## *SUBMODEL

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 four 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, the stresses to the boundaries of the submodel, the forces to the boundaries of the submodel or the user may select to map the temperatures in a purely mechanical calculation to all nodes belonging to the submodel. Mapping the stresses or forces 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/force 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. It is not allowed to define a local coordinate system (with a *TRANSFORM card) in these 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. For the creation of this element set the parameter GENERATE is not allowed (cf. *ELSET). Although this element set contains element numbers belonging to the global model, it must be defined in the submodel input deck using the *ELSET card. For instance, suppose the global model contains elements from 1 to 1000 and that the submodel contains only 10 elements numbered from 1 to 10. Both models have no elements in common, however, they may have element numbers in common (as is the case in this example). Suppose that the global elements to be used for the interpolation of the boundary conditions onto the submodel have the numbers 600 up to 604. Then the following card defines the global elset

*ELSET,ELSET=GLOBALSET1
600,601,602,603,604


and has to be included in the submodel input deck, although in this deck only elements 1 to 10 are defined by a *ELEMENT card, i.e. in the submodel input deck element numbers are referenced which are not at all defined within the deck. This is fine for submodel decks only.

If no GLOBAL ELSET parameter is used the default GLOBAL ELSET 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 nodal or of the surface type. Whether actually displacements or stresses will be applied by interpolation from the global model depends on whether a *BOUNDARY, *DSLOAD, *CLOAD or *TEMPERATURE, card is used, respectively, each of them accompanied by the parameter SUBMODEL.

Mapping displacements or temperatures to the boundary of a submodel is usually very accurate. For stresses, the results may be unsatisfactory, since the stress values stored in the global model (and which are the basis for the interpolation) are extrapolations of integration point values. This frequently leads to a situation in which equilibrium for the submodel is not satisfied. To circumvent this, the user may perform a submodel analysis with displacement boundary conditions, store the forces at the boundaries in the frd-file and use this file as global model for a subsequent submodel analysis with force boundary conditions. In this way a correct force-driven analysis can be performed, for instance for crack propagation analyses in the submodel (displacement-driven analyses prevent the crack from growing).

First line:

• *SUBMODEL
• Enter the parameters TYPE and INPUT and their value, and, if necessary, the GLOBAL ELSET parameter.

Following line for TYPE=NODE:

• Node or node set to be assigned to this surface (maximum 16 entries per line).
Repeat this line if needed.

Following line for TYPE=SURFACE:

• Element face surface (maximum 1 entry per line).
Repeat this line if needed.

Example:

*SUBMODEL,TYPE=NODE,INPUT=global.frd
part,
1,
8


states that the present model is a submodel. The nodes with number 1, 8 and the nodes in the node set “part” belong to a Dirichlet part of the boundary, i.e. a part on which the displacements are 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: .