Example/asme 10 (#265)

* ASME example

* Spaces removed

* Modifications based on comments made on previous PR

* test included in test_examples.py

* unchanged files removed

* unchanged files removed

ansys/dpf/core/examples/downloads.py

@@ -405,3 +405,23 @@ def download_hemisphere() -> str:
 
     """
     return _download_file("hemisphere", "hemisphere.rst")
+
+
+def download_example_asme_result() -> str:
+    """Download an example result file from a static analysis and
+    return the download path.
+    Examples files are downloaded to a persistent cache to avoid
+    re-downloading the same file twice.
+    Returns
+    -------
+    str
+        Path to the example file.
+    Examples
+    --------
+    Download an example result file and return the path of the file
+    >>> from ansys.dpf.core import examples
+    >>> path = examples.download_example_asme_result()
+    >>> path
+    'C:/Users/user/AppData/local/temp/asme_example.rst'
+    """
+    return _download_file("postprocessing", "asme_example.rst")

ansys/dpf/core/examples/examples.py

@@ -18,4 +18,4 @@
 transient_therm = os.path.join(_module_path, "rth", "rth_transient.rth")
 msup_transient = os.path.join(_module_path, "msup_transient_plate1.rst")
 simple_cyclic = os.path.join(_module_path, "file_cyclic.rst")
-distributed_msup_folder = os.path.join(_module_path, 'msup_distributed')
+distributed_msup_folder = os.path.join(_module_path, 'msup_distributed')

