post processing n.
Skip this Video
Download Presentation
Post- processing

Loading in 2 Seconds...

play fullscreen
1 / 23

Post- processing - PowerPoint PPT Presentation

  • Uploaded on

Post- processing. J.Cugnoni , LMAF/EPFL, 2012. Finite element « outputs ». Essential variables: Displacement u , temperature T find u such that : K u = f Natural variables : Stress s , heat flux q

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

PowerPoint Slideshow about 'Post- processing' - brede

Download Now 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
post processing


J.Cugnoni, LMAF/EPFL, 2012

finite element outputs
Finiteelement « outputs »
  • Essential variables:
    • Displacementu, temperature T

findu suchthat: Ku = f

  • Natural variables :
    • Stress s, heat flux q
    • Directlyrelated to (derivatives of) essential variables by the constitutive relationship in linearproblems
  • Derived variables :
    • Likestrain = u, strainenergydensity, enthalpy
fe results type localization
FE results: type & localization
  • Data types:
    • Scalars (T): 1 component
    • Vectors (u): 3 components + magnitude
    • 2ndordertensors (s): 6 components if symm. + invariants (von Mises, max. principal, hydrostatic)
  • Localization:
    • Unique Nodal values
    • Element Nodal values
    • Gauss (integration) points values
    • Elementcentroid

Nodal displacement u

(unique nodal val., essential var.)

Unique Nodal value

Shape functions and derivatives are only evaluated at integ. pts

Shape functions & derivatives at integration pt of the element

=> B matrix

Strain tensor at integration pt

e = eBu

Element Integration pt

Displacement – Strain post processing


Stress calculation at integration pts (linear elasticity)

Strain tensor at integration pt i of element e: eei = eBeu

Element Integration pt

Constitutive relationship of element e

=> eC matrix

Element-wise constitutive relation

Stress tensor at integration pt i of element e: esi = eCeei

Element Integration pt


From integration pts to unique nodal values

Stress tensor at integration pt i

of the element e: esi

Element Integration pt

Shape functions or

other extrapolation functions

Stress tensor at nodal pt j

of the element e: esj

Element Nodal value

Weighted (or conditionnal)averaging

Stress tensor at nodal pt kof the global mesh: sk

Unique Nodal value

fe results in abaqus
FE results in Abaqus
  • Field output:
    • A snapshot of the values at all points in the model for a giventime
  • History output:
    • A « time curve » for a single variable at a given point over time
  • In STEP module:
    • Specifywhich variables must becomputed in field output & history outputs
    • Can specify a « frequency » to reduce the output size
    • For history output, youneed to define a « set » to extract time evolution of given points / elements
how to specify non default field history outputs
How to: specify non-default field / history outputs
  • Example:
    • open thermoMecaExo1Correct.cae
    • Select to Model-1-Transient
    • In Step module:
      • Edit existing Field output:
        • Add all Energy outputs, add Forces-> NFORC
        • Add Thermal outputs NFLUX & HFLA (heat flux * area)
      • History outputs:
        • Tool -> Set -> Create : create a set of points for history output
        • Create a new history output
        • Domain=Set, Output: Thermal->NT (nodal temperature)
    • Run the Job « thermoMecaTransient »

Video: PostProDemo1.swf

fe result visualization in abaqus
FE result visualization in Abaqus
  • Field outputs:
    • Select in Results -> Field outputs
    • Select the desired output time (Step & Frame)
    • Contour plot:
      • colormap + deformedshape
    • Symbol plot:
      • to display vectors or principal tensor components
    • Otherfeatures:
      • Cutting planes, display groups
      • A lot of options to customize display
result localization in abaqus
Result localization in Abaqus
  • Abaqus Standard solver stores onlynecessaryresults in ODB files:
    • Essential variables : unique nodal values
    • Natural variables: onlyatintegration points
    • Derived variables: localizedwhere in makessense
  • Abaqus CAE / visualization module can « extrapolate » someresultsatother locations
    • Example: evaluate unique nodal stresses fromintegration points
    • You can control the extrapolation in Results -> Option.
    • Use view« discontinuities » to identify « strong gradient » (=lowaccuracy) regions of yourmesh
how to visualize 3d fields
How to: visualize 3D fields
  • Example (open thermoMecaTransient.odb):
    • Contour plots of stress field, select time = 2000 s:
      • Select Mises, S33, Max. Principal components
      • Change Visualization options (deformation scale factor, colormap range, edges)
      • Cutting plane
    • Results Options (select Mises stress):
      • Disable averaging, look at element nodal values, notice the discontinuities.
      • Enable averaging, change the averaging threshold (0% -> 100%)
      • Display discontinuities, notice regions of large discontinuities: sharp corners = stress singularities !!
    • Symbol plot:
      • Use display group to isolate a region
      • View principal stress tensor and displacements

