Transcript Post-processing

J.Cugnoni, LMAF/EPFL, 2012

Essential variables:
◦ Displacement u, temperature T
find u such that : K u = 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

Data types:

Localization:
◦ Scalars (T): 1 component
◦ Vectors (u): 3 components + magnitude
◦ 2nd order tensors (s): 6 components if symm. +
invariants (von Mises, max. principal, hydrostatic)
◦
◦
◦
◦
Unique Nodal values
Element Nodal values
Gauss (integration) points values
Element centroid
Displacement – Strain post processing
Unique Nodal value
Shape functions and
derivatives are only
evaluated at integ. pts
Element Integration pt
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 = eB u
Stress calculation at integration pts (linear elasticity)
Element Integration pt
Element-wise
constitutive relation
Element Integration pt
Strain tensor at integration pt i
of element e: eei = eB eu
Constitutive relationship
of element e
=> eC matrix
Stress tensor at integration pt i
of element e: esi = eC eei
From integration pts to unique nodal values
Element Integration pt
Stress tensor at integration pt i
of the element e: esi
Shape functions or
other extrapolation functions
Element Nodal value
Stress tensor at nodal pt j
of the element e: esj
Weighted (or conditionnal)
averaging
Unique Nodal value
Stress tensor at nodal pt k
of the global mesh: sk

Field output:

History output:

In STEP module:
◦ A snapshot of the values at all points in the
model for a given time
◦ A « time curve » for a single variable at a given
point over time
◦ 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

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

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

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.
◦ Use view « discontinuities » to identify « strong gradient »
(=low accuracy) regions of your mesh

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

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

Example:
◦ Extract different stress values (int. pt, elem.
nodal, averaged nodal) at a given point
Video: PostProDemo3.swf

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

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

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

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 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 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?

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

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

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

Changing coordinate system:
◦ Create a coordinate system (for example cylindrical)
◦ In Result -> Options:
 choose Transformation, User defined
 Pick the coordinate system to use for 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)