Fem ppt swapnil
Upcoming SlideShare
Loading in...5
×
 

Fem ppt swapnil

on

  • 2,367 views

 

Statistics

Views

Total Views
2,367
Views on SlideShare
2,367
Embed Views
0

Actions

Likes
2
Downloads
252
Comments
1

0 Embeds 0

No embeds

Accessibility

Upload Details

Uploaded via as Adobe PDF

Usage Rights

© All Rights Reserved

Report content

Flagged as inappropriate Flag as inappropriate
Flag as inappropriate

Select your reason for flagging this presentation as inappropriate.

Cancel
  • Full Name Full Name Comment goes here.
    Are you sure you want to
    Your message goes here
    Processing…
Post Comment
Edit your comment

Fem ppt swapnil Fem ppt swapnil Presentation Transcript

  • FINITE ELEMENT ANALYSIS IN ABAQUS Siddhartha Ghosh* and Swapnil B. Kharmale** * Assistant Professor, ** Research Scholar (PhD Student ) Department of Civil Engineering Indian Institute of Technology, Bombay
  • ABAQUS : GeneralABAQUS is a highly sophisticated, general purpose finite element program,designed primarily to model the behavior of solids and structures underexternally applied loading. Salient features of ABAQUS Capabilities for both static and dynamic problems The ability to account all types of nonlinearities viz. material non-linearityand geometric non-linearity A very extensive element library, including a full set of continuum elements,beam elements, shell and plate elements A sophisticated capability to model contact between solids Capabilities to model a number of phenomena of interest, includingvibrations, coupled fluid/structure interactions, acoustics, buckling problems,and so on. (From:www.abaqus.comand and www.engin.brown.edu/courses/en www.engin.brown.edu/courses/en175/abaqustut/abaqustut)
  • ABAQUS : GeneralThe ABAQUS suite consists of three core products:• ABAQUS/Standard,For traditional implicit finite element analyses such as static, dynamics,thermal, all powered with the widest range of contact and nonlinear materialoptions• ABAQUS/ExplicitFor transient dynamics and quasi-static analyses using an explicit approach staticappropriate in many applications such as drop test, crushing and manymanufacturing processes. and• ABAQUS/CAE (Complete Abaqus Environment) nvironment)It provides a complete modelling and visualization environment for ABAQUSanalysis products. It has direct access to CAD models, advanced meshingand visualization
  • ABAQUS : GeneralHere we focus on ABAQUS/Standard Solver Structure Command Line ABAQUS CAE ABAQUS STANDARDNow we will model and analysis a single story Steel Plate Shear Wall (SPSW1) throughABAQUS/CAE(Note that it could be possible to create the model through command line which will bediscussed later)
  • ABAQUS/CAE LayoutYou can start ABAQUS CAE from the START menu or with a command line by typingabaqus cae in a Command window. Following figure shows how an ABAQUS/CAE looks Title bar Menu bar Tool bar Context bar View port Canvas & Drawing Toolbox area Area Prompt area Message area
  • ABAQUS CAE modulesI)PREPROCESSING• Part – Create individual parts• Property – Create and assign material properties• Assembly – Create and place all parts instances• Step – Define all analysis steps and the results you want• Interaction – Define any contact information• Load- Define and place all loads and boundary conditions• Mesh – Define your nodes and elementsII)ANALYSIS• Job – Submit your job for analysisIII)POSTPROCESSING• Visualization- View your results
  • 3-Dimensional FEM Problem Dimensional (Pushover Analysis of SPSW) To start learning ABAQUS CAE we will work through modelling asingle story Steel Plate Shear Wall (SPSW1) specimen whichincludes geometric nonlinearity (initial out-of-plane deformationsduring fabrication). The specimen is subjected to monotonic lateralload (Non-linear static pushover analysis) Problem StatementTo find the ultimate load carrying capacity (Lateral load) of singlestory steel plate shear wall (SPSW by non-linear static push over (SPSW1)analysis.
  • Details of SPSW SPSW1
  • Lateral Force- Deformation Behavior of SPSW
  • Selection of Element for Modelling SPSW SPSW1Infill Panel By using 3-Dimensional ShellElementBoundary Element By using 3-Dimensional Beam Element
  • PART MODULE− Create a new part as Infill_Panel 3-D planar Type : Deformable Basic feature: shell Approximate size: 6x6 (Note :- ABAQUS follows consistent unit so be specific to keep same unit. Here we kept SI units i.e. m for length N for force etc)
  • Part:- Infill_PanelThe following picture shows how a Part Infill_Panel look
  • − Create another new part as Boundary_Element 3-D planar Type : Deformable Part:Boundary_Element Boundary_Element Basic feature: wire Approximate size: 6 x6
