#
# Getting Started with Abaqus: Interactive Edition
#
# Script for rubber mount example
#
from abaqus import *
from abaqusConstants import *
session.viewports['Viewport: 1'].makeCurrent()
session.viewports['Viewport: 1'].maximize()
session.journalOptions.setValues(replayGeometry=COORDINATE,
recoverGeometry=COORDINATE)
from caeModules import *
from driverUtils import executeOnCaeStartup
executeOnCaeStartup()
Mdb()
##
## Sketch profile of the mount
##
s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__', sheetSize=0.3)
g, v, d, c = s.geometry, s.vertices, s.dimensions, s.constraints
s.sketchOptions.setValues(decimalPlaces=3, viewStyle=AXISYM)
s.setPrimaryObject(option=STANDALONE)
s.ConstructionLine(point1=(0.0, -100.0), point2=(0.0, 100.0))
s.FixedConstraint(entity=g[2])
mdb.models['Model-1'].sketches['__profile__'].sketchOptions.setValues(
gridFrequency=4)
s.rectangle(point1=(0.01, 0.0), point2=(0.025, 0.01))
s.DistanceDimension(entity1=g[2], entity2=v[0],
textPoint=(0.00998260825872421, -0.00830297358334064), value=0.01)
s.VerticalDimension(vertex1=v[0], vertex2=v[1], textPoint=(0.0,
0.00851448811590672), value=0.03)
s.ObliqueDimension(vertex1=v[0], vertex2=v[3],
textPoint=(0.025699570775032, -0.00830297358334064), value=0.05)
s.CircleByCenterPerimeter(center=(0.085, 0.025),
point1=(0.06, 0.00740899052470922))
s.CoincidentConstraint(entity1=v[5], entity2=g[5])
s.DistanceDimension(entity1=g[2], entity2=v[4],
textPoint=(0.0811913833022118, -0.023865295574069), value=0.1)
s.VerticalDimension(vertex1=v[2], vertex2=v[4],
textPoint=(0.115524396300316, 0.0262394621968269), value=0.0)
s.ObliqueDimension(vertex1=v[5], vertex2=v[3],
textPoint=(0.0519323498010635, 0.0), value=0.005)
s.autoTrimCurve(curve1=g[7], point1=(0.124150268733501, -0.00965208746492863))
s.autoTrimCurve(curve1=g[5], point1=(0.0601795427501202, 0.020298857241869))
s.autoTrimCurve(curve1=g[4], point1=(0.0557677671313286, 0.0308697782456875))
s.RadialDimension(curve=g[8],
textPoint=(0.0725325122475624, 0.0207393132150173),
radius=0.047169905660283)
d[6].setValues(reference=ON)
session.viewports['Viewport: 1'].view.fitView()
p = mdb.models['Model-1'].Part(name='Mount', dimensionality=AXISYMMETRIC,
type=DEFORMABLE_BODY)
p = mdb.models['Model-1'].parts['Mount']
p.BaseShell(sketch=s)
s.unsetPrimaryObject()
session.viewports['Viewport: 1'].setValues(displayedObject=p)
del mdb.models['Model-1'].sketches['__profile__']
##
## Create material 'Rubber'
##
mdb.models['Model-1'].Material('Rubber')
mdb.models['Model-1'].materials['Rubber'].Hyperelastic(type=POLYNOMIAL,
table=())
mdb.models['Model-1'].materials['Rubber'].hyperelastic.UniaxialTestData(table=((
0.054E6, 0.0380), (0.152E6, 0.1338), (0.254E6, 0.2210), (0.362E6, 0.3450),
(0.459E6, 0.4600), (0.583E6, 0.6242), (0.656E6, 0.8510), (0.730E6,
1.4268)))
mdb.models['Model-1'].materials['Rubber'].hyperelastic.BiaxialTestData(table=((
0.089E6, 0.0200), (0.255E6, 0.1400), (0.503E6, 0.4200), (0.958E6, 1.4900),
(1.703E6, 2.7500), (2.413E6, 3.4500)))
mdb.models['Model-1'].materials['Rubber'].hyperelastic.PlanarTestData(table=((
