This example demonstrates a basic structural study using scripting in ANSYS AIM. After you extract the ScriptingGuideExamples.zip file, you will find the files for this example in the AIM_Structural_Study directory.
ANSYS AIM Script The script for this example follows.
1 # encoding: utf-8
2 SetScriptVersion(Version="16.0")
3 Reset()
4
5 # Define working directory
6 workingDir = r"D:\ScriptingGuideExamples\AIM_Structural_Study\"
7 CADFile = "gearcasing.agdb"
8 projectName = "sce-4-mech.wbpj"
9
10 import os
11 fullPath = os.path.join(workingDir, CADFile)
12 savePath = os.path.join(workingDir, projectName)
13
14 with Transaction():
15 # Define Study system and access the container
16 system1 = GetSystem(Name="Study")
17 study1 = system1.GetContainer(ComponentName="Study")
18
19 # Define the Tasks and Groups
20 importComponent1 = Study.CreateTask(Type="Import", System=system1)
21 meshingComponent1 = Study.CreateTask(Type="Meshing", System=system1)
22
23 physicsDefinitionComponent1 = Study.CreateTask(Type="Physics Definition",System=system1)
24 solvePhysicsComponent1 = Study.CreateTask(Type="Solve Physics",System=system1)
25 # physicsDefinitionComponent1 and solvePhysicsComponent1 will be grouped together
26
27 physicsSolutionGroup1 = Study.CreateGroup(Name="Physics Solution")
28 physicsSolutionGroup1.Add(Component=physicsDefinitionComponent1)
29 physicsSolutionGroup1.Add(Component=solvePhysicsComponent1)
30
31 resultsEvaluationComponent1 = Study.CreateTask(Type="Results Evaluation", System=system1)
32
33 # Define the Import
34 import1 = importComponent1.GetTaskObject()
35
36 # Define the Part Meshing properties
37 partMesh1 = meshingComponent1.GetTaskObject()
38 partMesh1.EngineeringIntent = "StructuralOrThermalOrElectricConduction"
39 partMesh1.GlobalMeshSizingAttributes.UseAdvancedSizeFunction = "Adaptive"
40
41 # Define the Solution properties
42 physicsDefinition1 = physicsDefinitionComponent1.GetTaskObject()
43 physicsDefinition1.CalculationType = "Static"
44
45 # Define PhysicsRegion, SolverSettings, Material
46 physicsRegion1 = study1.CreateEntity(Type="PhysicsRegion",AssociatedObject=physicsDefinition1)
47 physicsRegion1.PhysicsType = "Structural"
48 physicsRegion1.Location = "AllBodies()"
49
50 solverSettings1 = study1.CreateEntity(Type="SolverSettings",AssociatedObject=physicsDefinition1)
51
52 material1 = study1.CreateEntity(Type="Material", AssociatedObject=physicsDefinition1)
53 material1.ImportEngineeringData(Name="Structural Steel")
54
55 materialAssignment1 = study1.CreateEntity(Type="MaterialAssignment",AssociatedObject=physicsDefinition1)
56 materialAssignment1.Material = material1
57 materialAssignment1.Location = [physicsRegion1]
58
59 # Define upstream-downstream links between the tasks
60 AddSourceToComponentInSystem(SourceComponent=importComponent1, TargetComponent=meshingComponent1)
61 AddSourceToComponentInSystem(SourceComponent=meshingComponent1, TargetComponent=physicsDefinitionComponent1)
62 AddSourceToComponentInSystem(SourceComponent=physicsDefinitionComponent1, TargetComponent=solvePhysicsComponent1)
63 AddSourceToComponentInSystem(SourceComponent=solvePhysicsComponent1, TargetComponent=resultsEvaluationComponent1)
64
65 # Add a Transcript tab
66 transcript1 = study1.CreateEntity(Type="Transcript", AssociatedObject=physicsDefinition1)
67
68 # Define Results
69 results1 = resultsEvaluationComponent1.GetTaskObject()
70
71 with Transaction():
72 # Import the CAD
73 Study.AddGeometryImportSourceOperation(ObjectReference=import1)
74 geometryImportSource1 = study1.GetGeometryImportSource(Name="GeometryImportSource 1")
75 geometryImportSource1.FilePath = fullPath
76 geometryImportSource1.GeometryPreferences.ImportNamedSelections = "True"
77 geometryImportSource1.GeometryPreferences.NamedSelectionKey = ""
78
79 importComponent1.Update(AllDependencies=True)
80
81 # Refresh other cells
82 meshingComponent1.Refresh()
