Next: seqa Up: Commands Previous: scal Contents

##
send

       'send' <set> 'abq'|'ans'|'ast'|'duns'|'fbd'|'frd'|'nas'| ->
                    'stl'|'tcg' <RETURN>|
                    ['lc <nr>']|
                    ['tmf']|
                    ['sta' <refspeed>]|
                    ['crp' <timefact> <refspeed> <writefreq>]|
                    ['comp']|
                    ['mpc' <rotation> <v1> <v2> <v3>]|
                    ['names']|
                    ['spc' <dofs(1-6)> <value>]|
                    ['slide' 's'|'rx'| ->
         'ry'|'rz'|'tx'|'ty'|'tz']|
                    ['pres' [<value>]|['lc'<nr> 'e'<nr>]]|
                    ['film' [[<temp>]|['lc'<nr> 'e'<nr>]] ->
         [[<coeff>]|['lc'<nr> 'e'<nr>]] ]|
                    ['rad' [[<temp>]|['lc'<nr> 'e'<nr>]] ->
         [[<emis>|['lc'<nr> 'e'<nr>]] ]|
                    ['dflux' [[<load>]|['lc'<nr> 'e'<nr>]] ]|
                    ['cflux' <load>]|
                    ['force' <f1> <f2> <f3>]|
                    ['sur']
       'send' <set> ['duns'|'isaac'|'foam'] [<base-type> <set>]| ->
         ['cyclic' <set> <set> 'tx'|'ty'|'tz'|'rx'|'ry'|'rz'| ->
                               'cx'|'cy'|'cz'|<vx,vy,vz>]
       'send' <dep-set> <indep-set> 'nas'|'abq'|'ans' ['cycmpc' ->
         'rx'|'ry'|'rz'|'cx'|'cy'|'cz'<segments> 'c'|'u'<NR>]| ->
         ['areampc' <dofs(1-6,t)> 'c'|'u'<Nr>]| ->
         ['areampc' 'slide']| ->
         ['areampc' 'presfit' ['s'<value>]]| ->
         ['gap' <vx> <vy> <vz> <tol>]

This keyword is used to send data to the file-system. The following formats are known (but not all options for all formats are fully supported so far); The geometry-format (fbd)
send all fbd
and a surface description with triangles (stl)
send all stl
Beside the stl file a so called edge file for NETGEN will be created if be2 elements are included in the mesh. The following mesh-related formats are known: Femview and Fam (frd), Nastran (nas), Abaqus (abq), Ansys (ans), CodeAster (ast), Samcef (sam) and Tochnog (tcg) but only ccx (Abaqus) is fully supported. Good support is also provided for ansys and nastran. 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. If the parameter ``lc'' follows
send set abq lc 1
then the values stored in Dataset 1 are written (works only on scalar datasets like temperatures and only for certain formats, for frd the lc parameter w/o any further values forces cgx to write all datasets but w/o the internally calculated ones). If the parameter ``tmf'' follows
send set abq tmf
then the mesh plus all temperatures with the necessary solver context for tmf calculations is written. If the parameter ``sta'' follows
send set abq sta 2900.
then the mesh plus all temperatures with the necessary solver context for a static calculations is written. Here the value for ``speed'' is a reference value for eventual nummerical values in the TEXT-Block of the Datasets (see ``Nodal Results Block''). If the parameter ``crp'' follows
send set abq crp 1. 2900. 1
then the mesh plus all temperatures with the necessary solver context for creep calculations is written. Here the value for ``timefact'' scales the time-values of the Datasets, ``speed'' is a reference value for eventual nummerical values in the Text-Block and scales values from a default load-file and writefreq limits the output to the result-file.

Special cases are the cfd-solvers Duns, Isaac and OpenFoam. The boundary patches are an integral part of the mesh. So it is necessary to specify all boundary patches when writing the mesh. All free surfaces of the mesh must be specified. This is an example for OpenFoam:
send all foam cyclic cyc1 cyc2 cx patch in patch out wall wall
will write the so called polyMesh description to the file-system. After the send command the set (all) with the mesh is specified, then the format (foam), then cyclic boundary conditions (cyclic cyc1 cyc2 cx) between set cyc1 and cyc2 of the axi-symmetric case around x (cx), then boundary conditions of type patch for set ``in'' (patch in), then boundary conditions of type patch for set ``out'' (patch out) and boundary conditions of type wall for set ``wall'' (wall wall).

The symmetric boundary-conditions (base-type: cyclic) can be axi-symmetric (c) around x,y,z or rectangular (r) in direction of x,y,z. Only for OpenFoam and in the rectangular (kartesian) case also a vector pointing in the direction of the symmetry can be specified (ie: 1.,1.,0.)

For isaac and duns the same syntax has to be used:
send all duns viscous-wall profil subsonic-inflow in subsonic-outflow out
send all isaac WALL profil FARFIELD far EXTRAPOLATE out
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 in a new session. 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 the solver then just the element- or node-numbers are 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. The user has to refer this numbers in the duns.script2 file when describing boundary conditions.

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 and optionally a forced deflection. 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. And
send moved-nodes abq spc 1 0.1
will move the nodes in set moved-nodes by 0.1 in 1 direction.

