ABAQUS Lecture Part I

42,276 views

Published on

Published in: Education, Technology, Business
8 Comments
64 Likes
Statistics
Notes
No Downloads
Views
Total views
42,276
On SlideShare
0
From Embeds
0
Number of Embeds
316
Actions
Shares
0
Downloads
0
Comments
8
Likes
64
Embeds 0
No embeds

No notes for slide

ABAQUS Lecture Part I

  1. 1. AE4131 ABAQUS Lecture Part I Patrick Roberts [email_address] x5-2773 Weber 201
  2. 2. Overview <ul><li>What is ABAQUS ? </li></ul><ul><li>Why learn ABAQUS ? </li></ul><ul><li>ABAQUS documentation and online resources </li></ul><ul><li>Solver structure </li></ul><ul><li>How to build a simple model </li></ul>
  3. 3. What is ABAQUS ? <ul><li>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. </li></ul><ul><li>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. </li></ul><ul><li>(From www.abaqus.com) </li></ul>
  4. 4. What is ABAQUS ? <ul><li>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. </li></ul><ul><li>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. </li></ul><ul><li>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. </li></ul><ul><li>(From www.abaqus.com) </li></ul>
  5. 5. Why learn ABAQUS ? <ul><li>Experience has shown that ABAQUS is the easiest FEA software package to learn. </li></ul><ul><li>Very good online documentation </li></ul><ul><li>Small learning curve which means you can model much faster. </li></ul>
  6. 6. ABAQUS documentation and online resources <ul><li>There are many online resources to help you find solutions. </li></ul><ul><li>ABAQUS Documentation http://www.isye.gatech.edu/v6.4 </li></ul><ul><li>Newsgroup sci.engr.analysis </li></ul><ul><li>ABAQUS Yahoo group </li></ul><ul><li>Engineering Computing Services http://www.ecs.gatech.edu </li></ul>
  7. 7. Solver Structure Standard Command line ABAQUS CAE
  8. 8. How to build a simple model <ul><li>All models are called input files . </li></ul><ul><li>An input file has two sections; Model and History </li></ul><ul><li>The Model section contains all the information about the model and comes before the history section. </li></ul><ul><li>The History section is what you do to the model. You work on the model in Steps . </li></ul><ul><li>Input files have a . inp extension and can be created in any ASCII (text) editor. </li></ul>
  9. 9. Beam example 20,000 lbs Steel beam, Young’s modulus 30x10 6 lbs/in 2 Length 100 inches, width = 1 inch, height = 2 inches x, 1 y, 2
  10. 10. Beam example <ul><li>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. </li></ul>
  11. 11. Sketch out your FEA model 20,000 lbs x, 1 y, 2 1 2 3 4 5 6 1 2 3 4 5 Nodes Elements
  12. 12. <ul><li>ABAQUS has a large library of elements </li></ul><ul><li>(From ABAQUS documentation) </li></ul><ul><li>I’ll pick B31 2-node linear beam </li></ul>Pick your elements
