Modeling Pretensioned Bolts


	The information about pretensioned 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 prestress in the bolt must be taken into account in order to correctly capture the behavior under service loads. The Bolt Pretension functionality in COMSOL Multiphysics is designed to simplify such analyses. You can model the bolts either using solid or beam elements.

During mounting, a bolt is tightened to a certain prestress. 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.

Sometimes the sequence in which the bolts are tightened is important. This will be the case if significant nonlinearities are induced by the tightening process. Modeling such a process is also fairly straightforward. This is, however, a less common case which adds some extra complexity to the modeling, so it will be discussed separately below.

Modeling the Bolts

You must use a specific modeling technique in order to use a bolt in a prestress analysis.

Using Solid Elements

You can model bolts using solid elements in 3D or 2D axial symmetry. In 3D, it is usually most efficient to add the predefined bolt geometries from the Part Libraries. In 2D axial symmetry, the bolt is always assumed to be axially symmetric, and thus having the Z-axis as its center of rotation.

Make sure that there is at least one interior boundary perpendicular to the bolt axis somewhere in the shank. In the following, this boundary is referred to as the slit boundary (Figure 2-24). The slit boundary can be composed of several adjacent boundaries in the geometry.

If you are using bolts from the Part Libraries, a slit boundary is predefined, and has the selection name Pretension cut. In order to make this boundary selection visible from the physics interface, select its check box in the section of the settings for the part instance (Figure 2-25).

If needed, add contact conditions between the bolt head and the component and between different components clamped by the bolt. In many cases, it is sufficient and more efficient to use a continuity condition between the bolt head and the component.

Add a node, in which the pretension force or stress is prescribed for a set of bolts sharing the same data.

For each bolt having the same essential data, add a subnode where its slit boundary is selected.

The label of the bolt, which is an input in the section, is used to identify the bolts during result evaluation. A suggestion for the name is automatically generated, based on the base name given in the parent node.


	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 pretension force is interpreted as the force in the whole bolt, and not as the force in the half-present bolt. This makes it possible to use the same Bolt Pretension node for a set of similar bolts where some of them are located in symmetry planes.

Figure 2-24: Example of a bolted joint with the bolt modeled as a solid.

Figure 2-25: Getting access to the slit boundary selection for a bolt from the Part Libraries.

Using Beam Elements

When modeling with beam elements, you will typically use a with three points to model each bolt (Figure 2-26).

There must be at least one interior point somewhere in the shank. In the following, this point will, in analogy with the solid, be referred to as the slit boundary.

Since there is no explicit bolt head when you model a bolt using beams, you need to connect it to the solid component using some type of abstract coupling. There are several options:

You can connect the end of the beam to the edge of the bolt hole (the lower end in Figure 2-26). Then, use the Solid–Beam Connection multiphysics coupling, with set to . In this case, you select the edge of the bolt hole.

You can create a circular boundary having the diameter of the bolt head on the surface of the component (the upper end in Figure 2-26). Then, use the Solid–Beam Connection multiphysics coupling, with set to . In this case, you select the annular solid boundary.

Even without creating an extra boundary, you can use the Solid–Beam Connection multiphysics coupling, with set to . Then set to and enter half the head diameter as . In this case, you select the entire boundary on which the bolt head is residing. This method is convenient, but will often give more spurious stresses around the bolt hole, since partial element faces will be connected.

You can use the two first approaches, but rather than using a multiphysics coupling for the connection, you can add rigid connectors in both physics interfaces, and then connect them. This approach is more expensive, since it adds degrees of freedom in both the rigid connectors, plus the constraints to couple them. It is however an approach that may be suitable for imported meshes, where connection data in this form is available.

All these techniques are shown in the Structural Mechanics Module Application Library example Modeling of Pretensioned Bolts.

Add a node, in which the pretension force or stress is prescribed for a set of bolts with the same data.

For each bolt having the same essential data, add a subnode where its slit boundary is selected.

Figure 2-26: A bolt modeled using the Beam interface.

The Predeformation Degree of Freedom

Each bolt defined in the node has a single global 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. An optional relaxation r can also be included.

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.

It is only meaningful to introduce the relaxation in a later study step. If it is present all the time, then its only effect would be to increase the predeformation during the pretension analysis by r. Thus, the value of r is usually a function of the load history, which is initially zero.

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 prestress 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:

Run the study step for the mounting simulation. The predefined study type is designed for this. You may need to apply the pretension load in smaller steps, if there are nonlinearities in the system. Then, you select in the section in the settings for the study step. Introduce a load ramping parameter, which is used to multiply the pretension forces.

Add one or more studies or study steps to analyze the effects of the service loads.

Since the pretension degrees of freedom are not solved for in the service load study steps, they must obtain their values from the pretension study step. If the study steps are sequential within the same study, no special action is needed, since the default then is to inherit values from the previous study step. For other cases, go to the section of the study step, set to , and then select the pretension study step.

Sequential Tightening

If you need to take the order of the bolt tightening into account, then you must use an auxiliary sweep where the sweep parameter is used to control the tightening history.

You need to perform the following steps:

In each node representing a bolt that is not fully pretensioned from the beginning of the study step, select the check box.

A new text field, , is now shown. In this text field, you enter a Boolean expression, which evaluates to a nonzero value at the parameter values when the prestress is applied. It may happen more than once, if the bolt is not given its full pretension force at once. An example of such an expression is round(par)==3 || round(par)==11.

If you want the bolt prestress (when applied) to have a value that differs from the value given in the parent node, change the setting of from to another option. Extending the example above, the expression for the pretension force could be 50[kN]*if(par>3.5, 1, 0.6). The only thing that matters here is the value of the force at the parameter values when the pretension force is set, in this example 3 and 11.

A sequential tightening precess may have a quite slow convergence rate until a certain number of bolts have been loaded. The reason is that it is common that two mating boundaries barely touch, so that many contact iterations are needed. It is advisable to start by giving all bolts a small prestress, maybe 1% of the final value, in order to stabilize the model.


	It is important to make sure that you only solve for the bolt predeformation degrees of freedom in the pretension study step, and not when analyzing the service loads. If you use the Bolt Pretension study type for the pretension study step, and any other study type to analyze the service loads, the solvers are automatically set up to handle this. The Bolt Pretension 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 Pretension 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 2-15: Bolt Variables.
Variable	Description
d_pre	Predeformation
F_bolt	Axial force in the bolt
F_shear	Shear force in the bolt (3D only)

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.

When there are pretensioned bolts in a study, evaluation groups containing the bolt forces will automatically be generated.


	Studies and Solvers in the COMSOL Multiphysics Reference Manual

•

Modeling of Pretensioned Bolts: Application Library path

•

Prestressed Bolts in a Tube Connection: Application Library path