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.