Video PostProDemo2.swf

extracting values at node element
Extracting values atnode / element
  • Select Field output, activate Contour plot
  • Use Tools->Query->Probe Value
    • Select Probe = Element or Probe = Node
    • Select result localization (for elements only)
      • Integration pts, Centroid, Element nodal
    • Activate the desired results in the table
    • Pick a node / element to add it to the list
    • Can write the table values to a text file: write
how to extract values at selected points
How to: extract values atselected points
  • Example:
    • Extract different stress values (int. pt, elem. nodal, averaged nodal) at a given point

Video: PostProDemo3.swf

extracting curves in abaqus
Extracting curves in Abaqus
  • Path = spatial curve to « cut the model »:
    • Use Tools -> Path -> Create to generate
    • Generation method:
      • Node list: pick nodes to define a polyline
      • Point list: enter coordinates of polyline vertices
      • Edge list: select element edges = efficient !!
      • Circular: select points to generate a circle
  • To plot / save the curve:
    • Use Tools -> XY data -> Create
      • Select source = Path
      • Choose the path
      • choose configuration = « undeformed »
      • activate include intersection
      • Generate the curve & save it for later use
how to extract a 2d curve along a path
How to: extract a 2D curvealong a path
  • Example:
    • Define a linear path based on 2 nodes
    • Define a path along edges with « feature edge » or « shortest distance » option
    • Define a circular path by 3 points
    • Extract curves of Mises Stress distribution along each path, save XY data
    • Plot all XY curves

Video: PostProDemo4.swf

extracting curves in abaqus1
Extracting curves in Abaqus
  • Time evolution curves :
    • From Field outputs:
      • Use Tools -> XY data -> Create
      • Choose source = Field Output
      • Select result localization (integ pt, nodal, …)
      • Select result to extract
      • Pick elements or nodes from 3D view
      • Plot and save if necessary
    • From History outputs:
      • Use Tools -> XY data -> Create
      • Choose source = History output
      • Select the desired history output, plot and save
how to extract a time evolution curve
How to: extract a time-evolutioncurve
  • Example:
    • Extract time evolution curves of the temperature at some nodes
    • Extract time evolution curves of the Mises stress at for different type of result localization
    • Plot all XY curves

Video: PostProDemo5.swf

exporting data from abaqus
Exporting data from Abaqus
  • Exporting field outputs
    • If needed, isolate a region of interest with Display Group
    • Use Report -> Field Output
    • Select the localization & type of the result
    • Select output file & check append / overwrite
    • Select Data: all data, column totals, statistics?
exporting data from abaqus1
Exporting data from Abaqus
  • Exporting XY curves
    • Create XY data and save it
    • Use Report -> XY
    • Select the XY curves
    • Select output file & check append / overwrite
    • Select Data: all data, column totals, statistics?
how to export data to text files
How to: export data to text files
  • Example:
    • Use Report-> Field Output to extract the min, max and average nodal temperature in a Text file
    • Create a XY curve of the time evolution of the temperature at one point and export it to another text file

Video: PostProDemo6.swf

extracting images movies
Extracting images & movies
  • Image capture / printing:
    • File -> Print
      • Choose Destination = Printer or File
      • If File, choose format (PNG for example) and file name
  • Movies:
    • Enter an animation mode:
      • Animate -> Time History / Scale Factor / Harmonic
    • Use Animate -> Save As to generate movie
      • Select destination file and format
      • Set Options to choose the level of compression
      • Choose display option (background ?)
      • Set frame rate to ~5 image/s
how to capture images and animations
How to: capture images and animations
  • Example:
    • Extract an image of Mises stress field at t=2000s showing the min & max values
    • Extract a movie of the time evolution of the temperature in the model

Video: PostProDemo7.swf

advanced post processing
Advanced post-processing
  • Changingcoordinate system:
    • Create a coordinate system (for examplecylindrical)
    • In Result -> Options:
      • choose Transformation, User defined
      • Pick the coordinate system to use for post processing
  • Calculatenew fields:
    • If necessary, create a new coordinate system: Tools -> Coord. System -> Create
    • Run Tools -> Create Field outputs -> Fromfields
      • Pick a time: Step & Increment
      • Enter an expression in the « calculator »:
        • Pickoperators & operands (fields) in the list
    • The new resultwillbe « save » in memoryonly in a temporaryStepcalled « Session Step »
    • You can use thistool to evaluatequantities in differentcoordinatesystems (for example stress in cylindricalcoordinates)