  • Infill_Panel and Boundary_Element Parts in ABAQUS/CAE
  • Property ModuleWe will add the material Steel and give it values E= 2.0E+11N/m2 Poissons ratio ν= 0.3, YieldStress = 2.0E+08N/m2,Plastic strain=0 (Note that elastically-perfectly plastic relationship is used forsteel)We will create section called Shellsection and give it category of Shell ,ContinuousShell/Homogenous and assign a thickness of 0.0025 with thickness integration point 5 0025mAssign material to this section
  • Property Module (Continued) Also create section called Boundarysection_col and Boundarysection_bea and give it category of Beam Create profile namely Columns and Beams using I- shaped cross section Assign same material to this section also Boundarysection_colI-Section profile for Columns I-Section profile for Beams Section
  • Property Module (Continued) Assign Shellsection to part named Infill_Panel Assign Boundarysection_col and Boundarysection_bea with Columns and Beams profile to part named Bounary_Element Assembly Module Now we will create two independent instances usingparts Infill_Panel and Boundary_Element Its easy to mesh the assembly as a whole usingindependent instances
  • Step ModuleBy default there is a Initial Step in Abaqus (i.e. System made step) which is used to define the .Boundary ConditionsWe will add a step after system made initial step called Transverse loadThe procedure type is General and type is Static. The nlgeom=Yes means geometricnonlinearity is on to account for large deformationsKeep the Output Request as preselected (By Default)
  • Step Module (Continued)After step called Transverse Load create a next analysis step Lateral LoadThe procedure type is General and type is Static Riks . Again nlgeom=Yes meansgeometric nonlineaarity is on to account for large deformations
  • Interaction Module In this module we will define the contact between two independent part namely Infill_Paneland Boundary_ElementCreate surface Infill_Panel_Master in part Infill_Panel
  • Similarly create surface Boundary_Element_Slave in part Boundary_Element Once these surfaces are created we can provide contact between them throughInteraction module Selection of Master surface
  • Selection of Slave surface
  • Interaction between two parts namely Infill_Panel and Boundary_Element
  • Creating Boundary Conditions in Initial StepCreate boundary conditions in Initial step (System made step)There are two type of Boundary conditions for this problem namelyBottom extreme nodes are fixed (U1=U2=U3 3=UR1=UR2=UR3=0)Edges are restrained in z-direction (U3=0)
  • Bottom extreme nodes are fixed (U1=U =U2=U3=UR1=UR2=UR3=0 i.e. Encastre)
  • Edges are restrained in z z-direction (U3=0)
  • Mesh ModuleNow we will mesh the assemblyBefore that we will assign the shell element to Infill_Panel part. The shell element is S4RAlso assign the beam element to Boundary_Element part. The beam element is B31
  • Assigning S4R Element to Infill_Panel part R
  • Assigning B31 Element to Boundary_Element part
  • Mesh Module (Continued) After assigning proper element to each of part next step is seeding. Here we are using mesh of 20x20 for Infill_Panel part and we will discritize each boundaryelement into 20 parts. So for whole assembly mesh density will be 20x20.
  • Meshing of whole Assembly of SPSW SPSW1
  • Load ModuleSTEP:- Transverse Load :- Apply a concentrated load (named as CFORCE-1)of 2N at middlenode in negative z-direction (i.e. Along 3-axis)
  • Load Module (Continue) STEP:- Lateral Load :- Apply a concentrated load (named as CFORCE-2)of 1000N at theTOPNODES in positive x-direction (i.e. Along 1-axis). axis). Remember here we kept the displacement contro thus load magnitude mentioned above is used trolas load control during initial part of analysis
  • Job ModuleWe will create a job called SPSW1Once this has been created just submit the job.The analysis should only take a couple of minutes.
  • Here you have an option toselect analysis viz Fullanalysis or Explicit analysisor RestartSubmitting job after elapsedtime
  • Visualization Module (Post processing)− Once your analysis is complete we want to see the results.− First we will see the deformed shape of SPSW1 in Step Transverse Load. (Remember this step is created to have initial out plane deformation (due to fabrications). So the out-of deformed shape is somewhat similar to buckling of plate )
  • Visualization Module (Continued)− Now we will see the deformed shape of SPSW1 in Step Lateral Load. (This step is static push over . Here out of plane deformations start increasing with increase in lateral load, and the buckling along the compression diagonal can be very clearly seen from the deformed shape of SPSW1 at the end of analysis)
