ae4131 abaqus lecture part i l.
Download
Skip this Video
Loading SlideShow in 5 Seconds..
AE4131 ABAQUS Lecture Part I PowerPoint Presentation
Download Presentation
AE4131 ABAQUS Lecture Part I

Loading in 2 Seconds...

play fullscreen
1 / 28

AE4131 ABAQUS Lecture Part I - PowerPoint PPT Presentation


  • 697 Views
  • Uploaded on

AE4131 ABAQUS Lecture Part I. Patrick Roberts gt0398b@prism.gatech.edu 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 ?.

loader
I am the owner, or an agent authorized to act on behalf of the owner, of the copyrighted work described.
capcha
Download Presentation

PowerPoint Slideshow about 'AE4131 ABAQUS Lecture Part I' - Jims


An Image/Link below is provided (as is) to download presentation

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.


- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -
Presentation Transcript
ae4131 abaqus lecture part i

AE4131ABAQUS LecturePart I

Patrick Roberts

gt0398b@prism.gatech.edu

x5-2773

Weber 201

overview
Overview
  • What is ABAQUS?
  • Why learn ABAQUS?
  • ABAQUS documentation and online resources
  • Solver structure
  • How to build a simple model
what is abaqus
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 abaqus4
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
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
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
Solver Structure

Command line

ABAQUS CAE

Standard

how to build a simple model
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
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 example10
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
Sketch out your FEA model

y, 2

20,000 lbs

4

5

2

3

1

x, 1

3

4

5

2

1

6

Nodes

Elements

pick your elements
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
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
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
To run ABAQUS
  • At the command line

abaqus job=filename

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

the results
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
A truss problem

y, 2

100 lbs

20 in.

x, 1

200 lbs

20 in.

Steel truss segments, Young’s modulus 30x106 lbs/in2

Diameter of each truss is 1 inch

beam example18
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 model19
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

5

3

4

2

1

1

4

2

6

5

3

Steel truss segments, Young’s modulus 30x106 lbs/in2

Diameter of each truss is 1 inch

pick your elements20
Pick your elements

(From ABAQUS documentation)

  • I’ll pick T3D2 2-node linear displacement
modal section
Modal Section

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

*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

history section
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
Looking at the results files

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

models with continuum elements
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.
3d cantilever beam model data
3D Cantilever Beam Model data

** 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

*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.

**

model section cont
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
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)