FEA - Abaqus Scripting Interface

Abaqus Scripting Interface (ASI) is a Python-based scripting platform for Abaqus/CAE. Using this, you can simulate an entire problem, create macros, or create add-on modules. Generally Abaqus’s GUI is quite intuitive and we don’t think of working with ASI. However, when performing multiple scenarios and making use of complex assemblies - file size is one of the many benefits that ASI can help you with.

An example would be simulating mixed mode loading conditions using Arcan fixture and butterfly specimen. The specimen is required to be tested at different angles (different loading conditions), however overall setup remains the same. Now I can “save as” multiple instances of simulation results, each file may be about 20-30 MB each depending on the result variables selected.

In ASI I can create variables for each loading condition and simply edit the variable in the text file, then run the simulation. Text files are 2-3 KB each. Some of the benefits you will receive when using ASI are:

• Significantly smaller file size
• Quick variable changes compared to changes made using GUI
• Fewer distractions
• Quicker simulation times (compared to number of clicks required when using GUI)

An example of a butterfly specimen is given below using aluminium alloy AA2219. Note that this is for ASI demonstration purposes only, accuracy of the results is not verified here. Here are the steps to test the given script:

• Step 1: copy and paste the code in a word editor i.e. notepad
• Step 2: save the file with .py extension i.e. arcan.py
• Step 3: open Abaqus/CAE
• Step 4: click on File Menu
• Step 5: click on Run Script
• Step 6: find and select the file you just saved i.e. arcan.py
• Step 7: it will start the script and solve

################### CODE STARTS HERE ###################

from abaqus import*

from abaqusConstants import*

from caeModules import*

myModel = mdb.Model(name=’Arcan’)

import part

mySketch=myModel.ConstrainedSketch(name=’Profile’,sheetSize=62.5)

mySketch.Line(point1=(0,0), point2=(0,46))

mySketch.Line(point1=(0,46), point2=(62.5,46))

mySketch.Line(point1=(62.5,46), point2=(27.42893219,7.071067812))

mySketch.ArcByCenterEnds(center=(34.5,0),point1=(24.5,0),point2=(27.42893219,7.071067812),direction=CLOCKWISE)

mySketch.Line(point1=(24.5,0), point2=(0,0))

myArcan=myModel.Part(name=’arcan_sample’,dimensionality=THREE_D,type=DEFORMABLE_BODY)

myArcan.BaseSolidExtrude(sketch=mySketch,depth=5.0)

import material

myAluminium = myModel.Material(name=’AA2219′,description=’AA2219 from matweb.com’)

elasticProperties = (68.9E3,0.33)

myAluminium.Elastic(table=(elasticProperties,))

mdb.models['Arcan'].materials['AA2219'].Plastic(table=(

(138.07, 0.00),

(152.28, 0.01),

(175.66, 0.04),

(190.40, 0.07),

(202.35, 0.10),

(210.90, 0.12),

(217.50, 0.15),

(219.48, 0.16))?????????)

import section

mySection = myModel.HomogeneousSolidSection(name=’arcansection’,material=’AA2219′)

region = (myArcan.cells,)

myArcan.SectionAssignment(region=region,sectionName=’arcansection’)

import assembly

myAssembly = myModel.rootAssembly

myInstance = myAssembly.Instance(name=’arcanInstance’,part=myArcan,dependent=OFF)

import step

myModel.StaticStep(name=’Step1′,previous=’Initial’,timePeriod=1,initialInc=0.1)

import load

endFaceCenter = (10,0,2.5)

endFace = myInstance.faces.findAt((endFaceCenter,))

endRegion = (endFace,)

myModel.DisplacementBC(name=’Fixed’,createStepName=’Step1′,region=endRegion,u1=0.0,u2=0.0,u3=0.0)

topFaceCenter=(30,46,2.5)

topFace = myInstance.faces.findAt((topFaceCenter,))

topSurface = ((topFace,SIDE1),)

myModel.Pressure(name=’Pressure’,createStepName=’Step1′,region=topSurface,magnitude=-20)

import mesh

region=(myInstance.cells,)

elemType=mesh.ElemType(elemCode=C3D20R,elemLibrary=STANDARD)

myAssembly.setElementType(regions=region,elemTypes=(elemType,))

myAssembly.seedPartInstance(regions=(myInstance,),size=4.0)

myAssembly.generateMesh(regions=(myInstance,))

import job

jobName=’quarter_90_deg’

myJob=mdb.Job(name=jobName,model=’Arcan’)

myJob.submit()

myJob.waitForCompletion()

################### CODE ENDS HERE ###################