Post processing
Download
1 / 23

Post- processing - PowerPoint PPT Presentation


  • 96 Views
  • 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

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

PowerPoint Slideshow about ' Post- processing' - brede


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

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)


ad