Post-processing

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

2. Finite element « outputs » • Essential variables: • Displacement u, temperature T find u such that: Ku = f • Natural variables : • Stress s, 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 • 2nd order tensors (s): 6 components if symm. + invariants (von Mises, max. principal, hydrostatic) • Localization: • Unique Nodal values • Element Nodal values • Gauss (integration) points values • Element centroid

4. 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

5. 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

6. 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

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)