How to get the material properties for defined element using Mechanical API or DPF?

Hello team,

I'm creating a script that gets the stress values in elements defined by element Id and would like to compare the stress values with the ultimate ones for material automatically. So, I wonder how to get the values of material properties for the element with a defined Id using Mechanical API or DPF?

Thanks

Find more posts tagged with

Mechanical

scripting

DPF

Accepted answers

All comments

dafedin

The following code:

import mech_dpf
import Ans.DataProcessing as dpf
mech_dpf.setExtAPI(ExtAPI)
dataSources = mech_dpf.GetDataSources(2)
mat_op = dpf.operators.metadata.material_provider()
mat_op.inputs.data_sources.Connect(dataSources)
mats = mat_op.outputs.materials.GetData()

bringing error:

Could not find the specified Output Type.

Why showed code doesn't work?

Pernelle Marone-Hitz

This example in the PyDPF documentation can be adapted to Mechanical DPF: https://dpf.docs.pyansys.com/version/0.8/examples/00-basic/12-get_material_properties.html

Pernelle Marone-Hitz

See this post for a Mechanical implementation: https://discuss.ansys.com/discussion/2554/python-result-example-plot-young-modulus-on-elements/p1?new=1

dafedin

@Pernelle Marone-Hitz said:
See this post for a Mechanical implementation: https://discuss.ansys.com/discussion/2554/python-result-example-plot-young-modulus-on-elements/p1?new=1

Hello Pernelle,

I used the proposed approach and it worked well but then I tried to run this script in Ansys Mechanical 2021R2 and got the error:
'MeshedRegion' object has no attribute 'GetPropertyField'
The possible reason is that there is no method GetPropertyField("mat") for 'MeshedRegion' object in the 2021R2 release of DPF. What is the best approach to get the values of material properties for the element with a defined ID in the 2021R2 release?

Thanks

Pernelle Marone-Hitz

Hi @dafedin , unfortunately there is a bug in older versions with GetPropertyField("mat") . Please upgrade to 2023R2. Sorry for the inconvenience.

dafedin

Hello Pernelle,

I have already upgraded to 2023R2 but our customers haven't. Maybe there is a way to do it using another API.

Thanks

Pernelle Marone-Hitz

Hi, as far as I'm aware there isn't, but I might have missed it. Let's see if some else chimes in.

Mike.Thompson

@Pernelle Marone-Hitz @dafedin

How about the materials module for Mechanical? This module can be imported and gives access to material properties that are in Workbench/Mechanical. I think this is also covered in the intro to Mechanical scripting course

Pernelle Marone-Hitz

@Mike.Thompson @dafedin I thought the question was around DPF. Sure in Mechanical scripting we can use the materials module. There are many examples on the forum (for example, this one: https://discuss.ansys.com/discussion/35/can-you-provide-an-example-of-using-the-materials-module-in-mechanical) This approach would however be more convoluted: in Mechanical the material properties are tied to a body, so to know the materials property for a specific element ID you'll have to use MeshData to link the elem id to the body id.

KristianHansen

Dear, @Pernelle Marone-Hitz

I have tried extracting the "DAMP" material property, but I continue to only get zero-values back.

The following code is used:

'''
from ansys.dpf import core as dpf
import hansen_dpf_functions as hdpf
import numpy as np

from settings.config import \
USER_SETTINGS

Load models

model0 = dpf.Model(USER_SETTINGS['model0Path'] + r"\file.rst")
full_mesh = model0.metadata.meshed_region

mats = full_mesh.property_field("mat")
op = dpf.operators.result.mapdl_material_properties() # operator instantiation
op.inputs.properties_name.connect("DAMP")
op.inputs.materials.connect(mats)
op.inputs.data_sources.connect(model0)
my_properties_value = op.outputs.properties_value()

my_properties_value[0].data
'''

And the following output is given:

DPFArray([0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0.,
0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0.,
0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0.,
0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0.,
0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0.,
0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0.,
0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0., 0.,
0., 0., 0., 0., 0., 0.])

I have defined a constant structural damping coefficient in the assigned material of 0.2.
Is the assigned material damping not transferred to the mapdl_material_properties?

