1. Why Screwed Connections Matter in Structural Simulation
Screw connections are among the most common joining techniques in all of engineering, be it mechanical, aerospace, or even the construction industry. Typical use cases include:
the robust load transfer between structural components,
detachable joints for maintenance and assembly,
preloaded connections to increase stiffness and fatigue resistance,
or the generation of contact pressure to ensure sealing.
Hence, due to their vast importance in engineering, it is essential to also understand the different failure modes that govern screws, for example, slip, separation, fatigue, bearing, and pullout. To be able to analyze an assembly for all of these risks, it is imperative to correctly model each screwed connection, accounting for the generated global stiffness, local stress concentrations, and the resulting load paths and force distributions.
Finite element analysis has established itself as highly relevant to industry due to its rich yield and information in all of these topics, making it standard practice in aerospace, automotive, and machinery industries. Additionally, such simulations have blended well into this ecosystem of design analyses, but not replacing, but rather augmenting standards such as the VDI 2230.
Many simulation environments succeed in accurately modeling screws. In the following, we are going to reference the widely used software packages ANSYS Mechanical and the Altair suite, including HyperMesh and OptiStruct. Below is an extensive summary of the different techniques available:
a. Bonded Contact Without Explicit Screws
The simplest and thus fastest approximation of a screwed connection is to omit the screw itself, but rather directly mate the contacted surfaces as fully bonded, i.e., no relative motion. Although very superficial, due to the fast evaluation time, it can have its benefits for surrogate modeling and early-stage design. Typical implementations are the bonded contact in Ansys Mechanical or the tight contact in HyperMesh/Optistruct. The advantages are thus the extremely low modeling effort. together with its numerical robustness and speed. There are multiple reasons for this. Firstly, not modeling a screw, of course, lowers the total element count. Secondly , since only bonded contacts are used, no non-linearity is introduced into the problem. These advantages can further be maximized by not even modeling the screw holes on either component. Further simplifying the meshing process, as well as the mesh itself.
However, of course, these simplifications also bear limitations. Three important ones are worth dissecting:
First, no bolt pre-load representation. Since no screw is modeled, it is also not possible to account for the clamping force resulting from a tightened screw. This preload can be highly relevant since it typically is of very high magnitude. A simple M6 screw can supply well over 1 ton of force already, M16 screws well over 10 tons
Second, the bonding of both components eliminates the observation of cleavage or slip, which can be, depending on the problem, catastrophic in consequences. An important example here is pressure containers, which are typically screwed together to supply enough force for the gasket to continue to seal.
Third, the bonding results in an unrealistic stiffness for most joints, since unlimited force transmission can happen even far away from the screw.
Typical use cases include:
Concept studies
Surrogate models
Global stiffness estimation
Non-critical joints
b. Rigid Element Connections (RBE2 / RBE3)
Rigid element connections allow simplified accounting of load transfer via rigid coupling, with negligible increase in problem size. This can be done by modeling the force transmission via rigid spiders instead of physical bolts. Typical implementations are RBE2/RBE3 elements in OptiStruct or remote points or rigid regions in ANSYS.
Similar to bonded contacts, their main advantage lies in their simplicity and stability. Setting up such connections is done quickly through the engineer and also allows for a fast calculation of the problem. In addition to this, in contrast to bonded contacts, they also allow for a clear force extraction of the simulated screw by inspecting the created reference node.
Albeit they are thus able to give a numerical value for the loads, they still exhibit artificially stiff behavior, potentially falsifying the prediction. This is evident when bearing in mind that the physical properties of the screw are still nowhere included in the model. Thus, joining two components with an M3 screw would yield the same results as an M20 screw. Additionally, it is still not possible to include preload or friction effects in this simulation.
That makes rigid element connections in FEA best suited for :
load path definition
early sizing of surrounding structures
and simple post-processing of reaction forces.
c. Beam-Based Bolt Models (1D Bolt Representation)
As mentioned, the above models did not allow for accounting for the specific properties of the bonded joint, such as bolt material, bolt size, and preload, but rather created idealized overstiffened connections. Beam elements as a surrogate for bolts are the simplest method of incorporating these factors, establishing them as the industry standard for many engineering problems.
