Transcript AE4131 Lecture ABAQUS Part I

AE4131
ABAQUS Lecture
Part I
Patrick Roberts
[email protected]
x5-2773
Weber 201
Overview
• What is ABAQUS?
• Why learn ABAQUS?
• ABAQUS documentation and online
resources
• Solver structure
• How to build a simple model
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)
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)
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.
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.gatech.edu
Solver Structure
Command
line
ABAQUS
CAE
Standard
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.
Beam example
y, 2
20,000 lbs
x, 1
Steel beam, Young’s modulus 30x106 lbs/in2
Length 100 inches, width = 1 inch, height = 2 inches
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.
Sketch out your FEA model
y, 2
20,000 lbs
2
1
1
4
3
2
Nodes
Elements
3
5
4
5
6
x, 1
Pick your elements
• ABAQUS has a large library of elements
(From ABAQUS documentation)
• I’ll pick B31 2-node linear beam
Simple Input file (Model data)
*HEADING
CANTILEVER BEAM
**
** This is in inches
**
*NODE
1, 0.
6, 100.
*NGEN, NSET=allnodes
1, 6
*ELEMENT, TYPE=B31
1, 1, 2
*ELGEN, ELSET=BEAM
1, 5
*BEAM SECTION, SECTION=RECTANGULAR, ELSET=BEAM, MATERIAL=STEEL
1., 2.
*MATERIAL, NAME=STEEL
*ELASTIC
30.E6,
*BOUNDARY
1, ENCASTRE
Simple Input file (History Section)
*STEP, PERTURBATION
*STATIC
**
** The load is in pounds
**
*CLOAD
6, 2, -20000.
*EL PRINT, POSITION=AVERAGED AT NODES, SUMMARY=YES
S11, E11
SF,
*NODE FILE, NSET=allnodes
U, CF, RF
*OUTPUT, FIELD, VARIABLE=PRESELECT
*ELEMENT OUTPUT
SF,
*OUTPUT, HISTORY
*NODE OUTPUT, NSET=allnodes
U, CF, RF
*END STEP
To run ABAQUS
• At the command line
abaqus job=filename
Use the Input File
filename
WITHOUT the file
extension (.inp)
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.
A truss problem
y, 2
20 in.
100 lbs
x, 1
20 in.
Steel truss segments, Young’s modulus 30x106 lbs/in2
Diameter of each truss is 1 inch
200 lbs
Beam example
I want to know stresses and strains in all
truss segments due to the static loads
shown in the figure.
Sketch out your FEA model
y, 2
7
8
6
7
12
11
17
1
1
9
8
13
2
9
3
3
11
12
16
20
4
4
x, 1
5
Steel truss segments, Young’s modulus 30x106 lbs/in2
Diameter of each truss is 1 inch
10
15
14
19
18
2
10
5
6
Pick your elements
(From ABAQUS documentation)
• I’ll pick T3D2 2-node linear displacement
Modal Section
*HEADING
CANTILEVER BEAM
**
** This is in inches
**
*NODE
1, 0., 0.
6, 100., 0.
7, 0., 20.
12, 100., 20.
*NSET, NSET=FIXED
1, 7
*NGEN, NSET=allnodes
1, 6
7, 12
*ELEMENT, TYPE=T3D2, ELSET=BEAM
1, 1, 2
2, 2, 3
3, 3, 4
4, 4, 5
5, 5, 6
6, 7, 8
7, 8, 9
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, ELSET=BEAM,
MATERIAL=STEEL
1.,
*MATERIAL, NAME=STEEL
*ELASTIC
30.E6,
*BOUNDARY
FIXED, ENCASTRE
History Section
*STEP, PERTURBATION
*STATIC
**
** The load is in pounds
**
*CLOAD
6, 1, 200.
12, 2, -100,
*EL PRINT, POSITION=AVERAGED AT NODES, SUMMARY=YES
S, E
*NODE FILE, NSET=allnodes
U, CF, RF
*OUTPUT, FIELD, VARIABLE=PRESELECT
*ELEMENT OUTPUT
S, E
*OUTPUT, HISTORY
*NODE OUTPUT, NSET=allnodes
U, CF, RF
*END STEP
Looking at the results files
Starting with the .log file you should review
the results files.
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.
Continuum Elements
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,NSET=FIX1
1,1601,200
*NGEN,NSET=FIX2
8001,9601,200
*NFILL,NSET=FIX
FIX1,FIX2,4,2000
*NGEN,NSET=END1
193,1793,200
*NGEN,NSET=END2
8193,9793,200
*NFILL,NSET=END
END1,END2,4,2000
*NFILL,NSET=CBEAM
FIX,END,192,1
**
*NSET, NSET=SENSOR
8993
Model section (cont.)
**
** Make master elements for beam
**
*ELEMENT,TYPE=C3D20R
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,ELSET=CBEAM
1,4,400,1,48,4,10,2,4000,2000
*ELSET, ELSET=LOCSTRESS
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, MATERIAL=STEEL, ELSET=CBEAM
*MATERIAL, NAME=STEEL
**
** Youngs modulus is in lbf/in^2
**
*ELASTIC
29.E6,0.3
**
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)