Bolt Pre-tension Techniques in Abaqus

In the realm of finite element analysis (FEA), understanding bolted connections is crucial for structural integrity. Our blog post, “Bolt Pre-tension Techniques in ABAQUS,” delves into this critical aspect, aiming to equip engineers and analysts with essential skills. From theoretical foundations to advanced techniques, the post offers a comprehensive guide for both seasoned analysts and newcomers, promising insights to elevate FEA expertise. Join us in tightening your virtual bolts and exploring the tension shaping robust engineering simulations.

The image below, extract from Abaqus Analysis User’s Guide, is a simple example that illustrates the concept of an assembly load (bolt pre-tension).

Container A is sealed by pre-tensioning the bolts that hold the lid, which places the gasket under pressure. This pre-tensioning is simulated in Abaqus/Standard by adding a “cutting surface,” or pre-tension section, in the bolt, and subjecting it to a tensile load. By modifying the elements on one side of the surface, Abaqus/Standard can automatically adjust the length of the bolt at the pre-tension section to achieve the prescribed amount of pre-tension. In later steps further length changes can be prevented so that the bolt acts as a standard, deformable component responding to other loadings on the assembly.

First Technique: Pre-tension Section

When it comes to applying bolt pre-tension in Abaqus/Standard, the conventional method—though not my personal preference—is often the go-to. This technique involves applying bolt pre-tension across a user-defined pre-tension section. The load is actually applied in a pre-tension node associated with that specific section.

Abaqus/Standard offers flexibility in applying bolt pre-tension loads, accommodating fasteners modeled by continuum, truss, or beam elements. For the purpose of this discussion, we’ll delve into continuum elements, as they are the predominant choice in 99% of cases.

Pre-tension section

For continuum elements, the pre-tension section is defined as a surface inside the fastener that “cuts” it into two parts.

This section is defined by the surfaces of the elements, specifically from one side of the designated section. It’s important to note that these elements, known as underlying elements, play a crucial role in the pre-tension application. As a best practice, aligning the element’s surfaces perpendicular to the axis of the bolt is highly recommended.

Controlling pre-tension node

The assembly load is transmitted across the pre-tension section by means of the pre-tension node. The pre-tension node should not be attached to any element in the model. The coordinates of this node are not important.

Notice that there’s a local coordinate system automatically created at the pre-tension node with the X (1) axis defined in the direction normal to the pre-tension section.

The pre-tension section has only one degree of freedom (degree of freedom 1, or X), which represents the relative displacement at the two sides of the cut in the direction of the normal.

Abaqus/Standard computes an average normal to the section—in the positive surface direction, facing away from the continuum elements used to generate the surface (Underlying Elements)—to determine the direction along which the pre-tension is applied.

Applying the pre-tension load

The pre-tension load is transmitted across the pre-tension section by means of the pre-tension node.

You can apply a concentrated load to the pre-tension node. This load is the self-equilibrating force carried across the pre-tension section, acting in the direction of the normal on the part of the fastener underlying the pre-tension section (the part that contains the underlying elements that were used in the definition of the pre-tension section).

Animation of boat-pretension

The animation below helps us uderstand how the bolt pretension works.

Notice that the bolt’s length is decreased by modifying the elements on one side of the pre-tension section (the underlying elements side).

Abaqus/Standard automatically adjusts the length of the component at the pre-tension section to achieve the prescribed amount of pre-tension. This adjustment is done by moving the nodes of the underlying elements that lie on the pre-tension section relative to the same nodes when they appear in the other elements connected to the pre-tension section. As a result, the underlying elements will appear shrunk, even though they carry tensile stresses when a pre-tension is applied.

Controlling the pre-tension node during the analysis

You can maintain the initial adjustment of the pre-tension section by using a boundary condition fixing the degrees of freedom at their current values at the start of the step once an initial pre-tension is applied in the fastener; this technique enables the load across the pre-tension section to change according to the externally applied loads to maintain equilibrium. If the initial adjustment of a section is not maintained, the force in the fastener will remain constant.

Example

The image below shows one common example of bolt pre-tension application: a bracket, bolt, and spacer assembly.

This assembly method is commonly used in the front suspension of vehicles. For instance, the upper and lower control arm connect to the vehicle frame using this mechanism, as shown below highlighted by the red circles.

