Cantilever Beam¶

beamExample.py from Reproducing the cantilever beam tutorial.

Reproduce the cantilever beam example from the Appendix of the Getting Started with Abaqus: Interactive Edition Manual.

The example leads you through the Abaqus/CAE modeling process by visiting each of the modules and shows you the basic steps to create and analyze a simple model. In Creating and Analyzing a Simple Model in Abaqus/CAE, you create a model of a steel cantilever beam and load its top surface. You then analyze the beam and plot the resulting stresses and displacements. Fig. 1 illustrates the model that you create and analyze.

../../_images/gst-beam.png — Fig. 1 A loaded cantilever beam.¶

from abaqus import *
from abaqusConstants import *

backwardCompatibility.setValues(includeDeprecated=True, reportDeprecated=False)

# Create a model.

myModel = mdb.Model(name="Beam")

# Create a new viewport in which to display the model
# and the results of the analysis.

myViewport = session.Viewport(name="Cantilever Beam Example", origin=(20, 20), width=150, height=120)

# -----------------------------------------------------

import part

# Create a sketch for the base feature.

mySketch = myModel.ConstrainedSketch(name="beamProfile", sheetSize=250.0)

# Create the rectangle.

mySketch.rectangle(point1=(-100, 10), point2=(100, -10))

# Create a three-dimensional, deformable part.

myBeam = myModel.Part(name="Beam", dimensionality=THREE_D, type=DEFORMABLE_BODY)

# Create the part's base feature by extruding the sketch
# through a distance of 25.0.

myBeam.BaseSolidExtrude(sketch=mySketch, depth=25.0)

# -----------------------------------------------------

import material

# Create a material.

mySteel = myModel.Material(name="Steel")

# Create the elastic properties: youngsModulus is 209.E3
# and poissonsRatio is 0.3

elasticProperties = (209.0e3, 0.3)
mySteel.Elastic(table=(elasticProperties,))

# -------------------------------------------------------

import section

# Create the solid section.

mySection = myModel.HomogeneousSolidSection(name="beamSection", material="Steel", thickness=1.0)

# Assign the section to the region. The region refers
# to the single cell in this model.

region = (myBeam.cells,)
myBeam.SectionAssignment(region=region, sectionName="beamSection")

# -------------------------------------------------------

import assembly

# Create a part instance.

myAssembly = myModel.rootAssembly
myInstance = myAssembly.Instance(name="beamInstance", part=myBeam, dependent=OFF)

# -------------------------------------------------------

import step

# Create a step. The time period of the static step is 1.0,
# and the initial incrementation is 0.1; the step is created
# after the initial step.

myModel.StaticStep(
    name="beamLoad", previous="Initial", timePeriod=1.0, initialInc=0.1, description="Load the top of the beam."
)

# -------------------------------------------------------

import load

# Find the end face using coordinates.

endFaceCenter = (-100, 0, 12.5)
endFace = myInstance.faces.findAt((endFaceCenter,))

# Create a boundary condition that encastres one end
# of the beam.

endRegion = (endFace,)
myModel.EncastreBC(name="Fixed", createStepName="beamLoad", region=endRegion)

# Find the top face using coordinates.

topFaceCenter = (0, 10, 12.5)
topFace = myInstance.faces.findAt((topFaceCenter,))

# Create a pressure load on the top face of the beam.

topSurface = ((topFace, SIDE1),)
myModel.Pressure(name="Pressure", createStepName="beamLoad", region=topSurface, magnitude=0.5)

# -------------------------------------------------------

import mesh

# Assign an element type to the part instance.

region = (myInstance.cells,)
elemType = mesh.ElemType(elemCode=C3D8I, elemLibrary=STANDARD)
myAssembly.setElementType(regions=region, elemTypes=(elemType,))

# Seed the part instance.

myAssembly.seedPartInstance(regions=(myInstance,), size=10.0)

# Mesh the part instance.

myAssembly.generateMesh(regions=(myInstance,))

# Display the meshed beam.

myViewport.assemblyDisplay.setValues(mesh=ON)
myViewport.assemblyDisplay.meshOptions.setValues(meshTechnique=ON)
myViewport.setValues(displayedObject=myAssembly)

# -------------------------------------------------------

import job

# Create an analysis job for the model and submit it.

jobName = "beam_tutorial"
myJob = mdb.Job(name=jobName, model="Beam", description="Cantilever beam tutorial")

# Wait for the job to complete.

myJob.submit()
myJob.waitForCompletion()

# -------------------------------------------------------

import visualization

# Open the output database and display a
# default contour plot.

myOdb = visualization.openOdb(path=jobName + ".odb")
myViewport.setValues(displayedObject=myOdb)
myViewport.odbDisplay.display.setValues(plotState=CONTOURS_ON_DEF)

myViewport.odbDisplay.commonOptions.setValues(renderStyle=FILLED)

Gallery generated by Sphinx-Gallery