  13. 13. Simple Input file ( Model data) <ul><li>*HEADING </li></ul><ul><li>CANTILEVER BEAM </li></ul><ul><li>** </li></ul><ul><li>** This is in inches </li></ul><ul><li>** </li></ul><ul><li>*NODE </li></ul><ul><li>1, 0. </li></ul><ul><li>6, 100. </li></ul><ul><li>*NGEN, NSET=allnodes </li></ul><ul><li>1, 6 </li></ul><ul><li>*ELEMENT, TYPE=B31 </li></ul><ul><li>1, 1, 2 </li></ul><ul><li>*ELGEN, ELSET=BEAM </li></ul><ul><li>1, 5 </li></ul><ul><li>*BEAM SECTION, SECTION=RECTANGULAR, ELSET=BEAM, MATERIAL=STEEL </li></ul><ul><li>1., 2. </li></ul><ul><li>*MATERIAL, NAME=STEEL </li></ul><ul><li>*ELASTIC </li></ul><ul><li>30.E6, </li></ul><ul><li>*BOUNDARY </li></ul><ul><li>1, ENCASTRE </li></ul>
  14. 14. Simple Input file ( History Section) <ul><li>*STEP, PERTURBATION </li></ul><ul><li>*STATIC </li></ul><ul><li>** </li></ul><ul><li>** The load is in pounds </li></ul><ul><li>** </li></ul><ul><li>*CLOAD </li></ul><ul><li>6, 2, -20000. </li></ul><ul><li>*EL PRINT, POSITION=AVERAGED AT NODES, SUMMARY=YES </li></ul><ul><li>S11, E11 </li></ul><ul><li>SF, </li></ul><ul><li>*NODE FILE, NSET=allnodes </li></ul><ul><li>U, CF, RF </li></ul><ul><li>*OUTPUT, FIELD, VARIABLE=PRESELECT </li></ul><ul><li>*ELEMENT OUTPUT </li></ul><ul><li>SF, </li></ul><ul><li>*OUTPUT, HISTORY </li></ul><ul><li>*NODE OUTPUT, NSET=allnodes </li></ul><ul><li>U, CF, RF </li></ul><ul><li>*END STEP </li></ul>
  15. 15. To run ABAQUS <ul><li>At the command line </li></ul><ul><li>abaqus job=filename </li></ul>Use the Input File filename WITHOUT the file extension (.inp)
  16. 16. The results <ul><li>You will get many files after your job is complete. </li></ul><ul><li>.dat Contains results information you can read. Very important for debugging. </li></ul><ul><li>.fil Only for the computer </li></ul><ul><li>.com Only for the computer </li></ul><ul><li>.odb Only for the computer but will be used by CAE </li></ul><ul><li>.msg Contains information you can read about how the job ran. Can be important for debugging. </li></ul><ul><li>.prt Only for the computer </li></ul><ul><li>.sta Contains information you can read about the status of the job while running </li></ul><ul><li>.log Contains information you can read about how the job ran. Can be important for debugging. </li></ul>
  17. 17. A truss problem 200 lbs 100 lbs x, 1 y, 2 Steel truss segments, Young’s modulus 30x10 6 lbs/in 2 Diameter of each truss is 1 inch 20 in. 20 in.
  18. 18. Beam example <ul><li>I want to know stresses and strains in all truss segments due to the static loads shown in the figure. </li></ul>
  19. 19. Sketch out your FEA model x, 1 y, 2 Steel truss segments, Young’s modulus 30x10 6 lbs/in 2 Diameter of each truss is 1 inch 1 2 3 4 5 6 7 8 9 10 11 12 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20
  20. 20. <ul><li>(From ABAQUS documentation) </li></ul><ul><li>I’ll pick T3D2 2-node linear displacement </li></ul>Pick your elements
  21. 21. Modal Section <ul><li>*HEADING </li></ul><ul><li>CANTILEVER BEAM </li></ul><ul><li>** </li></ul><ul><li>** This is in inches </li></ul><ul><li>** </li></ul><ul><li>*NODE </li></ul><ul><li>1, 0., 0. </li></ul><ul><li>6, 100., 0. </li></ul><ul><li>7, 0., 20. </li></ul><ul><li>12, 100., 20. </li></ul><ul><li>*NSET, NSET=FIXED </li></ul><ul><li>1, 7 </li></ul><ul><li>*NGEN, NSET=allnodes </li></ul><ul><li>1, 6 </li></ul><ul><li>7, 12 </li></ul><ul><li>*ELEMENT, TYPE=T3D2, ELSET=BEAM </li></ul><ul><li>1, 1, 2 </li></ul><ul><li>2, 2, 3 </li></ul><ul><li>3, 3, 4 </li></ul><ul><li>4, 4, 5 </li></ul><ul><li>5, 5, 6 </li></ul><ul><li>6, 7, 8 </li></ul><ul><li>7, 8, 9 </li></ul>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. 