Example of worflow automation: create geometry, model setup, and postprocess

Pernelle Marone-Hitz

Is there an example of workflow automation with geometry creation, model setup and postprocessing?

Find more posts tagged with

SpaceClaim

Mechanical

Discovery

Accepted answers

All comments

Pernelle Marone-Hitz

Below is an example.

First, we'll create the geometry.

The script below will work both in SpaceClaim and in Discovery. It:

creates a base block and four smaller blocks on the top
defines a name for the base block
creates four named selections (one for the base block body, one for the smaller blocks bodies, one for the bottom base face and one for the upper faces)

# Python Script, API Version = V23
ClearAll()

# Geometry dimensions
par_L = MM(50) # length of base block
par_W = MM(25) # width of base block
par_H = MM(10) # height of base block

par_l = MM(20) # length of small block
par_w = MM(10) # width of small block
par_h = MM(5) # height of small block
offset = MM(2.5)

# Create base block
base_block = BlockBody.Create(Point.Create(MM(0), MM(0), MM(0)), Point.Create(par_L, par_W, par_H ), ExtrudeType.ForceAdd)
base_block.CreatedBodies[0].SetName('Base Block Body')
my_body_selection = Selection.Create(base_block.CreatedBodies[0])
my_body_selection.CreateAGroup('Base Block NS')
my_faces_selection = my_body_selection.ConvertToFaces()
for face in my_faces_selection.Items:
    if face.EvalMid().Point.Z == MM(0):
        Selection.Create(face).CreateAGroup('Base Face NS')

 # Create smaller blocks
small_block_1 = BlockBody.Create(Point.Create(offset, offset, par_H ), Point.Create( par_L/2 - offset, par_w, par_H + par_h ), ExtrudeType.ForceIndependent)
small_block_2 = BlockBody.Create(Point.Create(par_L/2 + offset, offset, par_H ), Point.Create(par_L-offset , par_w, par_H + par_h ), ExtrudeType.ForceIndependent)
small_block_3 = BlockBody.Create(Point.Create(offset, par_W - offset-par_w, par_H ), Point.Create( par_L/2 - offset, par_W - offset , par_H + par_h ), ExtrudeType.ForceIndependent)
small_block_4 = BlockBody.Create(Point.Create(par_L/2 + offset, par_W - offset-par_w, par_H  ), Point.Create(par_L-offset , par_W - offset, par_H + par_h), ExtrudeType.ForceIndependent)
my_body_selection = Selection.Create(small_block_1.CreatedBodies[0], small_block_2.CreatedBodies[0], small_block_3.CreatedBodies[0], small_block_4.CreatedBodies[0])
my_body_selection.CreateAGroup('Small Blocks NS')
my_faces_selection = my_body_selection.ConvertToFaces()
top_face_list = []
for face in my_faces_selection.Items:
    if face.EvalMid().Point.Z == par_H + par_h :
        top_face_list.append(face)
Selection.Create(top_face_list).CreateAGroup('Top Faces NS')

In SpaceClaim, the resulting tree can be found in the "Structure" tab, and the named selections in the "Groups" tab:

In Discovery, the tree is on the top left:

and the named selections can be found in the "Advanced Selection" menu at the bottom right:

Pernelle Marone-Hitz

Then, we'll create the Mechanical model setup and postprocessing.

For the script to work, it is assumed that two materials have already been added in Engineering Data:

(these could also be created through scripting). It is also assumed that a Steady State thermal analysis is considered (the code could easily be adapted for other boundary conditions for other types of analyses).

The script will:

add material assignements
add boundary conditions based on named selections
insert results
export these results to a specified folder to extract screenshots of the plots, animations of the plots, and values of the plots

Pernelle Marone-Hitz

The Mechanical script is:

# Retrieve bodies
all_bodies = ExtAPI.DataModel.Project.Model.Geometry.GetChildren(DataModelObjectCategory.Body,True)
base_block_body = [body for body in all_bodies if body.Name.Contains('Base')]
small_block_bodies = [body for body in all_bodies if body.Name.Contains('Solid')]


# Define material assignation
material_assignation_steel = ExtAPI.DataModel.Project.Model.Materials.AddMaterialAssignment()
sel = ExtAPI.SelectionManager.CreateSelectionInfo(SelectionTypeEnum.GeometryEntities)
sel.Ids = [body.GetGeoBody().Id for body in base_block_body]
material_assignation_steel.Location = sel
material_assignation_steel.Material = 'Structural Steel'


material_assignation_iron = ExtAPI.DataModel.Project.Model.Materials.AddMaterialAssignment()
sel = ExtAPI.SelectionManager.CreateSelectionInfo(SelectionTypeEnum.GeometryEntities)
sel.Ids = [body.GetGeoBody().Id for body in small_block_bodies]
material_assignation_iron.Location = sel
material_assignation_iron.Material = 'Aluminum'


# Define boundary conditions based on Named Selections


analysis = ExtAPI.DataModel.Project.Model.Analyses[0]


temp_base = analysis.AddTemperature()
temp_base.Location = ExtAPI.DataModel.GetObjectsByName("Base Face NS")[0]
temp_base.Magnitude.Output.SetDiscreteValue(0, Quantity(50, "C"))


convection = analysis.AddConvection()
convection.Location = ExtAPI.DataModel.GetObjectsByName("Top Faces NS")[0]
convection.FilmCoefficient.Output.SetDiscreteValue(0, Quantity(25, "W m^-1 m^-1 C^-1"))
convection.AmbientTemperature.Output.SetDiscreteValue(0, Quantity(5, "C"))


# Solve model
analysis.Solve()


# Insert results
solution = ExtAPI.DataModel.Project.Model.Analyses[0].Solution
temp_plot = solution.AddTemperature()
temp_plot_on_ns = solution.AddTemperature()
temp_plot_on_ns.Location = ExtAPI.DataModel.GetObjectsByName("Top Faces NS")[0]
solution.EvaluateAllResults()


# Export results
import os
export_folder = r'D:\Data'


all_results = solution.GetChildren(DataModelObjectCategory.Result,True)
for result in all_results:
    export_name = os.path.join(export_folder,result.Name)
    ExtAPI.Graphics.ExportImage(export_name +'.png')
    result.ExportAnimation(export_name + '.avi')
    result.ExportToTextFile(export_name + '.txt')