skin_mesh.nodes.coordinates_field.data = deformed_mesh.data
deformed_face_area = skin_mesh._as_vtk().area
print(face_area)

You could also covert the ironpython code to Cpython using same operator.