83 physicsDefinitionComponent1.Refresh()
84 resultsEvaluationComponent1.Refresh()
85
86 # Define Boundary Conditions
87 with Transaction():
88 support1 = study1.CreateEntity(Type="Support", AssociatedObject=physicsRegion1)
89 support1.Location = 'GetSelectionSet("@side1")'
90
91 with Transaction():
92 pressure1 = study1.CreateEntity(Type="Pressure", AssociatedObject=physicsRegion1)
93 pressure1.Location = 'GetSelectionSet("@side2")'
94 pressure1.Magnitude = "1.0E7 [Pa]"
95 # Define this as a input Parameter
96 parameter1 = Parameters.CreateParameter(Entity=pressure1, PropertyName="Magnitude", IsOutput=False)
97 parameter1.Expression = str(pressure1.Magnitude)
98 parameter1.DisplayText="Pressure1"
99
100 # Add post-processing contours
101 with Transaction():
102 contourResult1 = study1.CreateEntity(Type="ContourResult", AssociatedObject=results1)
103 contourResult1.Variable = "Displacement.mag"
104 contourResult1.Location = "AllBodies()"
105 contourResult1.DisplayText = "Total Deformation"
106 # Define this as a output Parameter
107 parameter2 = Parameters.CreateParameter(Entity=contourResult1, PropertyName="Summary.Max", IsOutput=True, IsDirectOutput=True)
108 parameter2.DisplayText="Maximum Deformation"
109
110 with Transaction():
111 contourResult2 = study1.CreateEntity(Type="ContourResult", AssociatedObject=results1)
112 contourResult2.Variable = "Stress.eqv"
113 contourResult2.Location = "AllBodies()"
114 contourResult2.DisplayText = "Eqv Stress"
115
116 with Transaction():
117 vectorResult1 = study1.CreateEntity(Type="VectorResult", AssociatedObject=results1)
118 vectorResult1.Variable = "Displacement"
119 vectorResult1.Location = "AllBodies()"
120
121 # Generate the Mesh
122 meshingComponent1.Update(AllDependencies=True)
123
124 # Perform the Simulation
125 # Perform the Simulation
126 with Transaction():
127 physicsDefinitionComponent1.Update(AllDependencies=True)
128 solvePhysicsComponent1.Update(AllDependencies=True)
129
130 # Update the Results
131 resultsEvaluationComponent1.Update(AllDependencies=True)
132
133 # Save project to working directory
134 Save(FilePath=savePath, Overwrite=True)
135
136 # Exit from Workbench AIM
137Discussion A description of each line follows.
Reset() command starts a new session.
The working directory is set, so that the script can load the geometry file from the specified location. When completing this example, this line will need to be modified to reflect your working location.
The 'os' module used in this script provides capabilities for interacting with operating system services. Refer to the Python Standard Library documentation for details on all available modules.
This part defines a basic Static Structural analysis template. All the different tasks (e.g., geometry import, mesh generation, solution and results) are created and populated.
Different tasks (e.g., geometry import, mesh generation, solution, and results) are created.
Define some global properties for the mesh generation.
Define PhysicsRegion, SolverSettings, and Material for the solution.
Define links between the tasks, i.e., meshing task takes the geometry from the import task as input; solution task takes the mesh generated from the meshing task, etc.
Add a Transcript tab so that solver output information can be monitored.
The geometry file is imported (along all NamedSelections) and other tasks are refreshed as their upstream data is updated.
Define a fixed support boundary condition on "side1" Named Selection.
Define a 1.0E7 Pa pressure load "side2" Named Selection and make it an input parameter, named "Pressure1".
Create a displacement magnitude contours on all bodies.
Make the maximum displacement magnitude as a output parameter, named "Maximum Deformation".
Create more contour and vector results.
Generate the mesh.
Perform the simulation.
Evaluate all of the results.
Save the project files.