How can I plot stresses on all plies of same material on fiber orientation system inside Mechanical?

Question

If a named selection is created based on plies with same material, fiber orientation system cannot be selected, since each ply might have a different orientation. This is easily doable in PyDPF-Composites, but it requires to move away from Mechanical GUI. Is there any option to stay in Mechanical GUI and get stresses on fiber direction for all plies of a specific material?

Javier Vique · Answer

In case of using 24R2, RetrieveResult() is not exposed, so the evaluation is driven by EvaluateAllResults(). Below the modified code for that version:

"""Ansys Mechanical scripting (2024 R2 compatible): scan every ply made of a

selected material and report, for each stress component (normal X/Y/Z and shear

XY/YZ/XZ), which ply holds the maximum value and which ply holds the minimum

value.

Difference with ``plies_min_max_stress.py``: ``RetrieveResult()`` is not exposed

in 2024 R2, so the evaluation is driven by ``Solution.EvaluateAllResults()``.

Since that call evaluates every result object of the Solution anyway, one

NormalStress and one ShearStress object are kept alive together and paired

component by component (SX with SXY, SY with SYZ, SZ with SXZ). For each ply the

three pairs are evaluated, which harvests the six stress components with only

three ``EvaluateAllResults()`` calls per ply instead of six.

Run from the Mechanical Scripting console (Automation > Scripting).

"""

SELECTED_MATERIAL = "Epoxy Carbon UD (230 GPa) Prepreg"

ANALYSIS_INDEX = 0

# Delete the temporary result objects once the scan is finished.

DELETE_TEMP_RESULTS = True

NORMAL_COMPONENTS = [

    ("SX (fiber direction)", "XAxis"),

    ("SY (transverse to fiber)", "YAxis"),

    ("SZ (through thickness)", "ZAxis"),

]

SHEAR_COMPONENTS = [

    ("SXY", "XYPlane"),

    ("SYZ", "YZPlane"),

    ("SXZ", "XZPlane"),

]

# Each normal component is evaluated together with the shear component of the

# same index, so both objects are refreshed by a single EvaluateAllResults().

COMPONENT_PAIRS = list(zip(NORMAL_COMPONENTS, SHEAR_COMPONENTS))

def get_ply_material(ply):

    """Return the material name of an AnalysisPly, or None if unavailable."""

    material = getattr(ply, "Material", None)

    if material is None:

        try:

            prop = ply.PropertyByName("Material")

        except Exception:

            return None

        if prop is None:

            return None

        material = getattr(prop, "StringValue", None) or prop.Value

    return str(material).strip() if material is not None else None

def build_ply_dictionary():

    """Return {material_name: [AnalysisPly, ...]} for the whole model."""

    all_plies = ExtAPI.DataModel.GetObjectsByType(DataModelObjectCategory.AnalysisPly)

plies_by_material = {}

    for ply in all_plies:

        material = get_ply_material(ply)

        if material is None:

            material = "<unknown>"

        plies_by_material.setdefault(material, []).append(ply)

    return plies_by_material

def collect_min_max(result):

    """Return (min, max) of the currently evaluated result values."""

    values = result.PlotData.Item["Values"]

    return (min(values), max(values))

def report(label, ply_min_max):

    """Print the ply holding the maximum and the ply holding the minimum."""

    if not ply_min_max:

        print("{0}: no data available.".format(label))

        return

max_ply = max(ply_min_max, key=lambda name: ply_min_max[name][1])

    min_ply = min(ply_min_max, key=lambda name: ply_min_max[name][0])

print(label)

    print("  Max: {0:.6e} on ply '{1}'".format(ply_min_max[max_ply][1], max_ply))

    print("  Min: {0:.6e} on ply '{1}'".format(ply_min_max[min_ply][0], min_ply))

plies_by_material = build_ply_dictionary()

print("Materials found in the model:")

for material, plies in plies_by_material.items():

    print("  {0}: {1} ply(ies)".format(material, len(plies)))

selected_plies = plies_by_material.get(SELECTED_MATERIAL, [])

solution = ExtAPI.DataModel.Project.Model.Analyses[ANALYSIS_INDEX].Solution

results_by_component = {}

for label, _ in NORMAL_COMPONENTS + SHEAR_COMPONENTS:

    results_by_component[label] = {}

normal_result = solution.AddNormalStress()

normal_result.CoordinateSystem = None

normal_result.CalculateTimeHistory = False

shear_result = solution.AddShearStress()

shear_result.CoordinateSystem = None

shear_result.CalculateTimeHistory = False

for ply in selected_plies:

    normal_result.Ply = [ply]

    shear_result.Ply = [ply]

for (normal_label, normal_orientation), (shear_label, shear_orientation) in COMPONENT_PAIRS:

        normal_result.NormalOrientation = getattr(NormalOrientationType, normal_orientation)

        shear_result.ShearOrientation = getattr(ShearOrientationType, shear_orientation)

solution.EvaluateAllResults()

results_by_component[normal_label][ply.Name] = collect_min_max(normal_result)

        results_by_component[shear_label][ply.Name] = collect_min_max(shear_result)

if DELETE_TEMP_RESULTS:

    normal_result.Delete()

    shear_result.Delete()

print("
=== Extreme plies for material '{0}' ===".format(SELECTED_MATERIAL))

for label, _ in NORMAL_COMPONENTS + SHEAR_COMPONENTS:

    report(label, results_by_component[label])

Javier Vique · Answer

If the user is only interested in understanding the maximum and minimum values and on which plies is happening, then we can use the script below:

"""Ansys Mechanical scripting: scan every ply made of a selected material and

report, for each stress component (normal X/Y/Z and shear XY/YZ/XZ), which ply

holds the maximum value and which ply holds the minimum value.

