A simple tutorial on how to use bolt pretension to clamp two parts together before applying a force to pull them apart. The attached file is an ANSYS 18.2 archive.
Here is a followup video showing how to do a beam connection. This takes a little less effort than the solid fastener shown above. The attached file is from ANSYS 2019 R3.
Here is a third model in the series that shows using midsurface bodies and shell elements to do the same thing as above on a slightly more complicated joint. Thanks to Aren for the geometry.
How can I apply bolt pretension to clamp two parts together in ANSYS V16.0 (I´m using beam element to emulate a 3D bolt).
Thank for you time.
I don't recall what ANSYS V16 looks like. Is Bolt Pretension listed in the Loads in Workbench? Please insert a screen snapshot of the available loads.
here you are, I have the option to insert BOLT PRETENSION in static structural but it does not display nothing on named selection.
Dear peteroznewman,here you are, these are the load available on ansysV16; I have been investigated how can i put this pretesnion on beam elements and the answer was using APDL comands but i haven´t found wich of them I must use.thanks for you answer.
Insert a Bolt Pretension, then pick a line body that is meshed with beam elements. What is stopping you from doing that?
The only requirement is that the line body must have a minimum of 2 elements along the length. If there is only 1 element, it will fail.
Hi Peter, maybe one day you will have time to look at this question,
I have tried to run the model for your first analysis, it is ok, except for the von mises equivalent stress, which is higher than in you video, what do you think can be the reason for it? Thank you in advance!
The reason for the difference in the initial result is that we were using different versions of software and the meshing parameters changed slightly to give a different mesh.
I got 469 MPa in the bolt, you got 545 MPa, but that was just an initial mesh. If you and I both did a mesh refinement study in the different versions of software, we might get closer to the same number, or discover that this model contains a stress singularity where the bonded contact holds the threaded end of the fastener in the hole.
Hi Peter, I have tried this one as well, I can not succeed with having the bolt head connection equal to 12 mm.
please see foto, do you know what can be an issue?
Hi Peter, could you please tell if you have used ACP? Could you please tell me if the same can be applied to ACP PRE? Could you please tell if the difference in results can be because of the versions of the program. Thank you
No, I have not used ACP. I expect bolt pretension can be used in ACP Pre but I have never used that myself.
It looks like you did not specify a Pinball Radius of 6 mm for the Beam connection.
Hi Peter, I have tired with pinball radius, it doesn't work. Could you please tell maybe I must choose a surface not an edge. Please see screenshots, I have tried several times and sorry to disturb.thank you
Hi, this issue was solved, I just needed to turn around the surfaces on which I applied connections for the beam. Thank you
Hi Peter, thank you again for help. The issue below was solved with pin ball radius, however, I got lower values of the equivalent von misses stress. Can you please comment on why it happened when you have time. Thank you
Different versions of software make different meshes which can cause different maximum stress values.
The point of the tutorial was to learn how to do this. Performing a Mesh convergence study is a separate activity.
A beam connection of a bolted preloaded joint is an efficient way to accurately transfer loads between flanges. It is adequate for models where the peak stress and area of concern is elsewhere in the model. If the peak stress is at the bolted joint, and that is an area of concern, then you should not be using an idealized representation, you should change over to a full solid fastener as shown in the first video.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.