Adding a settings api example, and other changes refactoring examples

examples/00-fluent/exhaust_system.py

@@ -1,8 +1,7 @@
 """.. _ref_exhaust_system_tui_api:
 
-Exhaust System: Fault-tolerant Meshing
+End-to-end Fault-tolerant Meshing Workflow
 ----------------------------------------------
-
 This tutorial illustrates the setup and solution of a three-dimensional
 turbulent fluid flow in a manifold exhaust system. The manifold configuration
 is encountered in the automotive industry. It is often important to predict
@@ -11,8 +10,7 @@
 unlike the watertight workflow used in Fluid Flow in a Mixing Elbow, is
 appropriate for geometries with imperfections, such as gaps and leakages.
 
-This tutorial demonstrates how to do the following in Ansys Fluent:
-
+End-to-end Fault Tolerant Meshing example demonstrating use of 'tui' modules:
 
 - Use the Fault-tolerant Meshing guided workflow to:
     - Import a CAD geometry and manage individual parts
@@ -37,10 +35,15 @@
 """
 
 ###############################################################################
-# First, connect with a Fluent server
+# First, download the geometry file and start Fluent as a service with
+# Meshing Mode, Double Precision, Number of Processors 2
 
 import ansys.fluent.core as pyfluent
 from ansys.fluent.core import examples
+from ansys.fluent.post import set_config
+from ansys.fluent.post.pyvista import Graphics
+
+set_config(blocking=True, set_view_on_display="isometric")
 
 import_filename = examples.download_file(
     "exhaust_system.fmd", "pyfluent/exhaust_system"
@@ -50,7 +53,7 @@
 # Start Fluent in double precision running on 2 processors
 
 session = pyfluent.launch_fluent(
-    meshing_mode=True, precision="double", processor_count=4
+    meshing_mode=True, precision="double", processor_count=2
 )
 
 ###############################################################################
@@ -650,6 +653,25 @@
 )
 # session.solver.tui.display.objects.display("scene-1")
 
+###############################################################################
+# Mesh display using PyVista
+
+graphics_session = Graphics(session)
+mesh_1 = graphics_session.Meshes["mesh-1"]
+mesh_1.show_edges = True
+mesh_1.surfaces_list = [
+    "inlet-1",
+    "inlet-2",
+    "inlet-3",
+    "outlet-1",
+    "flow-pipe",
+    "main.1",
+    "object1.1",
+    "object2.1",
+    "outpipe3.1",
+]
+
+mesh_1.display()
 ###############################################################################
 # Save case, data and exit.
 # session.solver.tui.file.write_case_data("exhaust_system.cas.h5")

examples/00-fluent/mixing_elbow.py

@@ -1,15 +1,15 @@
 """.. _ref_mixing_elbow_tui_api:
 
-Fluid Flow and Heat Transfer in a Mixing Elbow
-----------------------------------------------
+End-to-end Watertight Meshing Workflow
+---------------------------------------
 This example illustrates the setup and solution of a three-dimensional
 turbulent fluid flow and heat transfer problem in a mixing elbow. The mixing
 elbow configuration is encountered in piping systems in power plants and
 processindustries. It is often important to predict the flow field and
 temperature field in the area of the mixing regionin order to properly design
 the junction.
 
-This example demonstrates how to do the following:
+End-to-end Watertight Meshing example demonstrating use of 'tui' modules:
 
 - Use the Watertight Geometry guided workflow to:
     - Import a CAD geometry
@@ -43,12 +43,12 @@
 from ansys.fluent.post import set_config
 from ansys.fluent.post.pyvista import Graphics
 
-set_config(blocking=True)
+set_config(blocking=True, set_view_on_display="isometric")
 
 import_filename = examples.download_file("mixing_elbow.pmdb", "pyfluent/mixing_elbow")
 
 session = pyfluent.launch_fluent(
-    meshing_mode=True, precision="double", processor_count=4
+    meshing_mode=True, precision="double", processor_count=2
 )
 
