'''
-----------------------------------------------------------------------------
 Two dimensional submodel of a single edged notch specimen (linear
 elastic material) modeled using plane stress elements (CPS8).

 First the global model job is completed. The *.odb file from the global
 model is used to drive this submodel.

 Global model scripts to be run:
 2DSingleEdSymmGlCPS8_model.py and 2DSingleEdSymmGlCPS8_job.py
-----------------------------------------------------------------------------
'''

from abaqus import *
from abaqusConstants import *

import part, material, section, assembly, step, interaction
import regionToolset, displayGroupMdbToolset as dgm, mesh, load, job 

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

# Copy the global model into a new model

Mdb()
globalModelName = '2DSingleEdSymmGlCPS8'
openMdb(globalModelName)
subModelName = '2DSingleEdSymmSubCPS8'
mySubModel = mdb.Model(name=subModelName)

mySubModel = (mdb.Model(name=subModelName,
    objectToCopy=mdb.models[globalModelName]))
    
# Create a new viewport in which to display the model
# and the results of the analysis.

myAssembly = mySubModel.rootAssembly
myViewport = session.viewports['Viewport: 1']
myViewport.setValues(displayedObject=myAssembly)
myViewport.makeCurrent()
myViewport.maximize()

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

# Edit the model attributes to refer to the global model ODB file
# to drive the sub model.

mySubModel.setValues(description='Single edged notch specimen submodel', 
    globalJob='2DSingleEdSymmGlCPS8.odb')

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

# Create the sub model section of the global model

# Create a sketch for the base feature

myPlate = mySubModel.parts['Plate']
myViewport.setValues(displayedObject=myPlate)

mySubSketch = mySubModel.Sketch(name='plateProfile',sheetSize=200.0)
mySubSketch.sketchOptions.setValues(viewStyle=REGULAR)
mySubSketch.setPrimaryObject(option=STANDALONE)

mySubSketch.ArcByCenterEnds(center=(10.0,0.0), point1=(15.0,0.0),
    point2=(5.0,0.0), direction=COUNTERCLOCKWISE)
mySubSketch.Line(point1=(5.0,0.0), point2=(15.0,0.0))

mySubPlate = mySubModel.Part(name='subPlate', 
    dimensionality=TWO_D_PLANAR, type=DEFORMABLE_BODY)
mySubPlate.BaseShell(sketch=mySubSketch)
mySubSketch.unsetPrimaryObject()
del mySubModel.sketches['plateProfile']

myViewport.setValues(displayedObject=mySubPlate)

# Create a set referring to the whole part

faces = mySubPlate.faces.findAt(((10,2.5,0),))
mySubPlate.Set(faces=faces, name='subAll')

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

# Assign material properties

region = mySubPlate.sets['subAll']
mySubPlate.SectionAssignment(region=region,
    sectionName='SolidHomogeneous')

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

# Create an assembly
# Place the plate created above at the same position as in the
# global model. Then the instance of the full plate is deleted.

myViewport.setValues(displayedObject=myAssembly)
myAssembly.Instance(name='subPlate-1', part=mySubPlate, dependent=OFF)
mySubPlateInstance = myAssembly.instances['subPlate-1']
del myAssembly.features['myPlate-1']

# Partition the edge at t=0.5

pickedEdges = mySubPlateInstance.edges.findAt((9,0,0))
myAssembly.PartitionEdgeByParam(edges=pickedEdges, parameter=0.5)

# Delete all the sets/BCs/Loads/step/crack properties
# created for the global model

del myAssembly.sets['crackTip']
del myAssembly.sets['fixedEdge']
del myAssembly.sets['fixedPt']
del myAssembly.surfaces['loadSurf']
del mySubModel.steps['LoadPlate']
del myAssembly.engineeringFeatures.cracks['Crack']
del mySubModel.boundaryConditions['FixedInX']
del mySubModel.boundaryConditions['FixedInY']

# Create a set for the crack tip

verts = mySubPlateInstance.vertices
v1 = mySubPlateInstance.vertices.findAt((10,0,0))
verts1 = verts[v1.index:(v1.index+1)]
myAssembly.Set(vertices=verts1, name='subCrackTip')

# Create a set for the X edge of the plate

edges = mySubPlateInstance.edges
e1 = mySubPlateInstance.edges.findAt((12.5,0,0))
e1 = edges[e1.index:(e1.index+1)]
myAssembly.Set(edges=e1, name='subXEdge')

