Browsers provide a structured view of model data, which you can use to review, modify, create, and manage
the contents of a model. In addition to visualization, browsers offer features like search, filtering, and sorting,
which enhance your ability to navigate and interact with the model data.
FE geometry is topology on top of mesh, meaning CAD and mesh exist as a single entity. The purpose of FE geometry
is to add vertices, edges, surfaces, and solids on FE models which have no CAD geometry.
Tools and workflows that are dedicated to rapidly creating new parts for specific use cases, or amending existing
parts. The current capabilities are focused on stiffening parts.
Use PhysicsAI to build fast predictive models from CAE data. PhysicsAI can be trained on data with any physics or
remeshing and without design variables.
Use the Contour tool to visualize result data by coloring entities by value, allowing for easy identification of maximums
and minimums throughout the model. Contour plots can be created using any scalar data, including components or invariants
of vector or tensor results (for example: vonMises stress, displacement magnitude).
Use the Vector tool to draw arrows such that the direction in which the arrow points is the direction of the vector
and the length of the arrow is its magnitude. Individual vector components, shear, and complete resultants can be
plotted for vector-based results (for example: X, Y, Z, Resultant).
Use the Deformed tool to specify parameters for deformation display. This displays the original structure and the
deformed shape to see the total amount of movement, or view the deformed shape by itself.
Use the Marker tool to visualize result data by adding text on entities by ID and value, allowing for easy reference
of result values on selected entities. Marker plots can be created using any scalar data, including components or
invariants of vector or tensor results (for example: vonMises stress, displacement magnitude).
Use the Legend entity to create, edit and assign custom legends to any contour, vector and tensor or marker plot.
Legends can be numeric, or category based. It can be copied or saved to an external file and imported for re-use.
Explore, organize and manage your personal data, collaborate in teams, and connect to other data sources, such as
corporate PLM systems to access CAD data or publish simulation data.
Use the Beam Stress tool to display a contour of stress distribution on a
tessellation of a beam cross section.
Stress distribution is recalculated from vectors “1D Forces” and “1D Moments”
datatypes at first section (node 1) of a beam. It does not use any stress recovery
points from solver output.
You can control which of the force’s contributions to consider during the stress
calculation.
Stress is calculated using Elasticity theory (reference: Analysis and Design of
Elastic Beams: Computational Methods, Walter D. Pilkey).
Restriction:
Property must refer to either a Standard or Solid beam section.
A tessellation of the section is generated on-demand to display
the stress contour.
The result file needs to include vector datatypes “1D Forces” and “1D
Moments”.
OptiStruct native
*.h3d lacks such vectors and won’t
work.
*.op2, *.xdb file, or
any translation in *.h3d file will
work.
Currently, only the resultant force/moment at the first node of a beam
is considered during the stress calculation.
From the Post ribbon, click the Beam Stress tool.
Select 1D elements on which to calculate stress.
Use the drop-down on the guide bar to select the stress
quantity to evaluate.
Shear Y and Z are with respect to the elemental system.
Select force and moment in the microdialog.
The selected stress quantity is calculated from the forces and moments
contributions acting on first node of the beam element.
Select a loadcase for which stress is to be evaluated.
By default, the stress datatype is evaluated from the full acting load:
(Fx,Fy,Fz) & (Mx,My,Mz). You can disable any of these components to
evaluate the resultant stress without such contributions.
Selected beams can be contoured all at once by clicking on
the guide bar. Otherwise, clicking
Find enters a model tour with prev/ next options to
navigate across the selection.
During the model tour, the option Normal view
automatically sets the view normal to the section and fits the view on the
element.
Set display options by clicking
on the guide bar.
Mesh mode
The default stress calculation is performed using a meshed
section.
Coarse (default)
Faster for large selections and accurate enough in most
cases.
Around 4 elements in thickness for thin wall.
Fine
Creates a larger number of elements on thickness.
Capture higher stress
Can lead to artificial hotspots on sharp
corners
Scale Factor
If beam sections are small compared to the model size, it is
possible to scale them.
Contour Type
Display contour on Element (default) or on Node (see Figure 8).
Changing any of these options or force contributions/subcases will
auto-update the active contour.