gsi_nlskewplate_caemodel.py
#
# Getting Started with ABAQUS
#
# Script for nonlinear skew plate example
#
from abaqus import *
from abaqusConstants import *
session.journalOptions.setValues(replayGeometry=COORDINATE,
recoverGeometry=COORDINATE)
session.Viewport(name='Viewport: 1', origin=(1.3671875, 1.3671875),
width=201.25, height=135.625)
session.viewports['Viewport: 1'].makeCurrent()
Mdb()
##
## Switch to the part module
##
import part
##
## Sketch profile of the plate
##
s = mdb.models['Model-1'].Sketch(name='__profile__', sheetSize=4.0)
g, v, d = s.geometry, s.vertices, s.dimensions
s.sketchOptions.setValues(sheetSize=4.0, gridSpacing=0.1, grid=ON,
gridFrequency=2, constructionGeometry=ON, dimensionTextHeight=0.1,
decimalPlaces=2)
##
## Create vertical line
##
s.Line(point1=(-1.0, 0.2), point2=(-1.0, -0.2))
s.VerticalDimension(vertex1=v[1], vertex2=v[2], textPoint=(-1.311305612325670,
-0.1574429869651790))
##
## Create construction lines
##
s.AngularConstructionLine(point=(-1.0, -0.2), angle=30.0)
s.AngularConstructionLine(point=(-1.0, 0.2), angle=30.0)
s.Spot(point=(0.0, -0.2))
s.VerticalConstructionLine(point=(0.0, -0.2))
##
## Create lines
##
s.Line(point1=(-1.0, -0.2), point2=(0.0, 0.377350269189625))
s.Line(point1=(0.0, 0.377350269189625), point2=(0.0, 0.777350269189626))
s.Line(point1=(0.0, 0.777350269189626), point2=(-1.0, 0.2))
##
## Dimensional annotations
##
s.HorizontalDimension(vertex1=v[2], vertex2=v[11], textPoint=(
-0.09921059012413020, -0.4421343281865120))
p = mdb.models['Model-1'].Part(name='Plate', dimensionality=THREE_D,
type=DEFORMABLE_BODY)
p = mdb.models['Model-1'].parts['Plate']
p.BaseShell(sketch=s)
session.viewports['Viewport: 1'].setValues(displayedObject=p)
del mdb.models['Model-1'].sketches['__profile__']
##
## Switch to the property module
##
import material
import section
##
## Create material 'Steel'
##
mdb.models['Model-1'].Material('Steel')
mdb.models['Model-1'].materials['Steel'].Elastic(table=((30.0E9, 0.3), ))
##
## Create shell section
##
mdb.models['Model-1'].HomogeneousShellSection(name='PlateSection',
preIntegrate=ON,
material='Steel', thickness=0.008,
poissonDefinition=DEFAULT, temperature=GRADIENT)
##
## Create datum coordinate system
##
p1 = mdb.models['Model-1'].parts['Plate']
e = p1.edges
p1.DatumCsysByTwoLines(CARTESIAN, line1=e.findAt((-0.75,
-0.0556624327025937, 0.0), ), line2=e.findAt((0.0,
0.477350269189625, 0.0), ))
##
## Assign material orientation to the plate
##
p0 = mdb.models['Model-1'].parts['Plate']
f = p0.faces
faces = f[0:1]
region=(None, None,
f.findAt(((-0.666666666666667,
0.125783423063208, 0.0), (0.0, 0.0, 1.0)), ), None)
datum = p0.datums[2]
p0.assignMaterialOrientation(region=region, localCsys=datum, axis=AXIS_3)
##
## Assign section to the plate
##
p0 = mdb.models['Model-1'].parts['Plate']
f = p0.faces
faces = f[0:1]
region=(None, None,
f.findAt(((-0.666666666666667,
0.125783423063208, 0.0), (0.0, 0.0, 1.0)), ), None)
p0 = mdb.models['Model-1'].parts['Plate']
p0.SectionAssignment(region=region, sectionName='PlateSection')
##
## Switch to the assembly module
##
import assembly
import part
a = mdb.models['Model-1'].rootAssembly
session.viewports['Viewport: 1'].setValues(displayedObject=a)
##
## Set coordinate system (done by default)
##
a = mdb.models['Model-1'].rootAssembly
a.DatumCsysByDefault(CARTESIAN)
##
## Instance the plate
##
p = mdb.models['Model-1'].parts['Plate']
a.Instance(name='Plate-1', part=p, dependent=ON)
##
## Partition the plate
##
p = mdb.models['Model-1'].parts['Plate']
f = p.faces
faces=(f.findAt((
-0.666666666666667, 0.125783423063208, 0.0), (0.0, 0.0, 1.0)), )
e = p.edges
p.PartitionFaceByShortestPath(faces=faces,
point1=p.InterestingPoint(e.findAt((-0.75,
-0.0556624327025937, 0.0), ), MIDDLE),
point2=p.InterestingPoint(e.findAt((-0.25,
0.63301270189222, 0.0), ), MIDDLE))
