How to actually get the strain energy using pyAnsys dpf-core?

dominik.schwinn

I am trying to get the strain energy from a result-file using pyAnsys dpf-core. Actually I do not see a direct access to this result (maybe there is but I just cannot find it). So I tried to acess the strain energy density so that I can calculate the strain energy using the element volumes.

However, as a result from my Python code I get an empty array, even though the results do exist - at least I can see them (print and plot) in the in the ANSYS Mechanical GUI (ANSYS Classic).

The Python code I am using is

from ansys.dpf import core as dpf

rst_file = 'path_to_my_result_file.rst'

data_sources = dpf.DataSources()
data_sources.set_result_file_path(rst_file)
data_sources.result_files

loadcases = [1]
elem_ids = np.arange(1,3061)

lc_scoping = dpf.Scoping()
lc_scoping.ids = loadcases
elem_scoping = dpf.Scoping()
elem_scoping.ids=elem_ids

sene_op = dpf.operators.result.elastic_strain_energy_density()

sene_op.inputs.data_sources.connect(data_sources)
sene_op.inputs.time_scoping(lc_scoping)
sene_op.inputs.mesh_scoping(elem_scoping)
sene_op.inputs.bool_rotate_to_global(False)
sene_op.inputs.requested_location('Elemental')

sene_fc = sene_op.outputs.fields_container()
sene_f = sene_fc.get_field_by_time_id(1)
sene_data = sene_f.data
scoping_ids = sene_fc[0].scoping.ids

print(" strain energy ".center(40,'*'))
print(sene_data)
print(" scoping_ids ".center(40,'*'))
print(scoping_ids)

leading to the following output:
************ strain energy *************
[]
************* scoping_ids **************
[]

I am using ANSYS 2022R2 to solve my model and dpf-version 0.13.8 with Python 3.10.14.

Does anyone know how to resolve this issue? or maybe know how to directly access strain energy?

Thanks a lot in advance

Rohith Patchigolla

Hello @dominik.schwinn

I believe to have direct strain energy access in the rst file, one would need to activate nonlinearity of some sort (nonlinear material or large deflection effects) when solving the model and creating the rst file. Image from help documentation pasted below for reference.

If not, for linear analysis, one can acess the strain energy as shown below, perhaps by manually calculating strain energy density similar to the below mechanical dpf script (to give you the idea.)

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

analysis = Model.Analyses[1]
data_source = dpf.DataSources(r'' + analysis.WorkingDir + 'file.rst')

scop = dpf.Scoping()
scop.Ids = [1]

##Get Stress & Strain
Strain_op = dpf.operators.result.elastic_strain()
Strain_op.inputs.mesh_scoping.Connect(scop)# optional
Strain_op.inputs.data_sources.Connect(data_source)
my_Strain = Strain_op.outputs.fields_container.GetData()

Stress_op = dpf.operators.result.stress()
Stress_op.inputs.mesh_scoping.Connect(scop)# optional
Stress_op.inputs.data_sources.Connect(data_source)
my_Stress = Stress_op.outputs.fields_container.GetData()

##Compute Strain * Stress
dot_fc = dpf.operators.math.dot()
dot_fc.inputs.fieldA.Connect(my_Strain[0])
dot_fc.inputs.fieldB.Connect(my_Stress[0])
Product = dot_fc.outputs.field.GetData()

Scale_op = dpf.operators.math.scale()
Scale_op.inputs.field.Connect(Product)
Scale_op.inputs.ponderation.Connect(0.5)

my_EnergyDensity= Scale_op.outputs.field.GetData()