  • Visualization Module (Continued)− If we look at Von Mises stress distribution we see
  • Visualization Module (Continued) Here we will create X-Y plot First plot is of Horizontal component of Total Force developed at bottom extreme node vsincrement Creating X data X-Y
  • Visualization Module (Continued)Selection of bottom extreme nodes to create X data X-Y
  • Visualization Module (Continued)
  • Visualization Module (Continued)Similarly create plot of Horizontal displacement (U1) of top node vs increment
  • Visualization Module (Continued)− Now we will create a plot of Base shear (which is sum of horizontal component of total force developed at extreme bottom nodes (which are fixed support)) and lateral displacement of Top node
  • About ABAQUS Command line use (Input file creation )Note:-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 beforethe 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.Now we will discuss how to create the model SPSW1 through an inputfile and then we will run it through windows command prompt orthrough ABAQUS CAE
  • Simple Input File (Model Section)**The lines starting with ** (2 asterisks) commented and are ignored ** by the**ABAQUS solver. Other lines beginning with a single * denotes an ABAQUS keyword.*******************************************************************************HeadingSPSW1*Preprint, echo=YES, model=YES, history=YES, contact=YES********************************************************************************The *PREPRINT key controls what information is printed to the file named**SPSWl.dat. Here, we have asked ABAQUS to print out absolutely everything. The**SPSWl.dat file is rather large as a consequence Once the input file is correct, consequence.**you can set all the options to NO to reduce the size of the file.)******************************************************************************** (Creating geometry of model)******************************************************************************** PARTS*Part, name=PART-1-1******************************************************************************** (Defining the control node coordinate)*******************************************************************************NODE1, 0., 0., 0.21, 3, 0. 0.*NGEN, nset=bottom1, 21, 1********************************************************************************(nset=bottom is a node set which contains node started from 1 to 21 with an**interval of 1)*******************************************************************************NCOPY, CHANGE NUMBER=420, OLD SET=bottom, SHIFT, new set=top0, 3, 0
  • *NFILLbottom, top, 20, 21*Element, type=S4R 1, 1, 2, 23, 22 21, 22, 23, 44, 43********************************************************************************(Generating the intermediate shell elements in increment through *ELGEN command)*******************************************************************************ELGEN, elset=bottom1, 20, 1, 1*ELGEN21, 20, 1, 1, 19, 21, 20******************************************************************************** (Creating master elements by using *Element command.)*******************************************************************************Element, type=B31500, 1, 21000, 421, 4221500, 1, 222000, 21, 42*ELGEN, elset=beam500, 20, 11000, 20, 11500, 20, 212000, 20, 21********************************************************************************(By using *Elset command one can made different set or group of element which**will be helpful while assigning material properties,boundary conditions,loading**etc.)******************************************************************************
  • *Elset, elset=BEAM500, 501, 502, 503, 504, 505, 506, , 507, 508, 509, 510, 511, 512,513, 514, 515516, 517, 518, 519, 1000, 1001, 1002 1002, 1003, 1004, 1005, 1006, 1007, 1008,1009, 1010, 10111012, 1013, 1014, 1015, 1016, 1017, 1018 1018, 1019, 1500, 1501, 1502, 1503, 1504,1505, 1506, 15071508, 1509, 1510, 1511, 1512, 1513, 1514 1514, 1515, 1516, 1517, 1518, 1519, 2000,2001, 2002, 20032004, 2005, 2006, 2007, 2008, 2009, 2010 2010, 2011, 2012, 2013, 2014, 2015, 2016,2017, 2018, 2019*Nset, nset=_PICKEDSET2, internal, generate 1, 441, 1*Elset, elset=_I1, internal, generate 1, 400, 1*Elset, elset=_I5, internal, generate 500, 519, 1*Elset, elset=_I2, internal, generate 1000, 1019, 1*Elset, elset=_I3, internal, generate 1500, 1519, 1*Elset, elset=_I4, internal, generate 2000, 2019, 1** Region: (Section-1-_I1:Picked)*Elset, elset=_I1, internal, generate 1, 400, 1** Section: Section-1-_I1*Shell Section, elset=_I1, material=Steel0.0025, 5********************************************************************************(*Shell section command will create shell section having thickness =0.0025m with 5no. of integration point)******************************************************************************
