What is in this Article?

1. Introduction

2. Why is Bolt Preload Necessary

3. What is Pretension Load in Simulation

4. Pretension Load in Akselos 

5. How to create bolt with Pretension Load

Want to know more about related Articles

1. Introduction

This section introduces a brief instruction of creating a bolt component with the ability to activate pretension load on it. The pretension load is included to consider the effect of the tightening force on the bolt, the nut, and the object is tightened between them.

Pretension Load is a part of Modeling steps in Akselos Workflow to build any simulation model.

Terminologies

2. Why is Bolt Preload Necessary

Bolt preload ensures that the mating parts stay connected during the operation of the machine. Insufficient bolt preload may cause the bolts to become loose, leading to failure of the machine assembly or separation and lateral movement of the mating parts. Since tightening of bolts produces tensile loads in the bolt, the bolt preload is also known as bolt pretension.

Figure 2.1. Pre-Processing stage

The structure of bolt and nut Assembly will include:

• The bolt head is the flat portion of the bolt which transfers forces to the clamped plates.
• The nut and the bolt engage via threads which are cut into them. The nut holds the assembly and prevents slippage.
• Threads are helical groves cut in the shape of V or square. This is where the nut and bolt transfer forces between them.
• The portion of the bolt between the nut and the bolt head is the grip length. ‐ The threadless portion of the bolt is called the shank.
• Some simulation requires modeling the bolt with all details to study the effects of bolt head area, bolt diameter, thread pitch and angle, etc.
• Not all simulations require these details, as bolts are standardized components in many mechanical applications.

• Some simulations can be run with a simplified representation of the bolt as a line body.

Figure 2.2. Bolt part

3. What is Pretension Load in Simulation

Defining Bolt Preload in Finite Element Simulations:

• In the real world, bolts are tightened by applying torque.
• In real-life, tightening a bolt reduces its grip-length and produces tensile preload.
• Applying torque and rotating the nut in a simulation is computationally expensive and does not add any value or accuracy to the results.
• Instead, the shortening of the grip-length (which induces tensile preload) is mimicked in simulations by slicing the bolt into two parts and applying preload to both ends.
• The finite element mesh overlaps in the cut region, but it is a convenient way of representing shortening of grip length.
• Assuming that the bolt is represented by a cylinder, the cylinder is split into two halves.
• Two nodes are picked on each half, say nodes I and J. The two nodes are generally, physically coincident.
• Constraint equations are created to tie together the relative motion of nodes I and J.
• By specifying the relative displacement between nodes I and J, or by specifying the force applied on the preload force acting between nodes I and J, we introduce a tensile load in the two halves of the cylinder.
• Similar procedure can be used to split a line into two halves.
• In real-life, a machine is first assembled, and then operational loads are applied on the machine. Simulations mimic real-life scenarios.
• Two important steps to define bolt preload in simulations: load and lock.
  1. Load: Specify the tensile force developed in the bolt during its tightening.
  2. Lock: Simulates complete tightening of the bolt before applying any external loads on the assembly

Figure 3.1. Bolt pretension section

4. Pretension Load in Akselos 

Pretension is used to model the tightening and loading of fasteners (e.g. bolts) in a structure. The pretension load acts to apply the constraint in the axial direction that comes from the tightening of the fastener. It is often used in combination with nonlinear contact to model a bolted joint and precisely evaluate the stresses in the bolt shaft.

Pretension loads are applied on pre-defined cross-sections of a fastener. This means that the bolt representation (which can use either solid or beam elements) should be split into two pieces in order to have these cross-sectional surfaces/nodes.

Figure 4.1. 3D bolts and 1D bolts

Before using Pretension Load:

The Pretension belongs to both Source Operator and Constraint Operator.

Note that if both pretension_force and pretension_displacement values are defined, one of the following occurs:

1. if one of the two values is 0.0, that value is ignored.
2. if both values are 0.0, the zero pretension_displacement is applied.
3. if neither value is 0.0, an error is thrown.

Figure 4.2. Pretention Load properties

4.1. Force-Based Pretension

A force is applied to the cross-sectional areas of the bolt, defined by the pretension_force field. Although the force is related to the tightening torque, this force must only include the axial component. This requires a “unlocked/locked” step (using the locking parameter) procedure as follows:

1. “tightening” of the bolt is simulated:
   • During an “unlocked” step, the user-defined pretension force is applied.
   • No other non-pretension forces are applied to the structure.
   • The displacement of the cross-sectional surfaces is calculated.
2. the pretensioned structure is loaded normally.
   • A “locked” step is performed, the bolt is now simulated as a single solid piece.
   • The displacement calculated in the first step is applied to the cross-sectional surfaces.
   • All other forces and boundary conditions are applied to the structure as normal.

