1. Post-processing J.Cugnoni, LMAF/EPFL, 2009

2. Finite element « outputs » Essential variables:  Displacement u, temperature T find u such that : K u = f Natural variables :  Stress , heat flux q  Directly related to (derivatives of) essential variables by the constitutive relationship in linear problems Derived variables :  Like strain =  u, strain energy density, enthalpy

3. FE results: type & localization Data types:  Scalars (T): 1 component  Vectors (u): 3 components + magnitude  2 nd order tensors (  ): 6 components if symm. + invariants (von Mises, max. principal, hydrostatic) Localization:  Unique Nodal values  Element Nodal values  Gauss (integration) points values  Element centroid

4. Displacement – Strain post processing Nodal displacement u (unique nodal val., essential var.) Shape functions & derivatives at integration pt of the element => B matrix Strain tensor at integration pt  = e B u Unique Nodal value Element Integration pt Shape functions and derivatives are only evaluated at integ. pts

5. Stress calculation at integration pts (linear elasticity) Constitutive relationship of element e => e C matrix Stress tensor at integration pt i of element e: e  i = e C e  i Element Integration pt Element-wise constitutive relation Strain tensor at integration pt i of element e: e  i = e B e u Element Integration pt

6. From integration pts to unique nodal values Stress tensor at nodal pt k of the global mesh:  k Shape functions or other extrapolation functions Stress tensor at integration pt i of the element e: e  i Unique Nodal value Element Integration pt Stress tensor at nodal pt j of the element e: e  j Weighted (or conditionnal) averaging Element Nodal value

7. FE results in Abaqus Field output:  A snapshot of the values at all points in the model for a given time History output:  A « time curve » for a single variable at a given point over time In STEP module:  Specify which variables must be computed in field output & history outputs  Can specify a « frequency » to reduce the output size  For history output, you need to define a « set » to extract time evolution of given points / elements

8. 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

9. FE result visualization in Abaqus Field outputs:  Select in Results -> Field outputs  Select the desired output time (Step & Frame)  Contour plot: colormap + deformed shape  Symbol plot: to display vectors or principal tensor components  Other features: Cutting planes, display groups A lot of options to customize display

10. Result localization in Abaqus Abaqus Standard solver stores only necessary results in ODB files:  Essential variables : unique nodal values  Natural variables: only at integration points  Derived variables: localized where in makes sense Abaqus CAE / visualization module can « extrapolate » some results at other locations  Example: evaluate unique nodal stresses from integration points  You can control the extrapolation in Results -> Option..  View « discontinuities » to identify « strong gradient » (=low accuracy) regions of your mesh

11. 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

12. Extracting values at node / 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

13. Example:  Extract different stress values (int. pt, elem. nodal, averaged nodal) at a given point Video: PostProDemo3.swf

14. 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

15. 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

16. 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

17. 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

18. 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?

19. 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?

20. 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

21. 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

22. 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

23. Advanced post-processing Calculate new fields:  If necessary, create a new coordinate system: Tools -> Coord. System -> Create  Run Tools -> Create Field outputs -> From fields Pick a time: Step & Increment Enter an expression in the « calculator »:  Pick operators & operands (fields) in the list  The new result will be « save » in memory only in a temporary Step called « Session Step »  You can use this tool to evaluate quantities in different coordinate systems (for example stress in cylindrical coordinates)