  • ** Region: (Section-2-_I5:Picked), (Beam Orientation:Picked)*Elset, elset=_I5, internal, generate 500, 519, 1** Section: Section-2-_I5 Profile: Profile Profile-1******************************************************************************** (*Beam section command will create beam of I-cross section)*******************************************************************************Beam Section, elset=_I5, material=Steel, temperature=GRADIENTS, section=I0.0381, 0.0762, 0.059182, 0.059182, 0.006604 0.006604, 0.004318 006604,0.,0.,1.** Region: (Section-3-_I2:Picked), (Beam Orientation:Picked)*Elset, elset=_I2, internal, generate 1000, 1019, 1** Section: Section-3-_I2 Profile: Profile Profile-2*Beam Section, elset=_I2, material=Steel, temperature=GRADIENTS, section=I0.0381, 0.0762, 0.059182, 0.059182, 0.006604 0.006604, 0.004318 006604,0.,0.,1.** Region: (Section-4-_I3:Picked), (Beam Orientation:Picked)*Elset, elset=_I3, internal, generate 1500, 1519, 1** Section: Section-4-_I3 Profile: Profile Profile-3*Beam Section, elset=_I3, material=Steel, temperature=GRADIENTS, section=I0.0381, 0.0762, 0.059182, 0.059182, 0.006604 0.006604, 0.004318 006604,0.,0.,-1.** Region: (Section-5-_I4:Picked), (Beam Orientation:Picked)*Elset, elset=_I4, internal, generate 2000, 2019, 1
  • ** Section: Section-5-_I4 Profile: Profile Profile-4*Beam Section, elset=_I4, material=Steel, temperature=GRADIENTS, section=I0.0381, 0.0762, 0.059182, 0.059182, 0.006604 0.006604, 0.004318 006604,0.,0.,-1.*End Part******************************************************************************** (Used to assemble the different individual parts here in current problem only onepart is used.)******************************************************************************** ASSEMBLY*Assembly, name=Assembly*Instance, name=PART-1-1, part=PART-1-1*End Instance***Nset, nset=topnode, instance=PART-1-1431*Nset, nset=_PICKEDSET11, internal, instance=PART instance=PART-1-1 421, 422, 423, 424, 425, 426, 427, 428 434, 435, 436, 437, 438, 439, 440, 428,441*Nset, nset=_PICKEDSET13, internal, instance=PART instance=PART-1-1 221,*Nset, nset=_PickedSet8, internal, instance=PART instance=PART-1-1 1, 21*Nset, nset=_PickedSet9, internal, instance=PART instance=PART-1-12, 3, 4, 5, 6, 7, 8, 9, 1010, 11, 12, 13, 14, 15, 16, 1718, 19, 20, 22, 42, 43, 63, 64, 84, 85, 105, 106, 126, 127, 147, 148168, 169, 189, 190, 210, 211, 231, 232, 252, 253, 273, 274, 294, 295, 315, 316336, 337, 357, 358, 378, 379, 399, 400, 420, 421, 422, 423, 424, 425, 426, 427428, 429, 430, 431, 432, 433, 434, 435, 436, 437, 438, 439, 440, 441
  • *Nset, nset=_PickedSet10, internal, instance=PART instance=PART-1-12, 3, 4, 5, 6, 7, 8, 9, 10 10, 11, 12, 13, 14, 15, 16, 1718, 19, 20, 421, 422, 423, 424, 425, 426 427, 428, 429, 430, 431, 432, 433 426,434, 435, 436, 437, 438, 439, 440, 441*End Assembly******************************************************************************** (With this Geometry of model ends)******************************************************************************** MATERIALS******************************************************************************** (*Material command is used to define material which has been used to**different component of model It include all engineering properties of**material)*******************************************************************************Material, name=Steel*Elastic 2.0e+11, 0.3*Plastic2.50+08, 0.******************************************************************************** BOUNDARY CONDITIONS******************************************************************************** (*Boundary command is used to create appropriate boundary **conditions)******************************************************************************** Name: Disp-BC-1 Type: Symmetry/Antisymmetry/Encastre Antisymmetry/Encastre*Boundary_PickedSet8, ENCASTRE** Name: Disp-BC-2 Type: Displacement/Rotation*Boundary_PickedSet9, 3, 3*Boundary_PickedSet10, 2, 2
