MESH_SMOOTH


ID_NAME	= <`name_of_mesh_smooth`>	Name of the `MESH_SMOOTH` definition.
EL_GROUP	= <`name_of_element_group`>	Name of the element group for which `MESH_SMOOTH` is done.
MS_LAYER	= <`name_of_node_group`>, <`number_of_elementlayers`>	The mesh smooth element group is defined automatically. Starting with the referenced node group and the defined number of grouped element layers.
FREE_SF	= FIX, 0 = FIX, <`number_of_node_layers`>	Free surface nodes of the `MESH_SMOOTH` area, which is completely fixed (number of node layers <`number_of_node_layers`> depending on the remaining free design nodes).
	= FREE	Free surface nodes of the `MESH_SMOOTH` remaining free area (not fixed).
BOUNDARY	= FIX	Nodes on the border of the mesh smooth area are fixed.
	= FREE	No nodes are automatically fixed.
STRATEGY	= CONSTRAINED_LAPLACIAN	Use constrained Laplacian `MESH_SMOOTH` strategy.
	= LOCAL_GRADIENT	Use local gradient mesh smooth strategy; not recommended for models with many nodes in mesh smooth area.
	= EXTERNAL	Use an external mesh smooth code; recommended for CST solver.
LEVEL_QUAL	= NOT = LOW = MEDIUM = HIGH	Parameter to set the quality of the mesh. Increasing mesh quality with `NOT` -> `LOW` -> `MEDIUM` -> `HIGH`.
QUAL_LIST	= YES	List of the qualitative bad elements.
	= NO	No list of the qualitative bad elements.
QUAD_LOW_ANGLE	= <`value`> = 20	Angle between 0 and 89 degrees.
QUAD_HIGH_ANGLE	= <`value`> = 160	Angle between 91 and 180 degrees.
TRIA_LOW_ANGLE	= <`value`> = 20	Angle between 0 and 59 degrees.
TRIA_HIGH_ANGLE	= <`value`> = 140	Angle between 61 and 180 degrees.
TETRA_LOW_ASPECT	= <`value`> = 0.222	Value between 0.00177 and 1.30.
TETRA_ HIGH_ASPECT	= <`value`> = 8	Value between 1.36 and 999.
SOLVER_CHECK	= YES	The solver quality criteria are checked.
	= NO	The solver quality criteria are not checked.
SOLVER_STOP	= YES	Optimization is stopped if quality criteria are not satisfied.
	= NO	No stop.
Q4TAPER	= <`value`> = 0.5	Value for `Q4TAPER` (greater or equal 0).
Q4SKEW	= <`value`> = 30	Angle for `Q4SKEW` (greater or equal 0).
TETRAAR	= <`value`> = 100	Value for `TETRAAR` (greater or equal 0).
T3SKEW	= <`value`> = 10	Angle for `T3SKEW` (greater or equal 0).
FREEZE_DESIGN_NODES	= YES = NO	Do not modify design nodes during the mesh smoothing step if set to `YES`.
CORRECT_ ELEMENTS	= YES = NO	Correct supported elements that got too much distorted during optimization.
CE_CORRECTION_FACTOR	0 <= (`<value>)` < 1 = 0.5	Correct elements by multiplication of optimization displacements with this factor.
CE_CORRECTION_LOOPS	= <`int_value`> = 4	Trying to correct a single element <`int_value`> times.
CE_FAIL_ACTION	= RESET = CONTINUE	Handling of not correctable elements: RESET: Optimization displacement is set to zero for the current iteration. CONTINUE: Do nothing and risk a solver failure.

Items for STRATEGY = CONSTRAINED_LAPLACIAN


LEVEL_CONV	= LOW = MEDIUM = HIGH	Convergence parameter of `MESH_SMOOTH`.
LEVEL_DVCON	= NOT = LOW = MEDIUM = HIGH	Parameter for verifying frequency of `DVCON_SHAPE` entries during `MESH_SMOOTH`.

Items for STRATEGY = LOCAL_GRADIENT


FEATURE_RECOGNITION	= <`value`> = 30	Angle used for recognition of edges and corners (greater or equal 0).

Items for STRATEGY = EXTERNAL


FILE	= delta_mesh.onf <`file_name`>	Optional file containing the mesh smooth distortions.