##
## Create geometry set 'MidSpan'
##
a = mdb.models['Model-1'].rootAssembly
e1 = a.instances['Plate-1'].edges
a.Set(edges=e1.findAt((
(-0.5, 0.188675134594813, 0.0), ), ), name='MidSpan')
##
## Create geometry set 'EndA'
##
a = mdb.models['Model-1'].rootAssembly
e1 = a.instances['Plate-1'].edges
a.Set(edges=e1.findAt((
(-1.0, 0.1, 0.0), ), ), name='EndA')
##
## Create geometry set 'EndB'
##
a = mdb.models['Model-1'].rootAssembly
e1 = a.instances['Plate-1'].edges
a.Set(edges=e1.findAt((
(0.0, 0.477350269189625, 0.0), ), ), name='EndB')
##
## Switch to the step module
##
import step
##
## Create a static general step
##
mdb.models['Model-1'].StaticStep(name='Apply pressure',
previous='Initial',
description="""Nonlinear analysis: Uniform pressure (20 kPa) load""",
timePeriod=1, adiabatic=OFF, maxNumInc=100,
stabilization=None, timeIncrementationMethod=AUTOMATIC, initialInc=0.1,
minInc=1e-05, maxInc=1, matrixSolver=SOLVER_DEFAULT, amplitude=RAMP,
extrapolation=LINEAR, fullyPlastic="", nlgeom=ON)
session.viewports['Viewport: 1'].assemblyDisplay.setValues(
step='Apply pressure')
##
## Modify output requests
##
mdb.models['Model-1'].fieldOutputRequests['F-Output-1'].setValues(
variables=PRESELECT, frequency=2)
a0=mdb.models['Model-1'].rootAssembly
regionDef=a0.sets['MidSpan']
mdb.models['Model-1'].historyOutputRequests['H-Output-1'].setValues(
variables=('U1', 'U2', 'U3', 'UR1', 'UR2', 'UR3'), region=regionDef)
##
## Switch to load module
##
import load
session.viewports['Viewport: 1'].assemblyDisplay.setValues(loads=ON, bcs=ON,
fields=ON)
##
## Apply bc in local CSYS to set EndB (right edge)
##
a0 = mdb.models['Model-1'].rootAssembly
region = a0.sets['EndB']
datum = mdb.models['Model-1'].rootAssembly.instances['Plate-1'].datums[2]
mdb.models['Model-1'].DisplacementBC(name='Rail boundary condition',
createStepName='Apply pressure', region=region, u2=0.0, u3=0.0, ur1=0.0,
ur2=0.0, ur3=0.0, localCsys=datum)
##
## Apply encastre bc to set EndA (left edge)
##
a0 = mdb.models['Model-1'].rootAssembly
region = a0.sets['EndA']
mdb.models['Model-1'].EncastreBC(name='Fix left end',
createStepName='Apply pressure', region=region)
##
## Apply pressure load
##
a0 = mdb.models['Model-1'].rootAssembly
f1 = a0.instances['Plate-1'].faces
region=((
f1.findAt(((
-0.666666666666667, 0.259116756396542, 0.0), (0.0, 0.0, 1.0)), ((
-0.333333333333333, 0.318233512793084, 0.0), (0.0, 0.0, 1.0)), ), SIDE1),
)
mdb.models['Model-1'].Pressure(name='Pressure',
createStepName='Apply pressure', region=region, magnitude=2.0E4)
##
## Switch to mesh module
##
import mesh
session.viewports['Viewport: 1'].assemblyDisplay.setValues(mesh=ON, loads=OFF,
bcs=OFF, fields=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.meshOptions.setValues(
meshTechnique=ON)
##
## Assign global seed
##
p.seedPart(size=0.1)
##
## Use structured meshing
##
f1 = p.faces
regions=(
f1.findAt((
-0.666666666666667, 0.259116756396542, 0.0), (0.0, 0.0, 1.0)),
f1.findAt((
-0.333333333333333, 0.318233512793084, 0.0), (0.0, 0.0, 1.0)))
p.setMeshControls(regions=regions, technique=STRUCTURED)
##
## Assign element type
##
elemType1 = mesh.ElemType(elemCode=S8R5)
elemType2 = mesh.ElemType(elemCode=STRI65)
regions=(None, None,
f1.findAt(((
-0.666666666666667, 0.259116756396542, 0.0), (0.0, 0.0, 1.0)), ((
-0.333333333333333, 0.318233512793084, 0.0), (0.0, 0.0, 1.0)), ), None)
p.setElementType(regions=regions, elemTypes=(elemType1, elemType2))
##
## Generate mesh
##
p.generateMesh()
##
## Switch to job module
##
import job
session.viewports['Viewport: 1'].assemblyDisplay.setValues(mesh=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.meshOptions.setValues(
meshTechnique=OFF)
##
## Create job
##
mdb.Job(name='NlSkewPlate', model='Model-1',
description='Nonlinear Elastic Skew Plate. 20 kPa Load.')
a = mdb.models['Model-1'].rootAssembly
a.regenerate()
##
## Save model database
##
mdb.saveAs('NlSkewPlate.cae')
