1. CAD Import Partitioning & Meshing
J.Cugnoni LMAF / EPFL 2011

2. CAD Model Structure Vertices (0D): Edges (1D): Surfaces (2D):
Coordinates & coordinate system
Edges (1D):
several 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

3. CAD Example 3D CAD volume:
all edges are shared between boundary faces =>
no « free » edges => surface is closed => it’s a volume!

4. 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 engine, native geometry format of Abaqus 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

5. 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

6. Meshing: basic principle

7. 1D Meshing algorithms Method: Definition:
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

8. 1D Meshing algorithms Constant element size
Biased element size distribution
Default (global) element size

9. Meshing algorithms 2D Methods: Definition:
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

10. Mapped meshing algorithms 2D
Mapped meshing (works for surfaces having 3 to 5 corners)

11. Free meshing algorithms 2D
Advancing front meshing
Medial axis meshing

12. Meshing algorithms 3D Methods: Definition:
Propagate 2D mesh in the volume
Algorithms:
Structured / mapped meshing :
map volume to a simple case (hexa)
Semi-structured:
« extrusion » / « sweep » of a free 2D mesh (tri or quad)
Generates either hexa or prisms (wedges)
Free meshing:
Delaunay or Advancing Front tetrahedralization
Definition:
Just select the meshing algorithm
Automatically inherits the mesh size from the surfaces & edges

13. Mapped meshing algorithms 3D
Mapped meshing for hexa:
« simple » 3D primitives
here 1/8 of a sphere
Mapped meshing for hexa:
any extrusion of mapped quad. mesh

14. Sweep meshing algorithms 3D
Sweep meshing for wedges :
free tri. mesh + extrusion
Sweep meshing for hexa.:
free quad mesh + extrusion

15. Free meshing algorithms 3D
Free tetrahedral meshing:
free advancing front 2D meshing + 3D adv. front tetrahedralization
the most general meshing algorithm in Abaqus/CAE

16. Example: see demo & tutorial
Partitioning
Goal
Decompose the geometry into simpler volumes / faces
Method:
Cut edges, faces or volumes by planes, extrusions, sketch…
Useful to:
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

17. 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!!)

18. Two disconnected CAD regions Presence of two bounding faces
=> Duplicated nodes & no continuity of displacement
Two connected CAD regions
only one shared bounding face
=> shared nodes so displacement is continuous at nodes
Shared bounding face / edge
Duplicated bounding face / edge

19. Incompatible Meshes
Quadratic
Tetrahedral Mesh
Linear Hexahedral mesh
Linear Quadrangular faces
Quad. Triangular faces
Hanging nodes!!
Tetrahedral mesh regions can only be linked to prismatic (wedge) regions.
Prismatic regions can be linked to both hexa (along structured faces) and tetra.

20. Mesh quality Criteria Influence: Advice:
Geometry : Distortion ,aspect ratio, minimum angle, maximum angle, …
FE-based: jacobian
Influence:
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

21. 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

22. CAD & Meshing: advices In FEA pre-processor / mesher:
Always check imported geometry (free edges?)
If 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