0.055E6, 0.0690), (0.324E6, 0.2828), (0.758E6, 1.3862), (1.269E6, 3.0345),
(1.779E6, 4.0621)))
##
## Create material 'Steel'
##
mdb.models['Model-1'].Material('Steel')
mdb.models['Model-1'].materials['Steel'].Elastic(table=((200.E9, 0.3), ))
##
## Create solid sections for the rubber and steel
##
mdb.models['Model-1'].HomogeneousSolidSection(name='RubberSection',
material='Rubber', thickness=1.0)
mdb.models['Model-1'].HomogeneousSolidSection(name='SteelSection',
material='Steel', thickness=1.0)
##
## Partition the part into two regions (rubber and steel regions)
##
f, e, d = p.faces, p.edges, p.datums
t = p.MakeSketchTransform(
sketchPlane=f.findAt(coordinates=(0.043333, 0.001667, 0.0),
normal=(0.0, 0.0, 1.0)), sketchPlaneSide=SIDE1,
origin=(0.033052, 0.014514, 0.0))
s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',
sheetSize=0.134, gridSpacing=0.003, transform=t)
g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints
s.sketchOptions.setValues(decimalPlaces=3)
s.setPrimaryObject(option=SUPERIMPOSE)
p.projectReferencesOntoSketch(sketch=s, filter=COPLANAR_EDGES)
s.Line(point1=(0.026948, -0.009514), point2=(-0.03, -0.009514))
s.HorizontalConstraint(entity=g.findAt((-0.001526, -0.009514)))
s.PerpendicularConstraint(entity1=g.findAt((0.026948, -0.012014)),
entity2=g.findAt((-0.001526, -0.009514)))
pickedFaces = f.findAt(((0.043333, 0.001667, 0.0), ))
p.PartitionFaceBySketch(faces=pickedFaces, sketch=s)
s.unsetPrimaryObject()
del mdb.models['Model-1'].sketches['__profile__']
##
## Assign rubber section
##
p = mdb.models['Model-1'].parts['Mount']
f = p.faces
faces = f.findAt(((0.042303, 0.006937, 0.0), ))
region = regionToolset.Region(faces=faces)
p.SectionAssignment(region=region, sectionName='RubberSection', offset=0.0)
##
## Assign steel section
##
faces = f.findAt(((0.043333, 0.003333, 0.0), ))
region = regionToolset.Region(faces=faces)
p.SectionAssignment(region=region, sectionName='SteelSection', offset=0.0)
a = mdb.models['Model-1'].rootAssembly
session.viewports['Viewport: 1'].setValues(displayedObject=a)
##
## Set coordinate system (done by default)
##
a.DatumCsysByDefault(CARTESIAN)
##
## Instance the mount
##
p = mdb.models['Model-1'].parts['Mount']
a.Instance(name='Mount-1', part=p, dependent=ON)
##
## Create geometry set 'Middle'
##
e = a.instances['Mount-1'].edges
edges = e.findAt(((0.020708, 0.03, 0.0), ))
a.Set(edges=edges, name='Middle')
##
## Create geometry set 'Out'
##
v = a.instances['Mount-1'].vertices
verts = v.findAt(((0.01, 0.0, 0.0), ))
a.Set(vertices=verts, name='Out')
##
## Create surface 'Bottom'
##
s = a.instances['Mount-1'].edges
side1Edges = s.findAt(((0.0475, 0.0, 0.0), ))
a.Surface(side1Edges=side1Edges, name='Bottom')
##
## Create a static general step
##
mdb.models['Model-1'].StaticStep(name='Compress mount', previous='Initial',
description='Apply axial pressure load to mount', timePeriod=1,
adiabatic=OFF, maxNumInc=100, stabilization=None,
timeIncrementationMethod=AUTOMATIC,
initialInc=0.01, minInc=1e-05, maxInc=1, matrixSolver=SOLVER_DEFAULT,
