Next: seqa Up: Commands Previous: save Contents

##
send

       'send' <set> 'abq'|'ans'|'duns'|'fbd'|'frd'|'nas'|'tcg' <RETURN>|
                                            ['comp']|
                                            ['mpc' <rotation> <v1> <v2> <v3>]|
                                            ['names']|
                                            ['spc' <dofs(1-6)>]|
                                            ['slide' 's'|'rx'| ->
       'ry'|'rz'|'tx'|'ty'|'tz']|
                                            ['pres' <value>]|
                                            ['force' <f1> <f2> <f3>]|
                                            ['sur']
       'send' <dep-set> <indep-set> 'nas'|'abq'|'ans' ['cycmpc' ->
       'rx'|'ry'|'rz'|'cx'|'cy'|'cz'<segments> 'c'|'u'<NR>]|
                                                      ['areampc' ->
        <dofs(1-6)> 'c'|'u'<Nr>]\n");

This keyword is used to send data to the file-system. The following formats are known; one geometry-format (fbd)
send all fbd
and different mesh-related formats: Femview and Fam (frd), Nastran (nas), Abaqus (abq), Ansys (ans) and Tochnog (tcg). If no further parameter follows then just the definition of the nodes and elements will be written:
send all abq
will write the mesh in the format used by Abaqus and the CalculiX solver. A special case is duns, a cfd code, using only a grid instead of a mesh. This grid is automatically written during meshing.

The command
send set frd
will write nodes and/or elements in frd format. This file could be read in again later on to define sets during post-processing (see read) or just to look at it. If the parameter ``comp'' follows and the set includes not all nodes used by the included elements then missed nodes will be detected and stored as well in the set before the set is written, for example:
send elem frd comp
will at first include all nodes used by the elements to the set elem and will then write the file.

If the parameter ``names'' follows then just the element- or node-numbers will be written. This is useful for defining sets for the solvers:
send steel abq names
will write the the element numbers included in ``steel''. This file could be used to define a set for material assignments. If the solver-format ``duns'' is used then related numbers of surfaces (3D) or lines (2D) will be written. This information is necessary to apply boundary-conditions to duns. The numbers are used in the connectivity file (duns.conn) which will be created by the mesh-command.

It is also possible to define and send some constrains to the file system. To constrain degrees of freedom (dof) of selected nodes use the parameter ``spc'' in combination with the numbers of the constrained dofs. For example:
send hinge abq spc 123
will constrain the translational degrees of freedom of the nodes in set ``hinge''. Or
send hinge abq spc 12356
will leave just one rotational degree of freedom unconstrained.

The parameter ``slide'' in combination with one additional parameter will create equations that force the selected nodes to move only along a plane. If the additional parameter ``s'' is specified then the specified nodes will be attached to their element faces. But this will work only if enough nodes are selected to fully describe the element faces to which the nodes belong. For example
send sur abq slide s
should attach the surface node with the node-nr. 1 to the surface of the mesh. The node is used by the element nr. 10. This element uses the node 1, 2, 3, 4, 5, 6, 7 and 8 where 1, 2, 3 and 4 are lying on the surface of the mesh. The program will detect this element face only if the nodes 2, 3 and 4 were also included in the set ``sur''. The detected elements will be assigned to the set. So it is possible to check if some elements were missed.

If nodes should slide radially to the y axis then use ``ry'':
send sur abq slide ry
or use ``ty'' if the nodes should move only tangential to the y axix. In both cases the axial movement is still permitted.

The parameter ``pres'' is used to assign pressure values to element faces. It works similar to the ``slide s'' option. All element faces that should see the pressure must be fully defined by the nodes included in the specified set. For example
send surf abq pres 0.05
will assign the pressure value 0.05 to all fully described element faces in set surf.

The parameter ``force'' is used to assign force values to nodes. For example
send nodes abq force 1. 20. 0.
will assign the specified forces to all nodes of the set nodes.

The parameter ``mpc'' is used to create input for the user-subroutine umpc which forces all nodes from ``set'' to rotate by an average value specified with ``rotation'' around the vector v. The value has to be in degree were 90 degree is orthogonal. For example
send nodes abq mpc 4. 1. 0. 0.
will assign the nodes of the set ``nodes'' to the user-subroutine umpc and will force them to rotate by 4 degree around the x-axis.

The special purpose parameter ``sur'' works only for the frd format and will write the surfaces of the mesh as shell elements with a dataset describing the normals (element-data, not supported by cgx so far).
In addition it is possible to define so called ``cyclic symmetry'' equations. These equations are used when just a section of a rotation-symmetric part like a disk is modeled. These equations force the two cutting planes of such a section to move exactly equal in the cylindrical system. If the coordinate system of the displacements for the solver is rectangular (xyz) then the syntax is:
send dep indep nas cycmpc rx12 c1
Here ``dep'' is the set containing the nodes of the dependent side. These nodes will be replaced by the solver with the independent nodes from the set ``indep''. In this case the equations will be written in the nastran format ``nas'' (in nastran called MPC). The parameter ``rx12'' defines the displacement system as rectangular ``r'', the rotational axis is ``x'' and the ``12'' defines the number of segments in 360 deg, therefore the angle of the segment is 360 deg /12. If omitted then the value is calculated for each node separate. The ``c'' triggers the correction of the position of the dependent nodes to a position defined by the angle of the segment (highly recommended), ``u'' would prevent the correction. The ``1'' will be the identifier for the equations if the format is nas (nastran). In case the format would be ans (ansys) then the ``1'' would be the number of the first equation. No number is required for abq (abaqus and calculix). If the coordinate system of the displacements is cylindrical (rtz) then the example would be:
send dep indep nas cycmpc cx12 c1
Only the ``r'' from ``rx12'' is changed to ``c''. But so far a cyclindrical system is not supported by the calculix solver (Version 0.9).

Another useful method is to ``glue'' independent meshes together. For example if the mesh ofa blade and a disk are not connected but should be connected to each other. For this the dependent nodes are tied to independent elements by equations. Choose the finer mesh for the dependent side. The equations are based on the shape-functions of the element types. So far only the 8 and 20 noded brick elements and the tet4 element are supported by the correct shape functions. For example
send dep indep nas areampc 123 c1
will connect the nodes in the set dep to element-faces described by nodes included in the set indep. The set dep must contain all nodes which should be ``glued'' and the set indep should contain all nodes of the elements surfaces to which the dep nodes should be glued. The number ``123'' are the degrees of freedom which will be connected. The ``c'' triggers the correction of the position of the dependent nodes to a position on the surface of the independent elements (highly recommended), ``u'' would prevent the correction. The ``1'' will be the identifier for the equations if the format is nas (nastran). In case the format would be ans (ansys) then the ``1'' would be the number of the first equation. No number is required for abq (abaqus and calculix).

Next: seqa Up: Commands Previous: save Contents