Pre-tensioned Bolts
The information about pre-tensioned bolts is applicable if your license includes the Structural Mechanics Module.
Bolted joints are common in mechanical and civil engineering structures. If you are interested in analyzing the details of a bolted joint, the pre-stress in the bolt must be taken into account in order to correctly capture the behavior under service loads. The Bolt Pre-Tension functionality in COMSOL Multiphysics designed to simplify such analyses.
During mounting, a bolt is tightened to a certain pre-stress. The mounting of the bolt is, in general, accompanied by deformations of the surrounding structure. In the subsequent service, the force in the bolt can then change due to external loads.
Modeling the Bolts
You must use a specific modeling technique in order to use a bolt in a prestress analysis.
1
Model each bolt using solid elements in 3D. Usually it is most efficient to add the predefined bolt geometries from the Part Libraries.
2
Make sure that there is at least one internal boundary perpendicular to the bolt axis somewhere in the shank. In the following, this boundary is referred to as the slit boundary (Figure 2-17). The slit boundary can be composed of several boundaries in the geometry.
3
If you are using bolts from the Part Libraries, a slit boundary is predefined, and has the selection name Pre-tension cut. In order to make this boundary selection visible from the physics interface, select its Keep check box in the Boundary Selections section of the settings for the part instance (Figure 2-18).
4
If needed, add contact conditions between the bolt head and the component, and between different components clamped by the bolt.
5
Add a Bolt Pre-Tension node, in which the pre-tension force or stress is prescribed for a set of bolts with the same data.
6
For each bolt having the identical pre-tension stress, add a Bolt Selection subnode where the slit boundary is selected.
When a bolt is located in a symmetry plane (so that only half the bolt is modeled), and Automatic symmetry detection is selected in the Bolt Selection node, the given pre-tension force is interpreted as the force in the whole bolt, not as the force in the modeled half. This makes it possible to use the same Bolt Pre-Tension node for a set of similar bolts where some of them are located in symmetry planes.
Figure 2-17: Example of a bolted joint.
Figure 2-18: Getting access to the slit boundary selection for a bolt from the Part Libraries.
Each bolt defined in the Bolt Selection node has a single degree of freedom called predeformation, d. At the slit boundary, the two sides of the bolt are disconnected so that the displacements over it can be discontinuous. The discontinuity is represented by:
Here the subscript u denotes the upside of the slit boundary, and d denotes the downside. n is the normal pointing out from the downside. The sign has been selected so that d gets a positive value when the bolt force is tensile.
The axial force in the bolt is thus caused by a small overlap between the two sides of the slit boundary. It is computed as the reaction force belonging to the degree of freedom d.
Setting up the Study Steps
In an analysis of prestressed bolts, you have to use two or more separate study steps. They can be part of a single study, or be placed in different studies. The first study step, in which the bolt pre-stress is prescribed, simulates the mounting process. If you would only use a force to load the bolt, for example as an initial stress, the resulting stress in the bolt would be less than the intended, due to the compression of the material around the bolt. The prestress step ensures that the bolts have the intended prestress, irrespective of the flexibility of the surrounding structure and their interaction.
In the subsequent studies the bolt force is allowed to change, while keeping the extension of the bolt, as caused by the first study, fixed. The procedure to do this is as follows:
1
Run the study step for the mounting simulation. The predefined study type Bolt Pre-Tension is designed for this.
2
Add one or more studies or study steps to analyze the effects of the service loads.
3
Since the pre-tension degrees of freedom are not solved for in the service load study steps, they must obtain their values from the pre-tension study step. If the study steps are sequential within the same study, this action is not needed, since the default then is to inherit values from the previous study step. For other cases, go to the Values of Dependent Variables section of the study step, set Values of variables not solved for to User controlled, and then select the pre-tension study step.
 
It is important to make sure that you only solve for the bolt predeformation degrees of freedom in the pre-tension study step, and not when analyzing the service loads.
If you use the Bolt Pre-Tension study type for the pre-tension study step, and any other study type to analyze the service loads, the solvers are automatically set up to handle this. The Bolt Pre-Tension study type is actually a special case of a Stationary study step, with the sole purpose of activating the predeformation degrees of freedom. These degrees of freedom are by default not solved for in any other study type.
If you however set up your studies manually, the information below is useful. Also, in versions prior to 5.3, this automatic mechanism was not available, so in older models the studies were always set up manually.
You enable or disable the solution of individual degrees of freedom under the Dependent Variables node for a certain study step in the solver sequence. If required, begin by clicking Show Default Solver in the study node or in the Solver Configurations node of the study. Then move to the Dependent Variables node, and in the General section, set Defined by study step to User defined.
You can now go to the node for each predeformation degree of freedom below Dependent Variables and adjust the state of the Solve for this state check box.
For more information, see also Dependent Variables and Studies and Solvers in the COMSOL Multiphysics Reference Manual.
Results
The results in a bolt do not belong to any part of the geometry, but are global variables. To access the result from a certain bolt, a full scope of the type <interface>.<Bolt Pre-Tension tag>.<Bolt Selection tag>.<variable> must be used. An example could be solid.pblt1.sblt1.F_bolt. The bolt results are summarized in the table below.
Table 2-10: Bolt variables
Variable
Description
d_pre
Predeformation
F_bolt
Axial force in the bolt
F_shear
Shear force in the bolt
If you place a bolt in a symmetry plane, that only half of the bolt is modeled, this will automatically be detected. The results are reported for the whole bolt, not for the symmetric half.
Studies and Solvers in the COMSOL Multiphysics Reference Manual
Prestressed Bolts in a Tube Connection: Application Library path Structural_Mechanics_Module/Contact_and_Friction/tube_connection