amplitude=RAMP, extrapolation=LINEAR, fullyPlastic="", nlgeom=ON)
session.viewports['Viewport: 1'].assemblyDisplay.setValues(
step='Compress mount')
##
## Modify output requests
##
mdb.models['Model-1'].fieldOutputRequests['F-Output-1'].setValues(
variables=('S', 'PE', 'PEEQ', 'PEMAG', 'NE', 'LE', 'U', 'RF',
'CF', 'CSTRESS', 'CDISP'))
regionDef=a.sets['Out']
mdb.models['Model-1'].HistoryOutputRequest(name='H-Output-1',
createStepName='Compress mount', variables=('U1', 'U2', 'U3'),
region=regionDef)
session.viewports['Viewport: 1'].assemblyDisplay.setValues(loads=ON, bcs=ON,
predefinedFields=ON)
##
## Apply pressure load
##
region = a.surfaces['Bottom']
mdb.models['Model-1'].Pressure(name='Pressure',
createStepName='Compress mount', region=region, magnitude=500000.0)
##
## Apply symmetry bc to set "Middle'
##
region = a.sets['Middle']
mdb.models['Model-1'].DisplacementBC(name='Symmetry',
createStepName='Compress mount', region=region, u2=0.0)
##
## Suppress visibility of datum geometry
##
session.viewports['Viewport: 1'].assemblyDisplay.geometryOptions.setValues(
geometryEdgesInShaded=OFF, datumPoints=OFF, datumAxes=OFF, datumPlanes=OFF,
datumCoordSystems=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.setValues(mesh=ON, loads=OFF,
bcs=OFF, predefinedFields=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.meshOptions.setValues(
meshTechnique=ON)
##
## Assign edge seeds
##
p = mdb.models['Model-1'].parts['Mount']
e = p.edges
pickedEdges = e.findAt(((0.0225, 0.005, 0.0), ), ((0.0475, 0.0, 0.0), ),
((0.020708, 0.03, 0.0), ))
p.seedEdgeByNumber(edges=pickedEdges, number=30)
pickedEdges = e.findAt(((0.053289, 0.023434, 0.0), ), ((0.01, 0.01125, 0.0), ))
p.seedEdgeByNumber(edges=pickedEdges, number=14)
pickedEdges = e.findAt(((0.01, 0.00125, 0.0), ), ((0.06, 0.00375, 0.0), ))
p.seedEdgeByNumber(edges=pickedEdges, number=1)
##
## Use structured meshing
##
f = p.faces
pickedRegions = f
p.setMeshControls(regions=pickedRegions, technique=STRUCTURED)
##
## Assign element type to the rubber
##
elemType1 = mesh.ElemType(elemCode=CAX4H, elemLibrary=STANDARD)
elemType2 = mesh.ElemType(elemCode=CAX3, elemLibrary=STANDARD)
faces = f.findAt(((0.042303, 0.006937, 0.0), ))
pickedRegions =(faces, )
p.setElementType(regions=pickedRegions, elemTypes=(elemType1, elemType2))
##
## Assign element type to the steel
##
elemType1 = mesh.ElemType(elemCode=CAX4I, elemLibrary=STANDARD)
elemType2 = mesh.ElemType(elemCode=CAX3, elemLibrary=STANDARD)
faces = f.findAt(((0.043333, 0.003333, 0.0), ))
pickedRegions =(faces, )
p.setElementType(regions=pickedRegions, elemTypes=(elemType1, elemType2))
##
## Generate mesh
##
p.generateMesh()
session.viewports['Viewport: 1'].assemblyDisplay.setValues(mesh=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.meshOptions.setValues(
meshTechnique=OFF)
##
## Create job
##
mdb.Job(name='Mount', model='Model-1',
description='Axisymmetric mount analysis under axial loading',
modelPrint=ON)
a = mdb.models['Model-1'].rootAssembly
a.regenerate()
##
## Save model database
##
mdb.saveAs('Mount')
