ANSYS Multiphysics offer the user several hundred finite element types to use in their analysis. Not all elements support all degrees of freedom / physics. Some are optimized for 2-D analysis, others 3-D. A large range of element shapes are available offering the user many approaches to meshing their solid model. A non solved surface ad volume element (MESH200) is also available to allow a user to define the mesh on surfaces prior to sweeping the 2-D mesh into a 3-D volume.
A user typically builds or imports a MEMS model using the ANSYS Multiphysics geometry preprocessor. The geometry can be sliced and diced to make use of symmetry, or for the purpose of geometry defeaturing. After selecting an element type, a line, area or volume can be automatically meshed using our smart mesh tool, or alternatively more experience users can take direct control over the meshing attributes. Extremely detailed control is provided, such a line divisions, mesh concentration about keypoints, mesh expansion/contraction into a volume. Users can also concatenate line or areas to allow complex geometry to be mapped mesh. ANSYS Multiphysics will also automatically map mesh a geometry if this is doable. The ANSYS MEMS training course provides full details about how to efficiently mesh MEMS devices, including high aspect ratio surface micro machined geometry.
The following image is the ANSYS Multiphysics mesh toolbar. This is one of a suite of tool used to set up and control mesh parameters:
The following is a simple meshing example (for ANSYS Multiphysics 7.0) showing how a high aspect ratio volume with a tapered side wall can be efficiently map (brick) meshed. The key command used the VSWEEP command which sweeps a meshed area into a volume. The source and target areas are defined and the user also has control over the number of elements created along the "depth" of the sweep.
!
! VSWEEP example
!
/PREP7
ET,1,SOLID5 ! Element type
BLC5,0,0,0.8,0.4 ! Create a rectangular area
VEXT,1, , ,0,0,0.05,0.9,0.9,, ! Extrude the area in the z -direction, and scale it to create a tapered side wall
ET,2,MESH200 ! Unsolved element type used to define area mesh for sweep.
KEYOPT,2,1,6
KEYOPT,2,2,0
type,2 ! Use the unsolved element type for the following meshing commands
MSHAPE,0,2-D
MSHKEY,0
AMESH,1 ! mesh the first area
type,1 ! Use the SOLID45 element type for the following mesh commands
esize,,4 ! define the number ofeleents along the extrusion
vsweep,1,1,2 ! Sweep the area mesh into the volume
eplot ! plot the elements created
!
! EOF
!
The mesh this input files creates is shown below:
