Post- processing

1 / 23

# Post- processing - PowerPoint PPT Presentation

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.

## PowerPoint Slideshow about ' Post- processing' - brede

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

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
• 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
• 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
• Example:
• open thermoMecaExo1Correct.cae
• Select to Model-1-Transient
• In Step module:
• Edit existing Field output:
• 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
• 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
• 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
• 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 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 atselected points
• Example:
• Extract different stress values (int. pt, elem. nodal, averaged nodal) at a given point

Video: PostProDemo3.swf

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 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 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-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 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 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
• 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
• 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
• 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