22. History Section <ul><li>*STEP, PERTURBATION </li></ul><ul><li>*STATIC </li></ul><ul><li>** </li></ul><ul><li>** The load is in pounds </li></ul><ul><li>** </li></ul><ul><li>*CLOAD </li></ul><ul><li>6, 1, 200. </li></ul><ul><li>12, 2, -100, </li></ul><ul><li>*EL PRINT, POSITION=AVERAGED AT NODES, SUMMARY=YES </li></ul><ul><li>S, E </li></ul><ul><li>*NODE FILE, NSET=allnodes </li></ul><ul><li>U, CF, RF </li></ul><ul><li>*OUTPUT, FIELD, VARIABLE=PRESELECT </li></ul><ul><li>*ELEMENT OUTPUT </li></ul><ul><li>S, E </li></ul><ul><li>*OUTPUT, HISTORY </li></ul><ul><li>*NODE OUTPUT, NSET=allnodes </li></ul><ul><li>U, CF, RF </li></ul><ul><li>*END STEP </li></ul>
  23. 23. Looking at the results files <ul><li>Starting with the .log file you should review the results files. </li></ul>
  24. 24. Models with continuum elements <ul><li>To model most 3D structures that are bending Continuum or brick elements are the best. </li></ul><ul><li>Each element requires any nodes. </li></ul><ul><li>Models can be made by hand rather than CAE but can take much longer. </li></ul>
  25. 25. Continuum Elements
  26. 26. 3D Cantilever Beam Model data <ul><li>*HEADING </li></ul><ul><li>cantilever beam </li></ul><ul><li>** </li></ul><ul><li>** Coordinates are in inches </li></ul><ul><li>** </li></ul><ul><li>*NODE </li></ul><ul><li>1, 0.,0.,0. </li></ul><ul><li>193, 0.,0.,24. </li></ul><ul><li>1601, 2.,0.,0. </li></ul><ul><li>1793, 2.,0.,24. </li></ul><ul><li>8001, 0.,0.5,0. </li></ul><ul><li>8193, 0.,0.5,24. </li></ul><ul><li>9601, 2.,0.5,0. </li></ul><ul><li>9793, 2.,0.5,24. </li></ul><ul><li>** </li></ul>** 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. 27. Model section (cont.) <ul><li>** </li></ul><ul><li>** Make master elements for beam </li></ul><ul><li>** </li></ul><ul><li>*ELEMENT,TYPE=C3D20R </li></ul><ul><li>1, 1,401,4401,4001, 5,405,4405,4005, 201,2401,4201,2001, 205,2405,4205,2005, 3,403,4403,4003 </li></ul><ul><li>** </li></ul><ul><li>** Create elements for beam </li></ul><ul><li>** </li></ul><ul><li>*ELGEN,ELSET=CBEAM </li></ul><ul><li>1,4,400,1,48,4,10,2,4000,2000 </li></ul><ul><li>*ELSET, ELSET=LOCSTRESS </li></ul><ul><li>2,3,12,22,32,42,52,62,13,23,33,43,53,63,2002,2003 </li></ul><ul><li>2012,2022,2032,2042,2052,2062,2013,2023,2033,2043,2053,2063 </li></ul><ul><li>** </li></ul><ul><li>** Material properties for steel </li></ul><ul><li>** </li></ul><ul><li>*SOLID SECTION, MATERIAL=STEEL, ELSET=CBEAM </li></ul><ul><li>*MATERIAL, NAME=STEEL </li></ul><ul><li>** </li></ul><ul><li>** Youngs modulus is in lbf/in^2 </li></ul><ul><li>** </li></ul><ul><li>*ELASTIC </li></ul><ul><li>29.E6,0.3 </li></ul><ul><li>** </li></ul>
  28. 28. Student Accounts <ul><li>Now you are ready to work the projects. </li></ul><ul><li>You can use your AE student account in the AE Computer Lab (Knight 318) to run ABAQUS on these systems. </li></ul><ul><li>Or you can get an account on the ECS network (go to http://www.ecs.gatech.edu) </li></ul>

×