  • Simple Input File (History Section)** STEP: Transverse load******************************************************************************** (*Step command is used to create different analysis step like Static**General, Static Riks, Dynamic, Dynamic Explicit etc. In each analysis **stepone can define corresponding loading on model)*******************************************************************************Step, name="Transverse load ", nlgeom=YES********************************************************************************(nlgeom=YES means geometric nonlinearity is on to account for large**deformations)*******************************************************************************Static1., 1., 1e-05, 1.** LOADS** Name: CFORCE-1 Type: Concentrated force********************************************************************************(*Cload command is used for concentrated load. A load of 2N is applied at middlenode i.e._PICKEDSET13 in negative z-direction to initiate initial imperfection in directionplate )*******************************************************************************Cload_PICKEDSET13, 3, -2.**** OUTPUT REQUESTS*Restart, write, frequency=0********************************************************************************(*Restart command in ABAQUS allows multi step analysis. Here one can use**frequency=n that means saving the output after n interval,frequency =overlay means**directly give output at end of step without saving intermediate increment result,**frequency=0 means to save output for each interval)******************************************************************************
  • ** FIELD OUTPUT: F-Output-1*Output, field*Node OutputCF, RF, TF, U** FIELD OUTPUT: F-Output-2*Element Output, directions=YESE, ESF1, MISESMAX, NFORC, PE, PEEQ, S, SE, SEE, SF** HISTORY OUTPUT: H-Output-1*Output, history, variable=PRESELECT*End Step******************************************************************************** STEP: Lateral load*Step, name="Lateral load", nlgeom=YES, inc=10000********************************************************************************(In “Static Riks” step 0.1 indicate initial time increment 100 indicate time**period of step 1e-10 indicate minimum time increment allowed 1 indicate**maximum time increment allowed 20 indicates load proportionality factor,**topnode, 1, 0.05 indicates the displacement control means stop analysis when**x- directional displacement reached up to 0.05m)*******************************************************************************Static, riks0.1, 100., 1e-10, 1., 20., topnode, 1, 0 0.05** LOADS** Name: CFORCE-2 Type: Concentrated force********************************************************************************(A load of 10000N is applied at top edge nodes i.e._PICKEDSET11 in**positive x-direction for static pushover analysis.)*******************************************************************************Cload_PICKEDSET11, 1, 10000.
  • ** OUTPUT REQUESTS *Restart, write, frequency=0 ** FIELD OUTPUT: F-Output-3 *Output, field *Node Output CF, RF, TF, U ** FIELD OUTPUT: F-Output-4 ************************************************************************** ** (Field output will give the selected output) ************************************************************************** *Element Output, directions=YES E, EE, ESF1, IE, MISESMAX, NFORC, PE, PEEQ, S, SF ** HISTORY OUTPUT: H-Output-2 *Output, history, variable=PRESELECT *End StepTo run ABAQUS Input File on Command Prompt • At the command line abaqus job=filename int (say SPSW)
  • Output Files created during running an AnalysisFollowing files were created during running an analysis in a directory of job file (sayC:TempTutorialSPSW1)SPSW1.odb:-Out put database file which contains all requested field output and history output databasefor given job. SPSW1.dat:-This file contains all kinds of information about the computations that ABAQUS has done.In particular, if ABAQUS encounters any problems during the computation, error and warning messageswill be written to this file. SPSW1.log:- You will see some information about the time it took to for ABAQUS to completeexecution. You should also see that the file ends with ABAQUS JOB SPSW1 COMPLETED SPSW1.res:-The file named SPSW1.res is called a `restart file’ (the file always has .res extension). Thisfile contains full information about the analysis. The restart file is most useful if you want to plot the finiteelement mesh, or contours of stress, displacement, etc SPSW1.sta:-This file is continuously updated by ABAQUS as it runs, and tells you how much of thecomputation has been completed. SPSW1.msg:-The file named SPSW1.msg contains much more information concerning the incrementsused, the iterative process, and the tolerances that ABAQUS has applied to determine whether asolution has converged. SPSW1.fil:-The file named SPSW4.fil is called a `results file’ (the file always has a .fil extension). Thisfile contains data that were specifically requested in the ABAQUS input file.
  • THANK YOU!