Br,
Kristian

KristianHansen

For more info, I have made a script for screening the available results (Please see below)
The only non-zero entries are: ['EX', 'NUXY', 'DENS', 'ALPX', 'KXX', 'C', 'RSVX'] which I find very strange...

from ansys.dpf import core as dpf
import numpy as np

from settings.config import USER_SETTINGS

Load model

model0 = dpf.Model(USER_SETTINGS['model0Path'] + r"\file.rst")
full_mesh = model0.metadata.meshed_region
mats = full_mesh.property_field("mat")

property_names = [
"EX", "EY", "EZ", # Young's modulus in X, Y, Z directions
"NUXY", "NUYZ", "NUXZ", # Poisson's ratios
"GXY", "GYZ", "GXZ", # Shear moduli
"DENS", # Density
"ALPX", "ALPY", "ALPZ", # Thermal expansion coefficients
"DMPR", # Damping ratio
"DMPS", # Constant structural damping
"MU", # Coefficient of friction
"VISC", # Viscosity
"KXX", "KYY", "KZZ", # Thermal conductivity
"C", "CREF", # Specific heat, reference specific heat
"RSVX", "RSVY", "RSVZ", # Resistivity
"MURX", "MURY", "MURZ", # Relative permeability
"PRXY", "PRYZ", "PRXZ", # Plastic Poisson's ratio
"SIGXT", "SIGXC", "SIGYT", "SIGYC", # Tensile/compressive strengths
"EMIS", # Thermal emissivity
"BKIN", "MKIN", # Bilinear and multilinear kinematic hardening
"CREEP", # Creep constants
"PIEZ", # Piezoelectric matrix
"SONC", # Speed of sound
"ENTH", # Enthalpy
"DMPRAT","DMPSTR","DMPEXT","DAMP","DMPR","DMPS" # Other Damping keywords found in APDL reference
]

non_zero_properties = {}

for prop_name in property_names:
mat_prop = dpf.operators.result.mapdl_material_properties()
mat_prop.inputs.materials.connect(mats)
mat_prop.inputs.properties_name.connect(prop_name)
mat_prop.inputs.data_sources.connect(model0) # Connect the data source

prop_field = mat_prop.outputs.properties_value.get_data()

if prop_field and prop_field[0].data.size > 0:  # Ensure there's data
    data = prop_field[0].data
    if not np.all(data == 0):
        non_zero_properties[prop_name] = data
        print(f"{prop_name}: {data}")
    else:
        print(f"{prop_name}: All zeros")
else:
    print(f"{prop_name}: No data returned")

print("\nProperties that are not all zeros:")
for prop_name, data in non_zero_properties.items():
print(f"{prop_name}: {data}")

List of non-zero property names only

non_zero_list = [prop_name for prop_name in non_zero_properties.keys()]
print("\nList of non-zero properties:")
print(non_zero_list)

KristianHansen

A final update: writing out the input file confirms the correct assigment of a damping material property
An example is included below:

However, as shown with the "screening script" provided above, DMPS returns zero-values across all materials.

Temperature = 'TEMP' ! Temperature
MP,DENS,23,7850, ! kg m^-3
MP,ALPX,23,1.2e-05, ! C^-1
MP,C,23,434, ! J kg^-1 C^-1
MP,KXX,23,60.5, ! W m^-1 C^-1
MP,RSVX,23,1.7e-07, ! kg m^3 A^-2 s^-3
MP,EX,23,200000000000, ! Pa
MP,NUXY,23,0.3,
MP,MURX,23,10000,
MP,DMPS,23,0.2, ! <===== Damping is correctly parsed to solver
MP,UVID,23,ae106af0-c310-4b2a-ade1-449230bc7543
MP,UMID,23,cc778694-08bb-46b9-b2bb-6244373cf850

Pernelle Marone-Hitz

@KristianHansen This looks like a bug to me. Could you please open an official support case to your local Ansys support provider, so that we can further investigate and open a bug if needed ? Thank you

KristianHansen

Dear @Pernelle Marone-Hitz
I have opened an issue on the dpf core github (https://github.com/ansys/pydpf-core/issues/2197)

Thank you for taking the time to read through the issue.

Best regards,
Kristian

Pernelle Marone-Hitz

Dear @KristianHansen, I had mentioned Ansys Support as I initially thought you were using DPF in Mechanical. But reading your code again I realized you're indeed using PyDPF, so Github is the right route to go !
Best regards.