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 you type:
send sur abq slide s
and this should attach the node with the node-nr. 1 to a plane parallel to the surface of the corresponding element-face. This element uses the node 1, 2, 3, 4, 5, 6, 7 and 8 where 1, 2, 3 and 4 are on the surface of the mesh. The program will detect this element face and constrain the node only if the nodes 2, 3 and 4 were also included in the set ``sur''. The detected elements or faces of volume-elements will be assigned to the set. So it is possible to check the detected elements. Instead of providing a set with the necessary nodes, you might instead provide a set with shell-elements or/and faces of volume-elements. The nodes will be derived from them. In most cases this is the most convenient way.

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. For example
send surf abq pres 0.05
will assign the pressure value 0.05 to all element-faces in set surf. If a dataset with nodal values is available it is also possible to use this values instead of using a uniform value for all faces. For example
send surf abq pres lc1 e1
will specify the dataset-nr 1 and the entity-nr 1 to be used instead of a uniform value.

The parameter ``film'' is used to assign free-stream temperatures and thermal heat coefficients to element faces. It works similar to the ``pres'' option. For example
send surf abq film 1200. 0.5
will assign the film temperature of 1200 and the coefficient 0.5 to all element-faces in set surf. If datasets with nodal values are available it is also possible to use this values instead of using a uniform value for all faces. For example
send surf abq film lc1 e1 0.5
will specify the dataset-nr 1 and the entity-nr 1 to be used for the temperature instead of a uniform value, or
send surf abq rad lc1 e1 lc1 e2
will specify also the dataset-nr 1 with the entity-nr 2 to be used for the film-coefficients instead of a uniform value.

The parameter ``rad'' is used to assign a sink temperatures and the emissivity to element faces. It works similar to the ``pres'' option. For example
send surf abq rad 1200. 0.5
will assign the sink temperature of 1200 and the emissivity 0.5 to all element-faces in set surf. If datasets with nodal values are available it is also possible to use this values instead of using a uniform value for all faces. For example
send surf abq rad lc1 e1 1200.
will specify the dataset-nr 1 and the entity-nr 1 to be used for the temperature instead of a uniform value, or
send surf abq rad lc1 e1 lc1 e2
will specify also the dataset-nr 1 with the entity-nr 2 to be used for the emisivity instead of a uniform value.

The parameter ``dflux'' is used to assign an energy stream to element faces. It works similar to the ``pres'' option. For example
send surf abq dflux 0.5
will assign the flux of 0.5 to all element-faces in set surf. If a dataset with nodal values is available it is also possible to use this values instead of using a uniform value for all faces. For example
send surf abq dflux lc1 e1
will specify the dataset-nr 1 and the entity-nr 1 to be used instead of a uniform value.

The parameter ``cflux'' is used to assign an energy stream to nodes. For example
send surf abq cflux 0.5
will assign the flux of 0.5 to all nodes 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. Two files are produced. The one with the equations has to be included in the model-definition-section and the boundary-file in the step section.

The special purpose parameter ``sur'' will write the surfaces of the mesh either in abaqus-format for the *SURFACE command or in frd-format as shell elements with a dataset describing the normals. For example
send top abq sur
will write the elements in set top together with the face-identifier of the free element-faces.
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''. A thermal connection is created with:
send dep indep nas cycmpc tx c
The thermal connection is triggered by the ``t''. See comments above for the single parameters.

Another useful method is to ``glue'' independent meshes together. 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. 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 numbers ``123'' are the degrees of freedom which will be connected (``t'' will create a thermal connection). 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).

A special case is considered with the ``slide'' option in combination with the ``areampc'' option. For example if the mesh of a turbine-blade and a disk should be connected to each other then a sliding condition between this parts is necessary. The command:
send dep indep abq areampc slide
will connect the nodes in the set dep to element-faces described by nodes included in the set indep but only in the direction perpendicular to a plane defined by nodes of the dep-set. Therefore all dep-nodes and all indep-nodes must lie in the same plane and will slide in the same plane!

Another special case is considered with the ``presfit'' option in combination with the ``areampc'' option. For example if a cylindrical press fit should be simulated then a forced displacement between the two intersecting surfaces is necessary. This forces the dependent nodes to move to the independent face. Two modes are available:
send dep indep abq areampc presfit f
simulates sticking friction and with the option s
send dep indep abq areampc presfit s
works for sliding conditions. The user might request a certain value for the press fit if the overlapping of the mesh do not represent the necessary distance:
send dep indep abq areampc presfit s0.06
will move the dep-nodes 0.06 in the normal direction of the independent faces (works also with option f). Additional nodes are generated and can be used to request the reaction forces on the dependent nodes. They are stored in a set named N<dep-set-name><ind-set-name>. Two files are produced. The one with the equations has to be included in the model-definition-section and the boundary-file in the step section.

Also it is possible to define so called ``gap'' elements and related control-commands. These elements will connect parts if they are closer as a certain distance. For example if the distance is zero (contact). The command:
send dep indep abq gap 1. 0. 0.
will connect the nodes in the set dep and indep with gap-elements but only if they match each other in the direction 1.

Next: seqa Up: Commands Previous: scal Contents