Top profile Call Girls In dewas [ 7014168258 ] Call Me For Genuine Models We ...
Fem ppt swapnil
1. 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
2. ABAQUS : General
ABAQUS is a highly sophisticated, general purpose finite element program,
designed primarily to model the behavior of solids and structures under
externally applied loading.
Salient features of ABAQUS
Capabilities for both static and dynamic problems
The ability to account all types of nonlinearities viz. material non-linearity
and 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, including
vibrations, 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)
3. ABAQUS : General
The 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 material
options
• ABAQUS/Explicit
For transient dynamics and quasi-static analyses using an explicit approach
static
appropriate in many applications such as drop test, crushing and many
manufacturing processes.
and
• ABAQUS/CAE (Complete Abaqus Environment)
nvironment)
It provides a complete modelling and visualization environment for ABAQUS
analysis products. It has direct access to CAD models, advanced meshing
and visualization
4. ABAQUS : General
Here we focus on ABAQUS/Standard
Solver Structure
Command Line ABAQUS CAE
ABAQUS STANDARD
Now we will model and analysis a single story Steel Plate Shear Wall (SPSW1) through
ABAQUS/CAE
(Note that it could be possible to create the model through command line which will be
discussed later)
5. ABAQUS/CAE Layout
You can start ABAQUS CAE from the START menu or with a command line by typing
abaqus 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
6. ABAQUS CAE modules
I)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 elements
II)ANALYSIS
• Job – Submit your job for analysis
III)POSTPROCESSING
• Visualization- View your results
7. 3-Dimensional FEM Problem
Dimensional
(Pushover Analysis of SPSW)
To start learning ABAQUS CAE we will work through modelling a
single story Steel Plate Shear Wall (SPSW1) specimen which
includes geometric nonlinearity (initial out-of-plane deformations
during fabrication). The specimen is subjected to monotonic lateral
load (Non-linear static pushover analysis)
Problem Statement
To find the ultimate load carrying capacity (Lateral load) of single
story steel plate shear wall (SPSW by non-linear static push over
(SPSW1)
analysis.
10. Selection of Element for Modelling SPSW
SPSW1
Infill Panel By using 3-Dimensional Shell
Element
Boundary Element By using 3-Dimensional Beam Element
11. 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)
13. − Create another new part as Boundary_Element
3-D planar
Type : Deformable Part:Boundary_Element
Boundary_Element
Basic feature: wire
Approximate size: 6 x6
15. Property Module
We will add the material Steel and give it values E= 2.0E+11N/m2 Poisson's ratio ν= 0.3, Yield
Stress = 2.0E+08N/m2,Plastic strain=0 (Note that elastically-perfectly plastic relationship is used for
steel)
We will create section called Shellsection and give it category of Shell ,Continuous
Shell/Homogenous and assign a thickness of 0.0025 with thickness integration point 5
0025m
Assign material to this section
16. 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_col
I-Section profile for Columns I-Section profile for Beams
Section
17. 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 using
parts Infill_Panel and Boundary_Element
Its easy to mesh the assembly as a whole using
independent instances
18. Step Module
By default there is a Initial Step in Abaqus (i.e. System made step) which is used to define the
.
Boundary Conditions
We will add a step after system made initial step called Transverse load
The procedure type is General and type is Static. The nlgeom=Yes means geometric
nonlinearity is on to account for large deformations
Keep the Output Request as preselected (By Default)
19. Step Module (Continued)
After step called Transverse Load create a next analysis step Lateral Load
The procedure type is General and type is Static Riks . Again nlgeom=Yes means
geometric nonlineaarity is on to account for large deformations
20. Interaction Module
In this module we will define the contact between two independent part namely Infill_Panel
and Boundary_Element
Create surface Infill_Panel_Master in part Infill_Panel
21. Similarly create surface Boundary_Element_Slave in part Boundary_Element
Once these surfaces are created we can provide contact between them through
Interaction module
Selection of Master surface
24. Creating Boundary Conditions in Initial Step
Create boundary conditions in Initial step (System made step)
There are two type of Boundary conditions for this problem namely
Bottom extreme nodes are fixed (U1=U2=U3
3=UR1=UR2=UR3=0)
Edges are restrained in z-direction (U3=0)
27. Mesh Module
Now we will mesh the assembly
Before that we will assign the shell element to Infill_Panel part. The shell element is S4R
Also assign the beam element to Boundary_Element part. The beam element is B31
30. 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 boundary
element into 20 parts. So for whole assembly mesh density will be 20x20.
