#! /user/bin/python
# coding:utf-8
from abaqus import *
import testUtils
testUtils.setBackwardCompatibility()
from abaqusConstants import *
myModel = mdb.Model(name = 'Beam')
print '创建新视窗来显示模型和分析结果'
myViewport = session.Viewport(name = 'Cantilever Beam Example',
origin = (20,20), width = 150 , height = 120)
myViewport.makeCurrent()
myViewport.maximize()
print '导入part模块'
import part
print '创建基础特征的草图'
mySketch = myModel.ConstrainedSketch(name = 'beamProfile',sheetSize = 250.)
print '绘制矩形截面'
mySketch.rectangle(point1 = (-100,10),point2 = (100,-10))
print '创建三维变形体部件'
myBeam = myModel.Part(name = 'Beam',dimensionality = THREE_D,type = DEFORMABLE_BODY)
print '通过对草图拉伸25.0来创建部件'
myBeam.BaseSolidExtrude(sketch = mySketch,depth = 25.0)
print '导入material模块'
import material
print '创建材料'
mySteel = myModel.Material(name = 'Steel')
print '定义弹性材料属性，杨氏模量209.E3，泊松比0.3'
elasticProperties = (209.E3,0.3)
mySteel.Elastic(table = (elasticProperties,))
print '导入section模块'
import section
print '创建实体截面'
mySection = myModel.HomogeneousSolidSection(name = 'beamSection',
material = 'Steel',thickness = 1.0)
print '为部件分配截面属性'
region = (myBeam.cells,)
myBeam.SectionAssignment(region = region,sectionName = 'beamSection')
print '导入assembly模块'
import assembly
print '创建部件实例'
myAssembly = myModel.rootAssembly
myInstance = myAssembly.Instance(name = 'beamInstance',part = myBeam,dependent = OFF)
print '导入step模块'
import step
print '在初始分析步initial之后创建一个分析步，静力分析步的时间为1.0，初始增量为0.1'
myModel.StaticStep(name = 'beamLoad',previous = 'Initial',timePeriod = 1.0,
initialInc = 0.1,description = 'Load the top of the beam.')
print '导入Load模块'
import load
print '通过坐标找出端部所在面'
endFaceCenter = (-100,0,12.5)
endFace = myInstance.faces.findAt((endFaceCenter,))
print '在梁端部创建固定端约束'
endRegion = (endFace,)
myModel.EncastreBC(name = 'Fixed',createStepName = 'beamLoad',region = endRegion)
print '通过坐标找到上面'
topFaceCenter = (0,10,12.5)
topFace = myInstance.faces.findAt((topFaceCenter,))
print '在梁的上表面施加压力荷载'
topSurface = ((topFace,SIDE1),)
myModel.Pressure(name = 'Pressure',createStepName = 'beamLoad',
region = topSurface,magnitude = 0.5)
print '导入mesh模块'
import mesh
print '为部件实例指定单元类型'
region = (myInstance.cells,)
elemType = mesh.ElemType(elemCode = C3D8I,elemLibrary = STANDARD)
myAssembly.setElementType(regions = region,elemTypes = (elemType,0))
print '为部件实例撒种子'
myAssembly.seedPartInstance(regions = (myInstance,),size = 10.0)
print '为部件实例划分网格'
myAssembly.generateMesh(regions = (myInstance,))
print '显示划分网格后的梁模型'
myViewport.assemblyDisplay.setValues(mesh = ON)
myViewport.assemblyDisplay.meshOptions.setValues(meshTechnique = ON)
myViewport.setValues(displayedObject = myAssembly)
print '导入job模块'
import job
print '为模型创建并提交分析作业'
jobName = 'beam_tutorial'
myJob = mdb.Job(name = jobName,model = 'Beam',
description = 'Cantilever beam tutorial')
print '等待分析作业完成'
myJob.submit()
myJob.waitForCompletion()
print '分析完成，进入后处理'
print '导入visualization模块'
import visualization
print '打开输出数据库，显示默认云图'
myOdb = visualization.openOdb(path = jobName+'.odb')
myViewport.setValues(displayedObject = myOdb)
myViewport.odbDisplay.display.setValues(plotState = CONTOURS_ON_DEF)
myViewport.odbDisplay.commonOptions.setValues(renderStyle = FILLED)
print '将Mises云图输出为png文件'
session.printToFile(fileName = 'Mises',format = PNG,canvasObjects = (myViewport,))
print '文件Mises.png保存于工作目录，请查看'
