Transcript CAD Import, Partitionning &Meshing

CAD Import,
Partitioning &
Meshing
J.Cugnoni LMAF / EPFL 2009
CAD Model Structure

Vertices (0D):
 Coordinates

Edges (1D):
 several

& coordinate system
Vertices => line / curve
Surfaces (2D):
 closed
loop of edges (shared vertices), parametric 2D
space, normal = orientation

Volumes (3D):
a
closed set of surfaces (shared edges), unified
normal orientation
CAD Example
3D CAD volume:
all edges are shared between boundary faces =>
no « free » edges => surface is closed => it’s a volume!
CAD import in ABAQUS / CAE

Several formats are supported by Abaqus CAE:





STEP : universal file format, good for volumes & assemblies
IGES : universal file format, good for surfaces, ok for volumes
SAT : ACIS, native geometry format of CAE, good for nearly
everything
CATPart: CATIA v5 format, can be imported with a specific
module (1 licence)
Always check the geometry:





Free edges / invalid entities (tools => query => geom. diagnostic)
If free edges: stitch the surfaces (tools => geom. repair => part
=> stitch)
If meshing problems: convert to « precise » (tools => geom.
repair => part => convert to precise)
Check the dimensions / units !!
If you have problems with geometric operations (like partition),
try to Convert to Precise and Convert to Analytical
representation
Meshing: basic principle
Mesh generation in 3D is based on the same
hierarchy as the CAD model:
 1D:
meshing of the edges, starting from a user-
defined element size / distribution
 2D:
propagation of 1D mesh to 2D surface;
structured or free (advancing front or medial axis).
 3D:
propagation of 2D mesh to the 3D volume;
structured, semi-structured (sweep), free
Meshing: basic principle
1D Meshing algorithms

Method:
 Use
the curvilinear parameter to distribute
nodes along edges => create 1D elements

Definition:
 Constant
size: number of elements on edge
or element size
 Variable size: number of elements and bias
Bias = ratio of largest to smallest elem. size
 Pick the edge close to the end to be refined

1D Meshing algorithms
Biased
element size
distribution
Default
(global)
element size
Constant
element
size
Meshing algorithms 2D

Methods:
 Propagate 1D mesh on the surface
 Curved surface:
 Nearly planar: use projection on the best plane
 General: mesh in Parameter space
 Algorithms:
 Structured / mapped meshing
 Delaunay triangulation
 Advancing front meshing
 Medial axis

Definition:
 Just select the meshing algorithm
 Automatically inherits the mesh size
from the edges
Mapped meshing algorithms 2D
Mapped meshing (works for surfaces having 3 to 5 corners)
Free meshing algorithms 2D
Advancing front meshing
Medial axis meshing
Meshing algorithms 3D

Methods:
 Propagate 2D mesh in the volume
 Algorithms:
 Structured / mapped meshing :


Semi-structured:



« extrusion » / « sweep » of a free 2D mesh (tri or quad)
Generates either hexa or prisms (wedges)
Free meshing:


map volume to a simple case (hexa)
Delaunay or Advancing Front tetrahedralization
Definition:
 Just select the meshing algorithm
 Automatically inherits the mesh size
& edges
from the surfaces
Mapped meshing algorithms 3D
Mapped meshing for hexa:
any extrusion of mapped quad. mesh
Mapped meshing for hexa:
« simple » 3D primitives
here 1/8 of a sphere
Sweep meshing algorithms 3D
Sweep meshing for hexa.:
free quad mesh + extrusion
Sweep meshing for wedges :
free tri. mesh + extrusion
Free meshing algorithms 3D
Free tetrahedral meshing:
free advancing front 2D meshing + 3D adv. front tetrahedralization
the most general meshing algorithm in Abaqus/CAE
Partitioning

Goal


Method:


Cut edges, faces or volumes by planes, extrusions, sketch…
Useful to:




Decompose the geometry into simpler volumes / faces
Use structured or sweep meshing on certain region of the part
Enhance mesh quality & assign local refinements
Create new faces / edges for boundary conditions or output
Drawback:

If not used correctly: create a lot of small faces and edges =>
generate very small elements of bad quality
Example: see demo & tutorial
CAD & Meshing: continuity problem




Continuous Displacement field => need congruent
mesh on the boundaries with shared nodes at the
interface
Continuous mesh if and only if shared face or edge =>
When working with “imported” geometry, need to
« merge » boundary faces & edges!! => always check
for “Free edges” !!
Incompatible meshing methods can create “hanging”
nodes or displacement jumps which are not linked
across boundary; for example, linear to quadratic or
tetra to hexa transitions are not “compatible” =>
discontinuous displacement
If not possible to have shared boundaries, one need to
impose displacement compatibility through kinematic
constraints => additional equations (to avoid whenever
possible!!)
Incompatible Meshes
Hanging
nodes!!
Quadratic
Tetrahedral
Mesh
Quad.
Triangular
faces
Linear
Hexahedra
l mesh
Linear
Quadrangular
faces
Tetrahedral mesh regions can only be linked to prismatic (wedge) regions.
Prismatic regions can be linked to both hexa (along structured faces) and tetra.
Mesh quality

Criteria



Influence:






Geometry : Distortion ,aspect ratio, minimum angle, maximum
angle, …
FE-based: jacobian
Low quality = bad mesh convergence
Large stress field discontinuities
Some elements may « lock » for high aspect ratio
Create numerical « round-off » errors & singularities
May completely « crash » the solver if jacobian is negative !
Advice:


It is usually better to have « good quality » quadratic tetrahedra
than « highly deformed » hexahedra !!
Small edges & nearly tangent junction surfaces can be
problematic because they require too small or too sharp
elements => use virtual topology
CAD & Meshing: advices

In CAD:
 Create CLEAN parts for FEA:
 Avoid creating small surfaces & edges
 Avoid « tangent » connections (very small angles)
 Try to minimize the number of faces present in the model
 Prefer a single « sweep » / « loft » to complex cut / extrude
operations (=> can use structured meshing)
 Remove unsignificant geometric details:
 ask yourself what is important (abstraction) for the goal
of the modelling !!!
 Typical details: fillets / chamfers, small holes, unsignificant
components (bolts & nuts, rivets)
For complex parts / assemblies, it is usualy very time consuming to try
to « fix » the geometry & meshing problems, you should better
completely reconstruct a clean 3D CAD model just for FE analysis
CAD & Meshing: advices

In FEA pre-processor / mesher:
 Always
 If
check imported geometry (free edges?)
necessary: repair geometry or try a different format
 Partition
to create simpler volumes ( symmetries ? )
 Choice
of meshing method (if possible): Hex
structured > Hex swept > Wedges swept > Tetra free
 Use
compatible meshes at the interface !!!
 Check
mesh quality: at least no Analysis Error
 Define
local refinements where necessary
 Use
virtual topology if necessary