AE4131 ABAQUS Lecture Part I

1
AE4131ABAQUS LecturePart I

• Patrick Roberts
• gt0398b_at_prism.gatech.edu
• x5-2773
• Weber 201

2
Overview

• What is ABAQUS?
• Why learn ABAQUS?
• ABAQUS documentation and online resources
• Solver structure
• How to build a simple model

3
What is ABAQUS?

• The ABAQUS suite of software for finite element
  analysis (FEA) is known for its high performance,
  quality and ability to solve more kinds of
  challenging simulations than any other software.
• The ABAQUS suite consists of three core products
  ABAQUS/Standard, ABAQUS/Explicit and ABAQUS/CAE.
  Each of these packages offers additional optional
  modules that address specialized capabilities
  some customers may need.
• (From www.abaqus.com)

4
What is ABAQUS?

• ABAQUS/Standard, provides ABAQUS analysis
  technology to solve traditional implicit finite
  element analyses, such as static, dynamics,
  thermal, all powered with the widest range of
  contact and nonlinear material options.
  ABAQUS/Standard also has optional add-on and
  interface products with address design
  sensitivity analysis, offshore engineering, and
  integration with third party software, e.g.,
  plastic injection molding analysis.
• ABAQUS/Explicit, provides ABAQUS analysis
  technology focused on transient dynamics and
  quasi-static analyses using an explicit approach
  appropriate in many applications such as drop
  test, crushing and many manufacturing processes.
• ABAQUS/CAE, provides a complete modeling and
  visualization environment for ABAQUS analysis
  products. With direct access to CAD models,
  advanced meshing and visualization, and with an
  exclusive view towards ABAQUS analysis products,
  ABAQUS/CAE is the modeling environment of choice
  for many ABAQUS users.
• (From www.abaqus.com)

5
Why learn ABAQUS?

• Experience has shown that ABAQUS is the easiest
  FEA software package to learn.
• Very good online documentation
• Small learning curve which means you can model
  much faster.

6
ABAQUS documentation and online resources

• There are many online resources to help you find
  solutions.
• ABAQUS Documentation http//www.isye.gatech.edu/v6
  .4
• Newsgroup sci.engr.analysis
• ABAQUS Yahoo group
• Engineering Computing Services http//www.ecs.gate
  ch.edu

7
Solver Structure
Command line
ABAQUS CAE
Standard
8
How to build a simple model

• All models are called input files.
• An input file has two sections Model and History
  
• The Model section contains all the information
  about the model and comes before the history
  section.
• The History section is what you do to the model.
  You work on the model in Steps.
• Input files have a .inp extension and can be
  created in any ASCII (text) editor.

9
Beam example
y, 2
20,000 lbs
x, 1
Steel beam, Youngs modulus 30x106 lbs/in2
Length 100 inches, width 1 inch, height 2
inches
10
Beam example

• I want to know stresses and strains along the
  x-direction and the forces and moments in each
  section of the beam due to a static load.

11
Sketch out your FEA model
y, 2
20,000 lbs
4
2
3
5
1
x, 1
3
4
5
1
2
6
Nodes Elements
12
Pick your elements

• ABAQUS has a large library of elements
• (From ABAQUS documentation)
• Ill pick B31 2-node linear beam

13
Simple Input file (Model data)

• HEADING
• CANTILEVER BEAM
• This is in inches
• NODE
• 1, 0.
• 6, 100.
• NGEN, NSETallnodes
• 1, 6
• ELEMENT, TYPEB31
• 1, 1, 2
• ELGEN, ELSETBEAM
• 1, 5
• BEAM SECTION, SECTIONRECTANGULAR, ELSETBEAM,
  MATERIALSTEEL
• 1., 2.
• MATERIAL, NAMESTEEL
• ELASTIC
• 30.E6,

14
Simple Input file (History Section)

• STEP, PERTURBATION
• STATIC
• The load is in pounds
• CLOAD
• 6, 2, -20000.
• EL PRINT, POSITIONAVERAGED AT NODES,
  SUMMARYYES
• S11, E11
• SF,
• NODE FILE, NSETallnodes
• U, CF, RF
• OUTPUT, FIELD, VARIABLEPRESELECT
• ELEMENT OUTPUT
• SF,
• OUTPUT, HISTORY
• NODE OUTPUT, NSETallnodes
• U, CF, RF
• END STEP

15
To run ABAQUS

• At the command line
• abaqus jobfilename

Use the Input File filename WITHOUT the file
extension (.inp)
16
The results

• You will get many files after your job is
  complete.
• .dat Contains results information you can read.
  Very important for debugging.
• .fil Only for the computer
• .com Only for the computer
• .odb Only for the computer but will be used by
  CAE
• .msg Contains information you can read about how
  the job ran. Can be important for debugging.
• .prt Only for the computer
• .sta Contains information you can read about the
  status of the job while running
• .log Contains information you can read about how
  the job ran. Can be important for debugging.