# Create a set for the sub modeling boundary

e1 = mySubPlateInstance.edges.findAt((10,5,0))
e1 = edges[e1.index:(e1.index+1)]
myAssembly.Set(edges=e1, name='drivenBoundary')

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

# Create a step

mySubModel.StaticStep(name='subApplyLoad', 
    previous='Initial', description='Drive the submodel')

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

# Create interaction properties

# Create the contour integral definition for the crack

crackFront = crackTip = myAssembly.sets['subCrackTip']
verts = mySubPlateInstance.vertices
v1 = mySubPlateInstance.vertices.findAt((10,0,0))
v2 = mySubPlateInstance.vertices.findAt((15,0,0))
myAssembly.engineeringFeatures.ContourIntegral(name='subCrack',
    symmetric=ON, crackFront=crackFront, crackTip=crackTip,
    extensionDirectionMethod=Q_VECTORS, qVectors=((v1,v2),),
    midNodePosition=0.25, collapsedElementAtTip=SINGLE_NODE)

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

# Create loads and boundary conditions 

# Create a boundary condition for X edge to be fixed in Y

region = myAssembly.sets['subXEdge']
mySubModel.DisplacementBC(name='subYFixed', createStepName='Initial',
    region=region, u2=SET, distribution=UNIFORM, localCsys=None)

# Create the sub modeling boundary condition

region = myAssembly.sets['drivenBoundary']
mySubModel.SubmodelBC(name='subBC', createStepName='subApplyLoad',
    region=region, globalStep='1', globalIncrement=0,
    timeScale=OFF, dof=(1, 2), globalDrivingRegion='', 
    absoluteExteriorTolerance=0.0, exteriorTolerance=0.05)

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

# Create a mesh 

# Seed all the edges

edges = mySubPlateInstance.edges
pickedEdges1 = mySubPlateInstance.edges.findAt((11,0,0))
pickedEdges2 = mySubPlateInstance.edges.findAt((9,0,0))
pickedEdges1 = edges[pickedEdges1.index:(pickedEdges1.index+1)]
pickedEdges2 = edges[pickedEdges2.index:(pickedEdges2.index+1)]
myAssembly.seedEdgeByBias(end1Edges=pickedEdges1,
    end2Edges=pickedEdges2, ratio=3.0, number=6, constraint=FIXED)

pickedEdges = mySubPlateInstance.edges.findAt((10,5,0))
pickedEdges = edges[pickedEdges.index:(pickedEdges.index+1)]
myAssembly.seedEdgeByNumber(edges=pickedEdges, number=12,
    constraint=FIXED)

# Assign meshing controls to the respective regions

faces = mySubPlateInstance.faces
f1 = mySubPlateInstance.faces.findAt((10,2.5,0))
pickedRegions = faces[f1.index:(f1.index+1)]
myAssembly.setMeshControls(regions=pickedRegions, elemShape=QUAD_DOMINATED,
    technique=SWEEP)
elemType1 = mesh.ElemType(elemCode=CPS8, elemLibrary=STANDARD)
elemType2 = mesh.ElemType(elemCode=CPS6M, elemLibrary=STANDARD)
faces1 = mySubPlateInstance.faces
pickedRegions =(faces1, )
myAssembly.setElementType(regions=pickedRegions,
    elemTypes=(elemType1, elemType2))
partInstances =(mySubPlateInstance, )
myAssembly.generateMesh(regions=partInstances)

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

# Request history output for the crack

mySubModel.historyOutputRequests.changeKey(fromName='H-Output-1',
    toName='JInt')
mySubModel.historyOutputRequests['JInt'].setValues(
    contourIntegral='subCrack', numberOfContours=5)
mySubModel.HistoryOutputRequest(name='StressInt',
    createStepName='subApplyLoad',
    contourIntegral='subCrack', numberOfContours=5,
    contourType=K_FACTORS)
mySubModel.HistoryOutputRequest(name='Tstr',
    createStepName='subApplyLoad',
    contourIntegral='subCrack', numberOfContours=5,
    contourType=T_STRESS)

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

# Create the job 

myJob = mdb.Job(name=subModelName, model=subModelName,
    description='Contour integral analysis')
mdb.saveAs(pathName=subModelName)

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