In the previous section, we talked briefly about modeling a bolted joint and extracting useful results to guide the design process.
In this lesson, we will learn about the different methods of representing bolts in a finite element analysis.
Before we do that, let’s revisit the structure of a bolt and nut assembly.
The head is the flat portion of the bolt which transfers forces to the clamped plates.
The nut and the bolt engage with each other via threads that are cut into them.
Threads are helical groves cut in the shape of V or square, which is how forces are transferred between the bolt and the nut.
The nut holds the assembly and prevents slippage.
The portion of the bolt between the nut and the bolt head is the grip length.
The threadless portion of the bolt is called shank.
Bolts can be represented in two ways: as a solid body or as a line body.
Modeling the bolt as a solid body allows us to represent the threads, the bolt head area, the bolt diameter, etc.
We can also model non-linear contact behavior between the bolt and the nut.
But this method of representing bolts requires a large number of nodes, which increases the computational cost.
Bolts are usually designed such that the bolt fails before thread slippage occurs.
That is why modeling the threads is usually not required.
Further, we may have cases where we don’t need to account for frictional effects
or where the compression area on the flange need not be modeled very accurately.
In such cases, bolt modeling can be made computationally more efficient by using line bodies.
Line bodies require smaller number of nodes to discretize the bolt, and thus the solution time is reduced.
Using line bodies gives us a reduced stress state – in other words, we get 3 stress components instead of 6 –
but we can get fairly accurate results in bending and axial loading.
So line bodies may not be able to model every scenario accurately,
but for the cases that they can, using line bodies is much more computationally efficient.
First, let’s discuss modeling a bolt as a solid body.
The solid body may be discretized using 3D shapes such as tetrahedrons, prisms or cubes.
There are various solid elements like 8-noded hexahedron, 10-noded tetrahedron, 20-noded hexahedron etc.
Each node has 3 degrees of freedom.
So this means that a large number of equations need to be solved.
Due to this reason, solid models are computationally expensive.
Modeling bolts as solid bodies requires the least amount of preprocessing time
since Workbench Mechanical can automate meshing and contact detection.
When bolts are modeled as solid bodies, solid elements are used to mesh the bolt.
Solid elements have multiple integration points.
Stresses are calculated at each integration point and extrapolated to the nodes of the element.
A node is shared by multiple elements.
So averaged stress for the node is calculated based on the extrapolated stress values for that node in each element.
Due to this, solid models can capture local variations in stress and strain, such as seen in case of sharp corners, fillet radii, etc.
Thus, modeling bolts as solids is computationally expensive, but results in more accurate, detailed solutions.
Let’s look at an example in which the bolt is modeled as a solid body and meshed with solid elements in Workbench Mechanical.
If the length of the bolt is about 60 mm and it is meshed with hexahedral elements of size 3 mm, the total number of nodes is about 12600.
Since each node has 3 degrees of freedom, the bolt has 37800 degrees of freedom in total.
If a machine assembly has a large number of bolts, the total number of equations to be solved could become very large.
The system will require larger computer resources and longer computational time to calculate the solution.
Bolts should be modeled as solid bodies for the following cases.
One, if we need to calculate the local stresses in bolt heads, nuts etc.
Two, in order to model friction between bolt head and the clamped plates.
Or three, to model the stress distribution in the threaded portion when the bolt is loaded.
Other than these three cases and a few other special cases, we may use the computationally less expensive option of line bodies.
The second way of representing bolts is by using line bodies.
Bolts modeled as line bodies are represented using 1-dimensional 2 or 3-noded beam elements.
Each node has 3 translational and 3 rotational degrees of freedom.
Due to the low node count, the total number of degrees of freedom becomes less.
Thus, beam models can be solved faster and are computationally more efficient.
The bolt cross-section has four integration points where stresses are calculated.
These stresses are then extrapolated to the nodes.
But unlike solid elements, beam elements cannot calculate the averaged stresses at nodes.
One shortcoming of using line bodies to represent bolts is that we have a reduced state of stress
i.e. we can obtain only 3 stress components instead of 6.
While this is usually not an issue since a bolt is not compressed along the shaft, it is a point worth keeping in mind.
Line bodies require additional preprocessing effort, such as extracting the cross-section and connecting the line body to other parts.
Let’s come back to the bolt example we saw previously.
If we represent the same bolt as a line body and mesh it with beam elements of size 3 mm, the total number of nodes we get is 39.
With each node of the beam element having 6 degrees of freedom, the total degrees of freedom for the bolt is just 234.
Compare this with the 37800 degrees of freedom that we got when we represented the bolt as a solid body.
That is huge reduction in computational cost!
So bolts are represented as line bodies when we wish to reduce the solve time,
and when the stress or strain distribution in the bolts is not the primary interest.
When the role of the bolts is mainly for generating the preload,
and when we are only interested in the stress distribution on the clamped plates, we may consider modeling the bolts as line bodies.
To understand these modeling choices in practice, let’s look at a few simple cases here.
A bolt may be simplified by replacing its threaded portion with a cylinder, since we generally don’t need to model the threads.
In some simulations, the bolts are only required in order to generate preload.
In such cases, we can remove the bolt head, the nut, and the extra length of the bolt, and represent the bolt as a simple cylinder.
We can further simplify the bolt, by replacing the solid, cylindrical body with a line body.
Again, in such cases, bonded or MPC contact is used between the line body and the plate hole.
Now that we have looked at the different ways in which a bolt can be simplified, let’s see the actual finite element modeling in practice.
The first method is modeling the bolt as a solid body, with its threaded portion being replaced with a cylinder
and using solid elements to discretize the bolt.
Replacing the threaded portion with a cylinder reduces the node count.
Bonded contact is used between the nut and the bolt.
Since linear contact is used, solve time reduces.
In some cases, we may want to calculate stresses in the threaded portion of bolts.
But if we include the thread geometry, the number of nodes required to mesh the bolt increases tremendously.
So we want to find a way in which we can calculate the stress in the threaded portion, but not increase the number of nodes drastically.
The solution to this problem is to use geometry correction.
In this method, the threaded portion of the bolt and the nut is again replaced with a cylinder,
but instead of using bonded contact between the nut and the bolt, we use frictional contact with geometry correction.
When we use geometry correction between the bolt and the nut surfaces,
a correction is applied to the contact normal for these two surfaces based on user-inputs.
The user specifies the start and end points of the bolt axis, the mean pitch diameter of the bolt,
the pitch of the bolt, the half-thread angle and the number of starts.
Ansys Mechanical then calculates the contact normal behind-the-scenes.
Thus, this is a convenient way of getting approximate stress values in the threaded portion
without actually modeling the thread geometry and without increasing the number of nodes required to discretize the threads.
A third technique is representing the bolt as a line body and imprinting the bolt head area on the clamped plates.
A bonded or MPC contact is used between the line’s end point and the bolt head imprint.
This technique can approximately model the compression area on the clamped plates due to the bolt load.
As discussed earlier, using a line body to represent the bolt makes this method computationally efficient.
Instead of using the bolt head imprint, one can also use edges of the plate hole to connect with the line body.
Again, MPC or bonded contact can be used to connect end points of the line body to the plate hole edges.
The last technique is to create a beam connection without using any line geometry.
In the Contacts definition of Ansys Mechanical, there is an option to create beam connections,
where we can define the beam cross-section radius and material properties.
The beam is scoped to the selected entities such as plate hole edges, or the inner surface of the plate holes, using remote points.
This technique is more convenient as it doesn’t require creating line bodies, thus saving preprocessing time.