1D bolt representations are created by modeling the screw shaft as beam elements and then connecting them to the surrounding structure via rigid or elastic elements. They can thus be seen as an extension of the RBE method by introducing a non-infinite stiffness between the connecting points. Typical implementations include OptiStruct’s CBAR and CBEAM, and the beam elements in ANSYS Mechanical.
They are beneficial because they support preload definitions as well as defining the stiffness of the screw shafts by accordingly tuning the stiffness of the beam element while still staying efficient for large assemblies, since they are only one-dimensional and thus scale well. This results in a good balance between accuracy and cost.
Still, they lack the ability to resolve these stresses in a three-dimensional manner. For example, the local thread stresses are not depicted, and depending on the chosen interfaces for the RBE elements at either side, it is also quite regular that the forces are not distributed correctly. Additionally, it is necessary to manually calibrate the stiffness of the one-dimensional element, making sure it is in accordance with the stiffness of the entire screw. This becomes especially tedious for bolts with shanks or fit screws due to their changing cross-section, not only increasing labour but also room for error.
Typical deployments are:
VDI 2230 correlation
Fatigue-relevant load extraction
System-level structural analysis
d. 3D Solid Bolts Without Explicit Threads
By increasing the complexity of solid bolts with a 3D mesh, the geometric realism is substantially increased. A standard simplification for this is to omit the threads themselves, treating the screw and the female thread as cylindrical bodies that can then be directly bonded together. The bolt head is also modeled in accordance with its real shape and implemented through a solid mesh. Here, the contact of the screw head to the joint component can be set to either bonded or frictional, depending on the problem requirements. Implementations or do for all software, solid meshing together with appropriate contact definitions. Under the hood, pretension is applied by axially sectioning the screw into two parts and applying a relative axial displacement at the created interface, essentially artificially enlarging the screw length and thus creating tensioning forces that represent the pretension. The solver then manually tunes the artificial displacement to match the user-specified pretension. Both Ansys and Altair provide appropriate tools to streamline this process.
The gains of this approach lie in the increased resolution of the connection. 3D stresses, such as the notching effect between the screw head and the screw shaft, or the specific shape of the screw head, can be calculated, providing increased realism for the stresses inside the screw. Likewise, this also offers superior contact pressure predictions, since the screw stiffness is modeled three-dimensionally. The drawbacks of this approach mainly reduce the increased mesh effort, which takes longer to achieve for the simulation engineer, as well as increasing solving times, potentially also making the problem less robust. Additionally, the approach still has its limitations when it comes to the analysis of the thread behavior itself, as it is still idealized as a bonded cylindrical contact rather than depicting each thread individually. ANSYS offers a Bolt Thread Geometry Correction that promises the approximation of the thread stresses. However, this comes at the cost of having to set the element size to below a fourth of the pitch size, making the mesh size typically too small for practical evaluation.
Use cases are:
Local stress evaluation
Verification models
Research and validation studies
e. Fully Modeled Threads
(High-Fidelity Bolt Modeling)
Finally, maximum realism can be targeted by significantly increasing computational cost through high-fidelity modeling of the threads themselves. Such an explicit helical thread geometry for both the male thread of the screw and the female thread of the engaging component can then be mated together through frictional contacts. Here lie multiple implementation challenges. Firstly, creating an appropriate mesh is very difficult due to the extremely fine mesh size. It is not essential to set the mesh size to the pitch, but rather it must be significantly smaller, to also be able to account for the created stresses in every crease of the pitches. Even if meshing is achieved, this typically results in significant convergence issues due to the complex contact behavior. Nevertheless, it is the only way to accurately simulate thread stresses, which can be necessary if the governing failure mode is expected to be induced inside the threaded region. However, by following engineering standards such as the VDI 2230, it can be ensured that breakage occurs outside the engaged thread, thus circumventing any need to deploy such complex models in typical engineering problems.
Thus, their disadvantages in extremely high computational effort and infeasibility for full assemblies limit the typical usage to academic studies or model calibration and validation.