examples/00-basic/10-asme_secviii_divtwo.py

@@ -0,0 +1,146 @@
+"""
+.. _ref_ASME_SecVIII_Div2:
+
+ASME Section VIII Division 2: pressure vessels
+----------------------------
+This example demonstrates how PyDPF might be used to postprocess a Mechanical
+model according to an international standard.
+
+The standard chosen for this example is the well-known ASME Section VIII Division
+2 used for pressure vessels design.
+
+This example is taken from Workshop 02.1 from Ansys Mechanical Advanced Topics.
+Instead of using several user defined results as it is done in the workshop,
+DPF is able to calculate the triaxial strain limit and compare it with the
+equivalent plastic strain, as specified in Equation 5.7 assuming 0 forming strain.
+
+Please be aware that this is just an example, so it is the user's duty to verify
+that calculation is made according to latest ASME standard.
+"""
+
+# Here we import rst file from Workshop 02.1
+# Since it is a elastic-plastic analysis, there are several substeps. We focus
+# on the latest substep (number 4)
+
+import ansys.dpf.core as dpf
+from ansys.dpf.core import examples
+
+path = examples.download_example_asme_result()
+model = dpf.Model(path)
+dataSource = model.metadata.data_sources
+
+timeScoping = dpf.Scoping()
+timeScoping.location = dpf.locations.time_freq
+timeScoping.ids = [4]
+
+
+###############################################################################
+# Parameters input
+# ~~~~~~~~~~~~~~~~
+# User must go to ASME Section III Division 2 and get parameters alfasl & m2
+# Below the code if user is going to introduce these parameters manually
+# alfasl = input("Please introduce alfasl parameter from ASME\n")
+# alfasl = float(alfasl)
+# m2 = input("Please introduce m2 parameter from ASME\n")
+# m2 = float(m2)
+# Values for this exercise: alfasl = 2.2 & m2 = .288, same as original
+#
+
+alfasl = 2.2
+m2 = .288
+
+###############################################################################
+# Stresses & strains
+# ~~~~~~~~~~~~~~~~~~
+# Stresses and strains are read. For getting same results as Mechanical, we read
+# Elemental Nodal strains and apply Von Mises invariant. Currently this operator
+# does not have the option to define effective Poisson's ratio. Due to this,
+# a correction factor is applied.
+
+seqv_op = dpf.operators.result.stress_von_mises(time_scoping = timeScoping,
+                                                data_sources = dataSource,
+                                                requested_location = 'Nodal')
+seqv = seqv_op.outputs.fields_container()
+
+s1_op = dpf.operators.result.stress_principal_1(time_scoping = timeScoping,
+                                                data_sources = dataSource,
+                                                requested_location = 'Nodal')
+s1 = s1_op.outputs.fields_container()
+
+s2_op = dpf.operators.result.stress_principal_2(time_scoping = timeScoping,
+                                                data_sources = dataSource,
+                                                requested_location = 'Nodal')
+s2 = s2_op.outputs.fields_container()
+
+s3_op = dpf.operators.result.stress_principal_3(time_scoping = timeScoping,
+                                                data_sources = dataSource,
+                                                requested_location = 'Nodal')
+s3 = s3_op.outputs.fields_container()
+
+strain_op = dpf.operators.result.plastic_strain(data_sources = dataSource,
+                                                requested_location = 'ElementalNodal',
+                                                time_scoping = timeScoping)
+pstrain = strain_op.outputs.fields_container()
+
+eppleqv_op = dpf.operators.invariant.von_mises_eqv_fc(fields_container = pstrain)
+eppleqv = eppleqv_op.outputs.fields_container()
+
+poisson_ratio_correction = 1.3/1.5
+eppleqvmech_op = dpf.operators.math.scale_fc(fields_container = eppleqv,
+                                             ponderation = poisson_ratio_correction)
+eppleqvmech = eppleqvmech_op.outputs.fields_container()
+
+
+eppleqvave_op = dpf.operators.averaging.to_nodal_fc(fields_container = eppleqvmech)
+eppleqvave = eppleqvave_op.outputs.fields_container()
+
+###############################################################################
+# Triaxial strain limit calculation
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+# S12=S1+S2
+s12_op = dpf.operators.math.add_fc(fields_container1 = s1,
+                                   fields_container2 = s2)
+s12 = s12_op.outputs.fields_container()
+# S123=S12+S3
+s123_op = dpf.operators.math.add_fc(fields_container1 = s12,
+                                    fields_container2 = s3)
+s123 = s123_op.outputs.fields_container()
+# SVM_scale=SVM*3
+ratio = 3.0
+seqvs_op = dpf.operators.math.scale_fc(fields_container = seqv,
+                                       ponderation = ratio)
+seqvs = seqvs_op.outputs.fields_container()
+# S123/SVM*3
+sratio_op = dpf.operators.math.component_wise_divide(fieldA = s123,
+                                                     fieldB = seqvs)
+sratio = sratio_op.outputs.field()
+# S123/SVM*3-0.33
+sterm_op = dpf.operators.math.add_constant(field = sratio,
+                                           ponderation = -1/3)
+sterm = sterm_op.outputs.field()
+# -alfasl/(1+m2)*stressterm
+ratio2 = -alfasl/(1+m2)
+expt_op = dpf.operators.math.scale(field = sterm,
+                                   ponderation = ratio2)
+expt = expt_op.outputs.field()
+# exp(-alfasl/(1+m2)*stressterm)
+exp_op = dpf.operators.math.exponential(field = expt)
+exp = exp_op.outputs.field()
+# elu*exp(-alfasl/(1+m2)*stressterm)
+strainlimit_op = dpf.operators.math.scale(field = exp,
+                                          ponderation = m2)
+strainlimit = strainlimit_op.outputs.field()
+
+###############################################################################
+# Strain limit condition (less than 1 pass the criteria)
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+strainratio = dpf.operators.math.component_wise_divide(fieldA = eppleqvave,
+                                                       fieldB = strainlimit)
+strainratio = strainratio.outputs.field()
+
+###############################################################################
+# Strain limit condition is plot
+# ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+model.metadata.meshed_region.plot(strainratio)
+dpf.server.shutdown_all_session_servers()

tests/test_examples.py

@@ -15,6 +15,11 @@ def test_download_all_kinds_of_complexity():
     assert isinstance(Model(path), Model)
 
 
+def test_download_example_asme_result():
+    path = examples.download_example_asme_result()
+    assert isinstance(Model(path), Model)
+
+
 @pytest.mark.parametrize(
     "example",
     [