Unlike ``plot_stresses_fiber_direction_DevForum.py`` (one result object per ply),

this script creates a *single* NormalStress object and a *single* ShearStress

object, changes only the ``Ply`` property, calls ``RetrieveResult()`` and keeps

the min/max of that ply before moving to the next one. Both objects use

``CalculateTimeHistory = False`` so only the current result set is retrieved.

Run from the Mechanical Scripting console (Automation > Scripting).

"""

SELECTED_MATERIAL = "Epoxy Carbon UD (230 GPa) Prepreg"

ANALYSIS_INDEX = 0

# Delete the temporary result objects once the scan is finished.

DELETE_TEMP_RESULTS = True

NORMAL_COMPONENTS = [

    ("SX (fiber direction)", "XAxis"),

    ("SY (transverse to fiber)", "YAxis"),

    ("SZ (through thickness)", "ZAxis"),

]

SHEAR_COMPONENTS = [

    ("SXY", "XYPlane"),

    ("SYZ", "YZPlane"),

    ("SXZ", "XZPlane"),

]

def get_ply_material(ply):

    """Return the material name of an AnalysisPly, or None if unavailable."""

    material = getattr(ply, "Material", None)

    if material is None:

        try:

            prop = ply.PropertyByName("Material")

        except Exception:

            return None

        if prop is None:

            return None

        material = getattr(prop, "StringValue", None) or prop.Value

    return str(material).strip() if material is not None else None

def build_ply_dictionary():

    """Return {material_name: [AnalysisPly, ...]} for the whole model."""

    all_plies = ExtAPI.DataModel.GetObjectsByType(DataModelObjectCategory.AnalysisPly)

plies_by_material = {}

    for ply in all_plies:

        material = get_ply_material(ply)

        if material is None:

            material = "<unknown>"

        plies_by_material.setdefault(material, []).append(ply)

    return plies_by_material

def scan_plies(result, plies):

    """Set each ply on ``result``, retrieve it and record its min/max.

Returns {ply_name: (min_value, max_value)}.

    """

    ply_min_max = {}

    for ply in plies:

        result.Ply = [ply]

        result.RetrieveResult()

        values = result.PlotData.Item["Values"]

        ply_min_max[ply.Name] = (min(values), max(values))

    return ply_min_max

def report(label, ply_min_max):

    """Print the ply holding the maximum and the ply holding the minimum."""

    if not ply_min_max:

        print("{0}: no data available.".format(label))

        return

max_ply = max(ply_min_max, key=lambda name: ply_min_max[name][1])

    min_ply = min(ply_min_max, key=lambda name: ply_min_max[name][0])

print(label)

    print("  Max: {0:.6e} on ply '{1}'".format(ply_min_max[max_ply][1], max_ply))

    print("  Min: {0:.6e} on ply '{1}'".format(ply_min_max[min_ply][0], min_ply))

plies_by_material = build_ply_dictionary()

print("Materials found in the model:")

for material, plies in plies_by_material.items():

    print("  {0}: {1} ply(ies)".format(material, len(plies)))

selected_plies = plies_by_material.get(SELECTED_MATERIAL, [])

solution = ExtAPI.DataModel.Project.Model.Analyses[ANALYSIS_INDEX].Solution

normal_result = solution.AddNormalStress()

normal_result.CoordinateSystem = None

normal_result.CalculateTimeHistory = False

shear_result = solution.AddShearStress()

shear_result.CoordinateSystem = None

shear_result.CalculateTimeHistory = False

results_by_component = {}

for label, orientation_name in NORMAL_COMPONENTS:

    normal_result.NormalOrientation = getattr(NormalOrientationType, orientation_name)

    results_by_component[label] = scan_plies(normal_result, selected_plies)

for label, orientation_name in SHEAR_COMPONENTS:

    shear_result.ShearOrientation = getattr(ShearOrientationType, orientation_name)

    results_by_component[label] = scan_plies(shear_result, selected_plies)

if DELETE_TEMP_RESULTS:

    normal_result.Delete()

    shear_result.Delete()

print("
=== Extreme plies for material '{0}' ===".format(SELECTED_MATERIAL))

for label, _ in NORMAL_COMPONENTS + SHEAR_COMPONENTS:

    report(label, results_by_component[label])

Javier Vique · Answer

A workaround to get this plot is to extract the data for each ply and then use Python Result to plot the stresses. The attached code follows this approach, plotting only one single value per element which is the maximum of the nodal averaged stresses. It is assumed that model is based on solid approach.

plot_stresses_fiber_direction_DevForum.py