Meshing/Model Creation
Process of creating discretized model of solid composed of
finite elements.
Suppression of minor complex feature, geometric simplification for affordable
analysis
It is often necessary to remove minor complexities from the CAD geometry
before conducting analysis e.g. threads need to be suppressed, small protrusions
that are not
carrying load need to be removed. Another major simplification that
needs to be recognized and used is presence of any symmetry. If the geometry
is symmetric about any plane
and the loading is either symmetric or anti-symmetric (see discussion
under Boundary Condition), then only half the body needs to be modelled
with appropriate boundary
condition.
Major simplification
The 3D solid is reduced to an assemblage of rods, beams, shells(2D)
features using the criteria defined in the previous lectures.
Meshing
Manual Meshing
In this technique the analyst manually definess nodes and elements.
Rarely done now except for the most complex cases where automatic meshing
software fails or the analyst wants better quality of mesh.
Automatic Meshing
Two general techniques -- mapped meshes and free meshes.
Mapped Meshing
This is achieved by splitting oppposite boundary edges(2D)/faces(3D)
into a set number of segments and connecting them with lines -- with the
intersections defining interior nodes. Thus this requires the body to have
a regular number (3 or 4) "edges" and equal number of nodes on opposite
edges. This may be too restrictive for complex geometry or the presence
of holes but usually produces good mesh quality (well shaped elements)
when they work.
Free Meshing (method implemented in Pro/E mesh module)
In this method the surface is covered with elements of defined shape (triangles/quads, tetrahedra/hexahedra) using complex geometric algorithms. These algorithms attempt to cover the entire area/volume with well shaped elements. Such algoriithms usually work with triangles for 2D or tetrahedra for 3D. Free meshing will allow local control of element sizes.
Two popular algorithms for free meshing:
1.maximum area plane method: Suitable for complex slanted surfaces. A projection(shadow) of the surface onto a flat plane is meshed.
2.parametric space method: Every surface in
Pro/E(CAD) is represented parametrically as F(s,t) with s, t ranging from
0 to 1. In this meshing
technique nodes are generated by splitting
each parameter into intervals e.g. s=[0,0.1,0.2, ...,1.0] t=[0,0.1,0.2,...,1.0]
and taking all combination to
produce node coordinates i.e. 100 node
coordinates will be at {(0,0), (0,0.1),(0,0.2)....,(1.0,1.0)}.
These are then mapped to the physical coordinates
and connected to get a mesh.
Types of boundary conditionsBoundary Conditions
1.Displacement: constraints usually are meshed
as zero displacement/immovable.
2.Pressure: distributed loads
3.Force
4.Symmetry and Antisymmetry
If geometry is symmetric and loading is symmetric we can model only
half the body and impose symmetry BC on the displacement as below:
Symmetry BC
| Plane of symm. | X | Y | Z | RX | RY | RZ |
| X=0 | 0 | F | F | F | 0 | 0 |
| Y=0 | F | 0 | F | 0 | F | 0 |
| Z=0 | F | F | 0 | 0 | F | 0 |
If geometry is symmetric and loading is antisymmetric we
can model only half the body and impose antisymmetry BC on the displacement
as below:
Antisymmetry BC
| Pllane of
Symm |
X | Y | Z | RX | RY | RZ |
| X=0 | F | 0 | 0 | 0 | F | F |
| Y=0 | 0 | F | 0 | F | 0 | F |
| Z=0 | 0 | 0 | F | F | 0 | F |
F=> Free, RX,RY,RZ => rotations Notice ONLY out of plane motion allowed for any point on plane of symmetry.
St Venants Principle
The difference in stresses produced by two sets of statically equivalent
forces acting on a surface of area A diminishes with distance from A and
becomes
negligible at distances large compared to linear dimensions of A. Thus
for the purposes of analysis it is often acceptable to replace complex
boundary
condition with statically equivalent loads.