Second Technique: Translator Connector

This is the technique I usually use in my projects. Instead of setting up a pre-tension section, we use a translator connector to link the nut and bolt. Afterward, we apply a connector load to move the nut and achieve the desired bolt pre-tension.

Let’s walk through the steps to set up our previous model using this method.

Create nut coupling

The initial step is to establish a coupling (typically kinematic) that includes all nodes from the internal nut surface, as illustrated below.

Create bolt coupling

Additionally, we need to form another coupling that includes the nodes on the outer surface of a segment of the bolt, particularly in the area where the nut contacts the bolt.

Adjust coupling’s reference node position

Once you’ve created the couplings, make sure to line up the coupling’s reference points. They should sit on the bolt axis and be a bit apart, about 2 mm.

Also, arrange the reference points so that increasing the distance between them in the axial direction will shift the nut closer to the bolt head. If this sounds confusing, no need to stress. Check out the video linked in this blog post for a clear walkthrough of this idea.

Create Translator Connector

Now, proceed to establish a translator connector connecting those two reference nodes.

Once you create this connector, a local coordinate system is automatically set up. The X-axis aligns with the direction determined by a line connecting the two reference nodes. The origin is positioned at the first selected node, and the X-axis extends from the first to the second selected node.

**IMPORTANT NOTE: If you choose to manually create the connector coordinate system, note that if the X-axis is directed towards the opposite side (from the second to the first node), the rule outlined below for positive and negative force will be reversed. In this scenario, a positive load will induce tension, while a negative load will result in compression.

Keep in mind (or learn now if it’s new to you) that the translator connector has just one degree of freedom, namely, the local X-axis mentioned earlier. This implies that the two reference nodes can only move in that specific direction. Consequently, all other translational and rotational degrees of freedom are locked in place.

Given this, there’s no requirement to simulate contact between the nut and bolt. Tie contact between nut and bolt, as we did previously for the pre-tension section technique, is prohibited because doing so would restrict the relative movements between the nut and bolt.

Apply connector load

For the final step, apply the connector load. Here’s a key point to keep in mind: a positive connector load pulls the nodes apart, creating tension. On the flip side, a negative load compresses the nodes, pulling them closer.

In our model assembly, apply a positive connector load. This action will move the nodes away from each other, causing the nut to travel towards the bolt head. You can see this demonstrated in the animation below.

You can maintain the initial adjustment of the coupling’s reference nodes by using a boundary condition (*CONNECTOR MOTION) fixing the degree of freedom 1 (X) at its current value at the start of the next step once an initial pre-tension is applied in the fastener.

Conclusion

In this exploration of bolt pre-tension techniques within ABAQUS, we’ve journeyed through the conventional method of utilizing a pre-tension section and delved into an alternative approach employing a Translator Connector. Each method has its merits, catering to different preferences and project requirements.

The first technique, employing a pre-tension section, offers a systematic way to simulate bolt pre-tension. By defining a cutting surface and utilizing a pre-tension node, engineers can precisely control the pre-tension load. The process is elucidated with a clear example, showcasing its application in a common assembly scenario.

On the other hand, the second technique introduces a Translator Connector, providing a nuanced alternative. This method simplifies the process by linking the nut and bolt directly and applying a connector load to achieve pre-tension. The step-by-step guide ensures clarity, making it an attractive option for those who prefer a different approach.

Ultimately, the choice between these techniques depends on the specific demands of the project and the preferences of the analyst. As we conclude our exploration of bolt pre-tension in ABAQUS, it’s evident that a thorough understanding of both techniques equips engineers with a versatile toolkit for ensuring structural integrity and accuracy in finite element analysis. Whether you opt for the traditional pre-tension section or the innovative Translator Connector, the goal remains the same: tightening the virtual bolts to enhance the reliability of your engineering simulations.

Learn More

If you’re new to the finite element method and eager to demystify its complexities, I highly recommend exploring my comprehensive blog post on the subject: Finite Element Analysis (FEA) Demystified.

Additionally, for a deeper understanding and further insights, I encourage you to consult the Abaqus User’s Guide. This invaluable resource provides detailed information complementing the concepts discussed in my blog post. You can access the Abaqus User’s Guide at the following link: Abaqus User’s Guide.

By combining the foundational knowledge from my blog post with the practical guidance offered in the Abaqus User’s Guide, you’ll be well-equipped to embark on your journey into the fascinating world of finite element analysis. Happy learning!