The commands to
subdivide a macro structure into finite elements are grouped together under a
common dialog with property sheets. The dialog is made active by the command „Subdivision“ and remains active until it is closed by
pressing „Cancel“. Pressing „Plot“ causes the current subdivision data to be
plotted.
The following
commands are available:
Define
reference points for subdivision of macro elements |
|
The subdivision
of macro elements into finite elements is done by applying various patterns. It
is distinguished between regular subdivisions where opposite edges are
subdivided identical and irregular subdivisions. The patterns are distinguished
by a unique pattern ID.
The regular
subdivision is selected by ID 20, 40, 40 for macro elements of type 2x, 4x, 8x
and by ID 134, 30, 30 for types 3x and 6x (x = 0,2,5). The regular subdivision
is set by default for all elements after initialization.
The irregular
subdivision allows step-by-step refinements of the element mesh. There are
several transition patterns available. Transition patterns are selected by IDs
greater 100. The most flexible pattern is the pattern with ID 142 respectively
150, where all edges can have any number of subdivisions.
Solid elements
only have transition patterns for the bottom surface. The third direction
(z-direction) only can regularly be subdivided. The number of subdivisions for
this direction is specified with the command Pattern.
For each pattern
you’ll have to define the number of subdivisions (number of intermediate nodes)
for all edges of the bottom surface of the macro element in counter clock wise
order. With solid elements also the number of intermediate nodes for the third
direction must be given.
Marking the
resulting intermediate nodes with a graphical symbol can graphically show
subdivision data for edges. A shrink plot of elements may be especially useful
to check the subdivision of adjacent edges. The main directions of macro
elements will also be plotted to show the orientation of elements. This
information will be needed for the command Pattern
where the subdivision for individual directions of the elements must be
specified.
For the
specification of a subdivision the following commands are available:
Pattern specifies
the subdivision data (pattern ID + number of intermediate nodes for element
edges) for individual elements
Edges specifies subdivision data for
individual edges of the structure where it’s possible to have an automatic
regular continuation for the complete structure or selected elements by
assigning the same subdivision to opposite edges.
Continuation applies
existing subdivision data for individual edges to opposite edges, similar to
command Edges
Division assigns subdivision patterns in the
way that the resulting edges of the generated finite elements are all smaller
than the given value. It’s also possible to specify that opposite edges get the
same number of subdivisions (regular pattern).
Reference Point allows defining fixed points on
edges that should be considered when the element is subdivided.
Check does consistency checks on the existing subdivision data.
Edges are checked whether adjacent elements are equally subdivided. Optionally
a given inconsistency can be automatically corrected.
Note: Consistency checks for adjacent elements
require the use of identical nodes for common edges. Plotting the boundary
edges of a structure can check this. By using the command Compress nodes (see chapter “General commands“) it’s possible
to merge those narrow nodes into a single node.
The easiest way
to specify subdivisions is by using the command Division. It’s possible to specify different
granularity’s for different parts of the structure by using this command
several times with different values for different element sets. Inconsistency
between the parts must then be corrected with command Check.
To get a mostly
regular subdivision to macro elements, following steps should be used:
Specify
transition patterns for individual elements with the command Pattern.
Continue
the subdivisions of the edges for adjacent elements
Specify a
regular subdivision of all the remaining elements with Division and option “Continue”.
Check and
correct consistency of subdivision data with Check
Note: The
subdivision of macro elements only creates finite elements with straight edges
or one intermediate node on edges. To get elements with two nodes between
vertices or additional nodes inside the element, the command Type2Type has to be applied to change the element type
and to generate additional nodes.
Note: The
number of intermediate nodes on edges is limited to 60 nodes per edge. The
structure may be subdivided in several steps by transferring a new created FE
structure to a macro structure (command Macro <-> FE) and subdivide the new macro structure.
Note: If
transition patterns are used some triangular elements may be created. To avoid
this, first create Finite Elements with double edge length and subdivide these
elements again by using a regular pattern with one intermediate node on edges.
Performing
the subdivision of macro elements (Generating finite elements)
The subdivision
is done by the command Subdivision
The calculation
of additional nodes during the subdivision is done, on the basis of the
assigned pattern, by a C0-Coons interpolation of surfaces within the
global coordinate system. In some cases, for example nodes on a spherical or
cylindrical surface, it may be necessary to smooth the resulting nodes with the
command Smooth. This will for example be the case
when describing a cylindrical section by an element with spline curves.
The numbering of
the generated nodes of the finite element structure is done by the following
scheme: The 3 dimensional space where the entire finite element structure is
contained within is separated into small cubes. The generated nodes will have a
continuous numbering based on the cube they fall into where x-direction comes
before y-direction followed by z-direction. With the command Sort a different numbering scheme may be applied.
Each individual
macro element is subdivided into finite elements based on the previously
defined subdivision data. Afterwards nodes on common element edges or surfaces
or nodes with identical coordinates (within a given tolerance) are combined
into only one node (see parameter eps for the command Subdivision).
Attention:
Merging of nodes may be critical, if you don‘t give a value for eps, the chosen
value is determined considering the length of all elements and may be to small.
In any case check whether there are nodes within a small distance that should
be merged into a single node by plotting sharp edges or by using the command Compress nodes.
The consistency
of the generated Finite Element mesh can only be guaranteed if adjacent macro
elements have identical edges with identical vertices and if subdivision data
for these macro elements is also identical (edge related). This consistency
will be checked automatically before doing the subdivision. Found
inconsistencies will be shown on the screen. If any inconsistencies are found,
it will be asked for further processing. The same mechanism can be used with
the command Check where all edges with inconsistent
subdivision data are graphically shown and these inconsistencies may optionally
automatically be corrected.
Note: For
beam elements (type 2x) with an additional third node for defining the main
section, this third node will also be present for all the generated finite
elements.
Note: The
subdivision of a macro element for a specific pattern is first done for a unit
element. Afterwards the mesh is mapped to the geometry of the macro element. In
case of large distortions the resulting mesh may become unpredictable so it may
be useful to modify the macro structure to less distorted elements.
command Continuation.