Feat/gui mode

examples/00-fluent/README.txt

@@ -1,3 +1,3 @@
 Full Examples Using PyFluent
 ============================
-These examples demonstrate how to use Fluent solver capabilities from Python.
+These examples demonstrate how to use Fluent capabilities from Python.

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 Workflow example:
 
 - 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
 )
 
 ###############################################################################
@@ -651,7 +654,29 @@
 # session.solver.tui.display.objects.display("scene-1")
 
 ###############################################################################
-# Save case, data and exit.
+# 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.
 # session.solver.tui.file.write_case_data("exhaust_system.cas.h5")
 
-# session.exit()
+#########################################################################
+# Close Fluent
+
+session.exit()

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
+process industries. It is often important to predict the flow field and
+temperature field in the area of the mixing region in order to properly design
 the junction.
 
-This example demonstrates how to do the following:
+End-to-end Watertight Meshing Workflow example:
 
 - 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
 )
 
 ###############################################################################
@@ -516,4 +516,10 @@
 # Write final case and data.
 # session.solver.tui.file.write_case_data("mixing_elbow2_tui.cas.h5")
 
+#########################################################################
+# Close Fluent
+
+session.exit()
+
+
 ###############################################################################

examples/00-fluent/mixing_elbow_settings_api.py

@@ -0,0 +1,231 @@
+""".. _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
+process industries. It is often important to predict the flow field and
+temperature field in the area of the mixing region in 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.
+# session.solver.tui.file.write_case_data('mixing_elbow2_set.cas.h5')
+
+#########################################################################
+# Close Fluent
+
+session.exit()