 ###############################################################################

examples/00-fluent/mixing_elbow_settings_api.py

@@ -0,0 +1,229 @@
+""".. _ref_mixing_elbow_settings_api_beta:
+
+Fluent Setup and Solutoin using Settings API (Beta)
+--------------------------------------------------
+This example illustrates the setup and solution of a three-dimensional
+turbulent fluid flow and heat transfer problem in a mixing elbow. The mixing
+elbow configuration is encountered in piping systems in power plants and
+processindustries. It is often important to predict the flow field and
+temperature field in the area of the mixing regionin order to properly design
+the junction.
+
+This example demonstrates use of 'settings' modules (Beta):
+
+- Launch Ansys Fluent
+- Import Mesh
+- Define Material
+- Setup Cell Zone Conditions
+- Setup Boundary Conditions
+- Iniialize and Solve
+- Compute Mass Flow Rate and Temperature
+- Display Mesh and Contour using PyVista
+
+Problem Description:
+A cold fluid at 20 deg C flows into the pipe through a large inlet, and mixes
+with a warmer fluid at 40 deg C that enters through a smaller inlet located at
+the elbow. The pipe dimensions are in inches and the fluid properties and
+boundary conditions are given in SI units. The Reynolds number for the flow at
+the larger inlet is 50, 800, so a turbulent flow model will be required.
+"""
+# sphinx_gallery_thumbnail_number = 2
+
+###############################################################################
+# First, download the mesh file and start Fluent as a service with
+# Solver Mode, Double Precision, Number of Processors 2
+
+import ansys.fluent.core as pyfluent
+from ansys.fluent.core import examples
+from ansys.fluent.post import set_config
+from ansys.fluent.post.pyvista import Graphics
+
+set_config(blocking=True, set_view_on_display="isometric")
+
+import_filename = examples.download_file("mixing_elbow.msh.h5", "pyfluent/mixing_elbow")
+
+session = pyfluent.launch_fluent(precision="double", processor_count=2)
+###############################################################################
+# Import mesh and perform mesh check:
+# The mesh check will list the minimum and maximum x, y, and z values from the
+# mesh in the default SI unit of meters. It will also report a number of other
+# mesh features that are checked. Any errors in the mesh will be reported at
+# this time. Ensure that the minimum volume is not negative, since Ansys Fluent
+# cannot begin a calculation when this is the case.
+
+session.solver.root.file.read(file_type="case", file_name=import_filename)
+session.solver.tui.mesh.check()
+
+###############################################################################
+# Set the working units for the mesh:
+# select "in" to set inches as the working unit for length. Note:  Because the
+# default SI units will be used for everything except length, there is no need
+# to change any other units in this problem. If you want a different working
+# unit for length, other than inches (for example, millimeters), make the
+# appropriate change.
+
+session.solver.tui.define.units("length", "in")
+
+###############################################################################
+# Enable heat transfer by activating the energy equation.
+
+session.solver.root.setup.models.energy.enabled = True
+
+###############################################################################
+# Create a new material called water-liquid.
+
+session.solver.root.setup.materials.copy_database_material_by_name(
+    type="fluid", name="water-liquid"
+)
+
+###############################################################################
+# Set up the cell zone conditions for the fluid zone (elbow-fluid). Select
+# water-liquid from the Material list.
+
+session.solver.root.setup.cell_zone_conditions.fluid[
+    "elbow-fluid"
+].material = "water-liquid"
+
+###############################################################################
+# Set up the boundary conditions for the inlets, outlet, and walls for your CFD
+# analysis.
+# cold inlet (cold-inlet), Setting: Value:
+# Velocity Specification Method: Magnitude, Normal to Boundary
+# Velocity Magnitude: 0.4 [m/s]
+# Specification Method: Intensity and Hydraulic Diameter
+# Turbulent Intensity: 5 [%]
+# Hydraulic Diameter: 4 [inch]
+# Temperature: 293.15 [K]
+
+session.solver.root.setup.boundary_conditions.velocity_inlet["cold-inlet"].vmag = {
+    "option": "constant or expression",
+    "constant": 0.4,
+}
+session.solver.root.setup.boundary_conditions.velocity_inlet[
+    "cold-inlet"
+].ke_spec = "Intensity and Hydraulic Diameter"
+session.solver.root.setup.boundary_conditions.velocity_inlet[
+    "cold-inlet"
+].turb_intensity = 5
+session.solver.root.setup.boundary_conditions.velocity_inlet[
+    "cold-inlet"
+].turb_hydraulic_diam = "4 [in]"
+session.solver.root.setup.boundary_conditions.velocity_inlet["cold-inlet"].t = {
+    "option": "constant or expression",
+    "constant": 293.15,
+}
+
+###############################################################################
+# hot inlet (hot-inlet), Setting: Value:
+# Velocity Specification Method: Magnitude, Normal to Boundary
+# Velocity Magnitude: 1.2 [m/s]
+# Specification Method: Intensity and Hydraulic Diameter
+# Turbulent Intensity: 5 [%]
+# Hydraulic Diameter: 1 [inch]
+# Temperature: 313.15 [K]
+
+session.solver.root.setup.boundary_conditions.velocity_inlet["hot-inlet"].vmag = {
+    "option": "constant or expression",
+    "constant": 1.2,
+}
+session.solver.root.setup.boundary_conditions.velocity_inlet[
+    "hot-inlet"
+].ke_spec = "Intensity and Hydraulic Diameter"
+session.solver.root.setup.boundary_conditions.velocity_inlet[
+    "hot-inlet"
+].turb_hydraulic_diam = "1 [in]"
+session.solver.root.setup.boundary_conditions.velocity_inlet["hot-inlet"].t = {
+    "option": "constant or expression",
+    "constant": 313.15,
+}
+
+###############################################################################
+# pressure outlet (outlet), Setting: Value:
+# Backflow Turbulent Intensity: 5 [%]
+# Backflow Turbulent Viscosity Ratio: 4
+
+session.solver.root.setup.boundary_conditions.pressure_outlet[
+    "outlet"
+].turb_viscosity_ratio = 4
+
+###############################################################################
+# Disable the plotting of residuals during the calculation.
+
+session.solver.tui.solve.monitors.residual.plot("no")
+
+###############################################################################
+# Initialize the flow field using the Hybrid Initialization
+
+session.solver.root.solution.initialization.hybrid_initialize()
+
+###############################################################################
+# Solve for 150 Iterations.
+
+session.solver.root.solution.run_calculation.iterate.get_attr("arguments")
+session.solver.root.solution.run_calculation.iterate(number_of_iterations=150)
+
+###############################################################################
+# Create and display velocity vectors on the symmetry-xyplane plane.
+
+session.solver.root.results.graphics.vector["velocity_vector_symmetry"] = {}
+session.solver.root.results.graphics.vector["velocity_vector_symmetry"].print_state()
+session.solver.root.results.graphics.vector[
+    "velocity_vector_symmetry"
+].field = "temperature"
+session.solver.root.results.graphics.vector[
+    "velocity_vector_symmetry"
+].surfaces_list = [
+    "symmetry-xyplane",
+]
+session.solver.root.results.graphics.vector[
+    "velocity_vector_symmetry"
+].scale.scale_f = 4
+session.solver.root.results.graphics.vector["velocity_vector_symmetry"].style = "arrow"
+# session.solver.root.results.graphics.vector["velocity_vector_symmetry"].display()
+
+###############################################################################
+# Compute mass flow rate
+
+session.solver.root.solution.report_definitions.flux["mass_flow_rate"] = {}
+session.solver.root.solution.report_definitions.flux[
+    "mass_flow_rate"
+].zone_names.get_attr("allowed-values")
+session.solver.root.solution.report_definitions.flux["mass_flow_rate"].zone_names = [
+    "cold-inlet",
+    "hot-inlet",
+    "outlet",
+]
+session.solver.root.solution.report_definitions.flux["mass_flow_rate"].print_state()
+session.solver.root.solution.report_definitions.compute(report_defs=["mass_flow_rate"])
+
+###############################################################################
+# Mesh display using PyVista
+
+graphics_session = Graphics(session)
+mesh_1 = graphics_session.Meshes["mesh-1"]
+mesh_1.show_edges = True
+mesh_1.surfaces_list = [
+    "cold-inlet",
+    "hot-inlet",
+    "wall-elbow",
+    "wall-inlet",
+    "symmetry-xyplane",
+    "outlet",
+]
+
+mesh_1.display()
+
+###############################################################################
+# Temperature Contour display using PyVista
+
+contour_1 = graphics_session.Contours["contour_1"]
+contour_1.field = "temperature"
+contour_1.surfaces_list = ["symmetry-xyplane"]
+contour_1.display()
+
+###############################################################################
+# Write final case and data. Exit.
+# session.solver.tui.file.write_case_data('mixing_elbow2_set.cas.h5')
+# session.exit()
+
+###############################################################################

examples/02-postprocessing/post_processing_exhaust_manifold.py

@@ -1,20 +1,22 @@
 """.. _ref_post_processing_exhaust_manifold:
 
-Post Processing using PyVista and Matplotlib: Exhaust Manifold
-----------------------------------------------------------------------
+Post Processing using PyVista and Matplotlib
+---------------------------------------------
 This example demonstrates the postprocessing capabilities of PyFluent
 (using PyVista and Matplotlib) using a 3D model
 of an exhaust manifold with high temperature flows passing through.
 The flow through the manifold is turbulent and
 involves conjugate heat transfer.
 
-This example demonstrates how to do the following:
+This example demonstrates post-processing using pyvista:
 
 - Create surfaces for the display of 3D data.
 - Display filled contours of temperature on several surfaces.
 - Display velocity vectors.
 - Plot quantitative results using Matplotlib
 """
+# sphinx_gallery_thumbnail_number = -1
+
 ###############################################################################
 import ansys.fluent.core as pyfluent
 from ansys.fluent.core import examples
@@ -36,7 +38,7 @@
     filename="exhaust_system.dat.h5", directory="pyfluent/exhaust_system"
 )
 
-session = pyfluent.launch_fluent(precision="double", processor_count=4)
+session = pyfluent.launch_fluent(precision="double", processor_count=2)
 
 session.solver.tui.file.read_case(case_file_name=import_case)
 session.solver.tui.file.read_data(case_file_name=import_data)

tests/test_tui_api.py

@@ -1,10 +1,10 @@
 from util.solver_workflow import new_solver_session  # noqa: F401
 
 
-def test_report_system_proc_stats_tui(new_solver_session, capsys) -> None:
+def test_report_summary_tui(new_solver_session, capsys) -> None:
     new_solver_session.start_transcript()
     # Issue: Transcript missing for the first TUI command
-    new_solver_session.solver.tui.report.system.sys_stats()
-    new_solver_session.solver.tui.report.system.sys_stats()
+    new_solver_session.solver.tui.report.summary("no")
+    new_solver_session.solver.tui.report.summary("no")
     captured = capsys.readouterr()
-    assert "CPU/Memory Usage" in captured.out
+    assert "Settings" in captured.out