Remarks

In MESH_SMOOTH, certain elements are not permitted (for example, beam elements, for more information refer to the User Manual). From the user-defined element group, a system-defined element group with the name Mesh_smooth_id_name_'ELEM' is created. The non-permitted elements are eliminated and a system-defined node group Mesh_smooth_id_name_'NODE' is generated. That group contains all the required boundary nodes.
The calculation time for MESH_SMOOTH increases with an increase in the number of iterations, that is, LEVEL_CONV=LOW is faster as HIGH. A higher convergence parameter gives a better result in MESH_SMOOTH. The aim for the user is: work with the lowest convergence parameter as possible and only switch to the next highest convergence parameter when having problems.
BOUNDARY: MESH_SMOOTH is working on an element group and changes resulting from mesh smoothing should remain within this group. The BOUNDARY=FIX option is used to fix the nodes (inner and surface nodes) at the border of the mesh smooth area defined by the element group. In common, this behavior is preferred. All nodes fixed by these settings are stored a node group with the name <Mesh_smooth_id_name>_BOUN. If you do not want the "border" nodes to be fixed, you can select the BOUNDARY = FREE option. Then you are responsible to fix the proper nodes by yourself using DVCON_SHAPE entries.
FREE_SF: Free surface nodes include all surface nodes of the MESH_SMOOTH area that are neither design nodes (command DV_SHAPE operator ND_GROUP) or restricted in any way (command DVCON_SHAPE operator ND_GROUP). The specified number of node layers <number_of_node_layers> controls the area that is used for remeshing. If surface nodes are fixed with FREE_SF=FIX, a node group <Mesh_smooth_id_name>_SF is automatically created and a DVCON_SHAPE entry <Mesh_smooth_id_name>_SFIX is generated. The relevant entry for DVCON_SHAPE is then automatically activated in OPTIMIZE.
Calculation time for MESH_SMOOTH increases when the sequence is changed, LEVEL_DVCON = NOT -> LOW -> MEDIUM -> HIGH. The user should work with the lowest parameter possible and only switch to the next highest parameter when problems arise.
LEVEL_QUAL: Calculation time for MESH_SMOOTH increases in the sequence LEVEL_QUAL = NOT -> LOW -> MEDIUM -> HIGH. The user should work with the lowest parameter possible and only switch to the next highest parameter when problems arise. With LEVEL_QUAL=NOT the entries for QUAL_LIST, QUAD_LOW_ANGLE, QUAD_HIGH_ANGLE, TRIA_LOW_ANGLE, TRIA_HIGH_ANGLE, TETRA_LOW_ASPECT, TETRA_HIGH_ASPECT do not have any influence.

Determining quality: To determine the quality of an element, the angle of the element is determined. Tetrahedron elements have the additional quality determination of the aspect ratio. The value of quality is between 1 (the best element quality) and 0 (the worst element quality). Using the parameter QUAL_LIST the list of specifications of the worst elements are controlled with a quality of zero. The values shown with the help of QUAL_LIST are only internal values for MESH_SMOOTH and might be different from values of preprocessors.


QUAD surfaces (QUAD element, side surfaces from HEXA elements):
Optimal angle is 90 degrees:	Quality=1
Angle less than and equal to `QUAD_LOW_ANGLE`:	Quality=0
Angle greater than and equal to `QUAD_HIGH_ANGLE`:	Quality=0
TRIA surfaces (TRIA elements):
Optimal angle is 60 degrees:	Quality=1
Angle less than and equal to `TRIA_LOW_ANGLE`:	Quality=0
Angle greater than and equal to `TRIA_HIGH_ANGLE`:	Quality=0
TRIA surfaces (side surfaces from TETRA elements):
Optimal aspect ratio is 1.33 degrees:	Quality=1
Aspect ratio less than and equal to `TETRA_LOW_ASPECT`:	Quality=0
Aspect ratio greater than and equal to `TETRA_HIGH_ASPECT`:	Quality=0

Solver criteria of quality: SOLVER_CHECK must be activated so SOLVER_STOP can be executed. With SOLVER_CHECK=NO the entries SOLVER_STOP, Q4TAPER, Q4SKEW, TETRAAR, T3SKEW have no effect. The values found in Tosca Structure should be identical to the values set in the solver. A meaningful program stop in Tosca Structure because of bad mesh quality is better than having errors in the solver.

Example


MESH_SMOOTH
  ID_NAME  = my_mesh_smooth
  EL_GROUP = all_elements
  FREE_SF  = FIX, 3
END_