32. Load Module
STEP:- Transverse Load :- Apply a concentrated load (named as CFORCE-1)of 2N at middle
node in negative z-direction (i.e. Along 3-axis)
33. Load Module (Continue)
STEP:- Lateral Load :- Apply a concentrated load (named as CFORCE-2)of 1000N at the
TOPNODES in positive x-direction (i.e. Along 1-axis).
axis).
Remember here we kept the displacement contro thus load magnitude mentioned above is used
trol
as load control during initial part of analysis
34. Job Module
We will create a job called SPSW1
Once this has been created just submit the job.
The analysis should only take a couple of minutes.
35. Here you have an option to
select analysis viz Full
analysis or Explicit analysis
or Restart
Submitting job after elapsed
time
36. 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 )
37. 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)
39. Visualization Module (Continued)
Here we will create X-Y plot
First plot is of Horizontal component of Total Force developed at bottom extreme node vs
increment
Creating X data
X-Y
43. 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
44. 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 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.
Now we will discuss how to create the model SPSW1 through an input
file and then we will run it through windows command prompt or
through ABAQUS CAE
45. 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.
******************************************************************************
*Heading
SPSW1
*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)
******************************************************************************
*NODE
1, 0., 0., 0.
21, 3, 0. 0.
*NGEN, nset=bottom
1, 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=top
0, 3, 0
46. *NFILL
bottom, 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=bottom
1, 20, 1, 1
*ELGEN
21, 20, 1, 1, 19, 21, 20
******************************************************************************
** (Creating master elements by using *Element command.)
******************************************************************************
*Element, type=B31
500, 1, 2
1000, 421, 422
1500, 1, 22
2000, 21, 42
*ELGEN, elset=beam
500, 20, 1
1000, 20, 1
1500, 20, 21
2000, 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.)
******************************************************************************
50. *Nset, nset=_PickedSet10, internal, instance=PART
instance=PART-1-1
2, 3, 4, 5, 6, 7, 8, 9, 10
10, 11, 12, 13, 14, 15, 16, 17
18, 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
*Plastic
2.50+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
51. 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 **step
one can define corresponding loading on model)
******************************************************************************
*Step, name="Transverse load ", nlgeom=YES
******************************************************************************
**(nlgeom=YES means geometric nonlinearity is on to account for large
**deformations)
******************************************************************************
*Static
1., 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 middle
node i.e._PICKEDSET13 in negative z-direction to initiate initial imperfection in
direction
plate )
******************************************************************************
*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)
******************************************************************************
52. ** FIELD OUTPUT: F-Output-1
*Output, field
*Node Output
CF, RF, TF, U
** FIELD OUTPUT: F-Output-2
*Element Output, directions=YES
E, 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, riks
0.1, 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.
53. ** 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 Step
To run ABAQUS Input File on Command Prompt
• At the command line
abaqus job=filename int (say SPSW)
54. Output Files created during running an Analysis
Following files were created during running an analysis in a directory of job file (say
C:TempTutorialSPSW1)
SPSW1.odb:-Out put database file which contains all requested field output and history output database
for 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 messages
will be written to this file.
SPSW1.log:- You will see some information about the time it took to for ABAQUS to complete
execution. 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). This
file contains full information about the analysis. The restart file is most useful if you want to plot the finite
element 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 the
computation has been completed.
SPSW1.msg:-The file named SPSW1.msg contains much more information concerning the increments
used, the iterative process, and the tolerances that ABAQUS has applied to determine whether a
solution has converged.
SPSW1.fil:-The file named SPSW4.fil is called a `results file’ (the file always has a .fil extension). This
file contains data that were specifically requested in the ABAQUS input file.