17
A truss problem
y, 2
100 lbs
20 in.
x, 1
200 lbs
20 in.
Steel truss segments, Youngs modulus 30x106
lbs/in2 Diameter of each truss is 1 inch
18
Beam example

• I want to know stresses and strains in all truss
  segments due to the static loads shown in the
  figure.

19
Sketch out your FEA model
y, 2
10
8
9
12
7
10
11
8
9
6
7
15
12
13
14
11
16
17
19
18
20
x, 1
3
5
4
2
1
2
4
1
5
6
3
Steel truss segments, Youngs modulus 30x106
lbs/in2 Diameter of each truss is 1 inch
20
Pick your elements

• (From ABAQUS documentation)
• Ill pick T3D2 2-node linear displacement

21
Modal Section

• HEADING
• CANTILEVER BEAM
• This is in inches
• NODE
• 1, 0., 0.
• 6, 100., 0.
• 7, 0., 20.
• 12, 100., 20.
• NSET, NSETFIXED
• 1, 7
• NGEN, NSETallnodes
• 1, 6
• 7, 12
• ELEMENT, TYPET3D2, ELSETBEAM
• 1, 1, 2
• 2, 2, 3
• 3, 3, 4

8, 9, 10 9, 10, 11 10, 11, 12 11, 1, 8 12,
2, 9 13, 3, 10 14, 4, 11 15, 5, 12 16, 6, 12
17, 2, 8 18, 3, 9 19, 4, 10 20, 5, 11 SOLID
SECTION, ELSETBEAM, MATERIALSTEEL
1., MATERIAL, NAMESTEEL ELASTIC
30.E6, BOUNDARY FIXED, ENCASTRE
22
History Section

• STEP, PERTURBATION
• STATIC
• The load is in pounds
• CLOAD
• 6, 1, 200.
• 12, 2, -100,
• EL PRINT, POSITIONAVERAGED AT NODES,
  SUMMARYYES
• S, E
• NODE FILE, NSETallnodes
• U, CF, RF
• OUTPUT, FIELD, VARIABLEPRESELECT
• ELEMENT OUTPUT
• S, E
• OUTPUT, HISTORY
• NODE OUTPUT, NSETallnodes
• U, CF, RF
• END STEP

23
Looking at the results files

• Starting with the .log file you should review the
  results files.

24
Models with continuum elements

• To model most 3D structures that are bending
  Continuum or brick elements are the best.
• Each element requires any nodes.
• Models can be made by hand rather than CAE but
  can take much longer.

25
Continuum Elements
26
3D Cantilever Beam Model data

• HEADING
• cantilever beam
• Coordinates are in inches
• NODE
• 1, 0.,0.,0.
• 193, 0.,0.,24.
• 1601, 2.,0.,0.
• 1793, 2.,0.,24.
• 8001, 0.,0.5,0.
• 8193, 0.,0.5,24.
• 9601, 2.,0.5,0.
• 9793, 2.,0.5,24.

Create nodes for beam NGEN,NSETFIX1
1,1601,200 NGEN,NSETFIX2 8001,9601,200 NFILL,N
SETFIX FIX1,FIX2,4,2000 NGEN,NSETEND1
193,1793,200 NGEN,NSETEND2 8193,9793,200 NFILL
,NSETEND END1,END2,4,2000 NFILL,NSETCBEAM
FIX,END,192,1 NSET, NSETSENSOR 8993
27
Model section (cont.)

• Make master elements for beam
• ELEMENT,TYPEC3D20R
• 1, 1,401,4401,4001, 5,405,4405,4005,
  201,2401,4201,2001, 205,2405,4205,2005,
  3,403,4403,4003
• Create elements for beam
• ELGEN,ELSETCBEAM
• 1,4,400,1,48,4,10,2,4000,2000
• ELSET, ELSETLOCSTRESS
• 2,3,12,22,32,42,52,62,13,23,33,43,53,63,2002,2003
  
• 2012,2022,2032,2042,2052,2062,2013,2023,2033,2043
  ,2053,2063
• Material properties for steel
• SOLID SECTION, MATERIALSTEEL, ELSETCBEAM
• MATERIAL, NAMESTEEL

28
Student Accounts

• Now you are ready to work the projects.
• You can use your AE student account in the AE
  Computer Lab (Knight 318) to run ABAQUS on these
  systems.
• Or you can get an account on the ECS network (go
  to http//www.ecs.gatech.edu)