I’m trying to run detailed FEA on the thread fillets of a bolt, including both standard cylindrical threads and tapered threads (PAC-type). I was able to build the full 3D CAD model and generate a mesh, but when I run the simulation the results look unusual.
For the boundary conditions, I fixed the nut and defined contact between the mating thread surfaces. Then I created a rigid body constraint on the bolt head and applied a torque through a reference point.
As you can see in the attached image (as a new user i can only upload 1), I obtain very localized stress concentrations that appear as “point-like” spikes, in locations that do not seem physically justified. Could you help me identify what might be causing this? Could it be a CAD issue, meshing issue, or something related to how the contact/torque is applied?
Note: I’m not using the “bolt pretension/preload” tool because I’m not working with a simplified bolt model; I’m looking to model the threads explicitly.
I would start from a simplified axisymmetric model or at least a small portion of the thread. To get reasonable results, you will need a really good, locally refined mesh (always recommended to use quad/hex elements whenever possible in order to obtain better contact pressure distribution):
Thanks for your reply! Yeah, I read the post you mentioned, and while it was helpful, I decided to make this post since it didn’t mention explicitly modeled threads. I’m going to read the paper you referenced and run another simulation. I’ve never worked with axisymmetric models before, so I’ve been looking into that as well.
Standard axisymmetry won’t let you apply torque to the model, but it can be a good starting point to understand various aspects of thread contact modeling.
The key aspect to improve your model is to refine the mesh on the thread making it much denser. It will increase the solving time significantly, but is necessary to obtain good results. Hex mesh would be more computationally efficient, but it’s not easy to generate it in such a case (you would likely need to import the thread as a separate part and use the sweep technique to mesh it).
I get what you mean about the torque. However, I found some references that would let me convert the torque into an axial force using analytical relationships. I’m currently running a simulation similar to the first paper you shared, with a much denser mesh. Then, based on your YouTube video about chains, I was planning to build a model that I can later expand to the full bolt. Thanks for replying, and thanks for the references!
Indeed there are such formulas and if you don’t necessarily have to rotate the bolt, I would go with the axisymmetric model which is not only much faster to solve, but also much easier to mesh (remember to use quad elements). In fact, when threads are modeled (usually, they aren’t), the axisymmetric approach is probably the most common one.
It’s not a requirement that it rotates; the main goal is to be able to see the stress distribution. Once I achieve that and understand it, in the future I’d like to look into rotation as well. Thanks for all your replies and help.
The torque/angle approach may not be required to study threads. Once you’ve done your axi model understanding, and you know your axial bolt force load, you could cut your 3D bolt and apply that force to let the thread do its work, without the top (head side). This will avoid large finite sliding on contacts due to the twist. The net forces on threads will still be correct.
In case it helps, once you have a preliminary ‘true’ thread mesh that works, even if you get that patchy stress distribution (very common at the start), don’t forget the super-powerful sub-modelling technique. You drive a very fine local mesh off a global 1st model with contacts and the stiffness right; i.e. the load paths are correct; but stress contours are not.
Then you can daisy-chain sub-models zooming in, in stages, into the thread areas that matter. Here is is a sample slide on how I used to do that in my Abaqus times. This workflow was validated via prototyping at the time for a motorcycle company. All the way to fatigue prediction. Use sub-modelling in a creative way, it is super-powerful and fast to solve.
This was a while ago, should be faster/better nowadays. Food for thought…
I remember, there were a couple of white papers from Klaus Jürgen Bathe regarding Bolts in FEA with Adina. But since the software is now part of Bentley, I could only find this.
Speaking about Abaqus, during last year’s Regional User Meeting organized by Dassault Systèmes in Bamberg, Germany, there was a really great presentation from Raimer Ohlms with a summary of bolt modeling approaches in this software. Later, they also shared it on the SIMULIA Community (official user forum for Abaqus), but you will need a free 3DPassport account to access it.
Abaqus even has a way to account for the presence of a thread in contact without modeling it explicitly (this feature simply adjusts contact normal directions to be normal to faces of reference threads).
I want to thank everyone who kindly replied to this post, especially FEAnalyst. After reviewing your suggestions and the referenced papers, I was able to successfully build a 2D axisymmetric model with an explicit thread. Thank you!