The unlocked/locked steps are an important part of the procedure when using force-based pretension; if not used correctly this can lead to incorrect results. Displacement-based pretension does not require an unlocked step, but you must know (or calculate) the axial displacement beforehand.

When using force-based pretension, you can optionally print the axial displacements using the print_axial_displacements flag so that in the future you can switch to a displacement-based pretension as described in Displacement-Based Pretension below. The displacement values are written to the “log.processor.0” log file at the beginning of every “locked” step.

Figure 4.1.1. Example of the effect of “locking” on the deformation of a bolt, in an extreme case. The gap between halves is created for visualization purposes; normally the two halves of the bolt are coincident

4.2. Displacement-Based Pretension

Instead of applying a force to the cross-sectional surfaces as described in Force-Based Pretension, a displacement is applied directly, defined by the pretension_displacement field.

This has the advantage of not needing an “unlocked” step, since the goal of the unlocked step is to convert the pretension force to a displacement. For this reason, regardless of the value of the locked parameter all steps are treated as “locked.”

This disadvantage of displacement-based pretension is needing to know beforehand the displacement of the surfaces generated by the tightening. You can calculate this by running the simulation once using a force-based pretension approach and printing the displacements the print_axial_displacements option.

4.3. Other Properties

    Pretension Direction

The pretension direction can be automatically calculated from the normal of the master surface (if using solid elements) or from the axis of the master beam (if using beam elements). This is the recommended approach in most cases.

If you have an abnormal/non-flat cross-sectional surface, you can also manually define the pretension direction using the pretension_direction property.

    Unlocked Step

The following constraints are applied in the initial coordinate system:

Master Surface/Node

This means that the bolt cross-section can expand or contract, but it must remain perpendicular to the pretension direction. This constraint is necessary to avoid “cupped” cross-sectional surfaces that could occur if there was, for example, a pressure applied directly to the surface, which would give incorrect stress results inside the bolt.

Slave Surface/Node

• A “slave control node” is defined on the slave surface and is constrained in the lateral (non-pretension) direction to the “master control node.” This ensures that the axis of the bolt remains parallel. But the pretension direction remains unconstrained, so that the two halves of the bolt can separate or overlap to simulate “tightening.”
• The remaining nodes on the slave surface are constrained as follows:
  1. In the lateral directions to their closest nodes on the master surface, to ensure both halves of the bolt cross-section deform identically.
  2. In the pretension direction to the “slave control node,” to ensure that the two cross-section surfaces remain parallel.
• If using beam elements, the rotational degrees of freedom on the slave node are also constrained to equal those of the master node.

    Locked Step

These are also the constraints applied for displacement-based pretension, regardless of the value of the user-defined locked parameter.

• Each slave node is constrained to its respective master node in all directions. In the pretension direction, the offset from the unlocked step (or given directly by the user) is maintained.
• If using beam elements, the rotational degrees of freedom on the slave node are also constrained to equal those of the master node.
• No other constraints.

This allows for some rotation of the cross-section surface, but the pretension displacement/offset is always applied in the initial direction.

5. How to create bolt with Pretension Load

The referent steps are listed as below.

  STEP 1: Componentization

A 3D CAD model should be made including the bolt and the nut. The bolt-nut model is then divided into two components at the middle of the bolt. However, we will keep the two components at their original position and export both of them into a single CAD file that will be used later in the meshing software.

Figure 5.1. 3D bolt in cad

    STEP 2: Mesh Settings

Mesh the two components and assign each component to a separate block. The two components need to be unmerged at the cutting plane after meshing. The two inner surfaces of the bolt and the nut are assigned to sideset IDs 100 and 101. That means there are face ports that will be connected to the face ports of the object tightened between the nut and the bolt.

Figure 5.2. Mesh and Sideset 

    STEP 3: Import Component

Now you can import the 3D bolt component into your current collection:

Collections ribbon → Create -> Component Type → In the New Component Types, click Add Meshes → choose the mesh file that was exported in the previous step → click the Create button.

Figure 5.3. Import mesh component

    STEP 4: Create stored selection

Right click on the Stored Selection → Select Add Boundary Sets Selection → Select to surface of Pretension load.

Figure 5.4. Create Stored Selection

    STEP 5: Create Load Case and Add Pretention Load

Right click on Load Case → Add Load Case → Right click on the Load Case 1, select Add Load…

Figure 5.5. Add Load

Select the Pretension →  click Add button

Figure 5.6. Add Pretension Load

    STEP 6: Define properties of the Pretension Load in the Properties Tree

Figure 5.7. Set Load properties

Want to know more about related Articles:

• Create Load Case & Load
• Stored Selections