Keyword type: model definition
This option is used to define a pre-tension in a bolt or similar structure. There are three parameters: SURFACE, ELEMENT and NODE. The parameter NODE is required as well as one of the parameters SURFACE and ELEMENT. The latter two parameters are mutually exclusive.
With the parameter SURFACE an element face surface can be defined on which the pre-tension acts. This is usually a cross section of the bolt. This option is used for volumetric elements. Alternatively, the bolt can be modeled with just one linear beam element (type B31). In that case the parameter ELEMENT is required pointing to the number of the beam element.
The parameter NODE is used to define a reference node. This node should not be used elsewhere in the model. In particular, it should not belong to any element. The coordinates of this node are immaterial. The first degree of freedom of this node is used to define a pre-tension force with *CLOAD or a differential displacement with *BOUNDARY. The force and the displacements are applied in the direction of a vector, which is the normal to the surface if the SURFACE parameter is used and the axis of the beam element if the ELEMENT parameter is used. This vector can be defined underneath the *PRE-TENSION SECTION keyword. If the vector is specified away from the elements whose faces belong to the surface (volumetric case) or in the direction going from node 1 to node 2 in the element definition (for the beam element), a positive force or positive displacements correspond to tension in the underlying structure. If no such vector is defined by the user, it is calculated automatically as the mean of the normals away from the elements whose faces belong to the surface (volumetric case) or as the vector extending from node 1 to node 2 (beam case).
Notice that in the volumetric case the surface must be defined by element faces, it cannot be defined by nodes. Furthermore, the user should make sure that
Internally, the nodes belonging to the element face surface are copied and a linear multiple point constraint is generated between the nodes expressing that the mean force is the force specified by the user (or similarly, the mean differential displacement is the one specified by the user). Therefore, if the user visualizes the results with CalculiX GraphiX, a gap will be noticed at the location of the pre-tension section.
For beam elements a linear multiple point constraint is created between the nodes belonging to the beam element. The beam element itself is deleted,i.e. it will not show up in the frd-file. Therefore, no other boundary conditions or loads can be applied to such elements. Their only reason of existence is to create an easy means in which the user can define a pretension. To this end the nodes of the beam element (e.g. representing a bolt) should be connected by linear equations or a *DISTRIBUTING COUPLING card to nodes of the structures to be held together.
Following line (optional):
Example: *PRE-TENSION SECTION,SURFACE=SURF1,NODE=234 1.,0.,0.
defines a pre-tension section consisting of the surface with the name SURF1 and reference node 234. The normal on the surface is defined as the positive global x-direction.
Example files: pret1, pret2, pret3.