Keyword type: model definition
This keyword is used to define submodel boundaries. A submodel is a part of a bigger model for which an analysis has already been performed. A submodel is used if the user would like to analyze some part in more detail by using a more dense mesh or a more complicated material model, just to name a few reasons. At those locations where the submodel has been cut from the global model, the boundary conditions are derived from the global model results. These are the boundaries defined by the *SUBMODEL card. In addition, in a purely mechanical calculation it allows to map the temperatures to all nodes in the submodel (not just the boundary nodes).
There are three kinds of boundary conditions one may apply: the user may map the displacements from the global model (or temperatures in a purely thermal or a thermo-mechanical calculation ) to the boundaries of the submodel (Dirichlet boundary conditions), the user may want to map the stresses to the boundaries of the submodel (Neumann or natural boundary conditions) or the user may select to map the temperatures in a purely mechanical calculation to all nodes belonging to the submodel (Dirichlet boundary conditions). Mapping the stresses may require fixing a couple of additional nodes to prevent rigid body modes.
In order to perform the mapping (which is basically an interpolation) the global model is remeshed with tetrahedra. The resulting mesh is stored in file TetMasterSubmodel.frd and can be viewed with CalculiX GraphiX.
There are three parameters of which two are required. The parameters TYPE and INPUT are required. TYPE can take the value SURFACE or NODE, depending on whether the user wants to define stress boundary conditions or displacement/temperature boundary conditions, respectively. The parameter INPUT specifies the file, in which the results of the global model are stored. This must be a .frd file.
A submodel of the SURFACE type is defined by element face surfaces. These must be defined using the *SURFACE,TYPE=ELEMENT card. Submodels of the NODE type are defined by sets of nodes. Several submodel cards may be used in one and the same input deck, and they can be of different types. The global result file, however, must be the same for all *SUBMODEL cards. Furthermore, a node (for the NODE type submodel) or an element face (for the SURFACE type submodel) may only belong to at most one *SUBMODEL.
The optional parameter GLOBAL ELSET defines an elset in the global model which will be used for the interpolation of the displacements or stresses onto the submodel boundary defined underneath the *SUBMODEL card. Default is the complete global model. Global elsets of different *SUBMODEL cards may have elements in common.
Notice that the *SUBMODEL card only states that the model at stake is a submodel and that it defines part of the boundary to be of the Dirichlet or of the Neumann type. Whether actually displacements or stresses will be applied by interpolation from the global model depends on whether a *BOUNDARY,SUBMODEL, *DSLOAD,SUBMODEL or *TEMPERATURE card is used, respectively.
First line:
Following line for TYPE=NODE:
Following line for TYPE=SURFACE:
Example: *SUBMODEL,TYPE=NODE,INPUT=global.frd part, 1, 8
states the the present model is a submodel. The nodes with number 1, and 8 and the nodes belong to a Dirichlet part of the boundary, i.e. a part on which the displacements may be obtained from the global model. The results of the global model are stored in file global.frd. Whether they are really used, depends on whether a *BOUNDARY,SUBMODEL card is defined for these nodes.
Example files: .