1. AE4131 ABAQUS Lecture Part I
Patrick Roberts
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

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

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
Newsgroup sci.engr.analysis
ABAQUS Yahoo group
Engineering Computing Services

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, Young’s 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
20,000 lbs 2 3 4 1 5
x, 1 1 2 3 4 5 6
Nodes
Elements

12. Pick your elements ABAQUS has a large library of elements
(From ABAQUS documentation)
I’ll 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, 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

14. Simple Input file (History Section)
*STEP, PERTURBATION
*STATIC **
** The load is in pounds
*CLOAD
6, 2,
*EL PRINT, POSITION=AVERAGED AT NODES, SUMMARY=YES
S11, E11
SF,
*NODE FILE, NSET=allnodes
U, CF, RF
*OUTPUT, FIELD, VARIABLE=PRESELECT
*ELEMENT OUTPUT
*OUTPUT, HISTORY
*NODE OUTPUT, NSET=allnodes
*END STEP

15. Use the Input File filename WITHOUT the file extension (.inp)
To run ABAQUS
At the command line
abaqus job=filename
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, Young’s 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 model6 8 7 8 9 10 9 11 10 12 7 11 12 13 14 15 16 17 18 19 20
x, 1 1 1 2 2 3 4 5 4 3 5 6
Steel truss segments, Young’s modulus 30x106 lbs/in2
Diameter of each truss is 1 inch

20. Pick your elements I’ll pick T3D2 2-node linear displacement
(From ABAQUS documentation)
I’ll pick T3D2 2-node linear displacement

21. Modal Section *HEADING 8, 9, 10 CANTILEVER BEAM 9, 10, 11 **
** 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

22. 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
*OUTPUT, HISTORY
*NODE OUTPUT, NSET=allnodes
*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.
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

27. 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

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