Hello Everybody!
I am currently writing my master thesis in which I am trying to understand the stiffness values of tapered roller bearing. For this, I am have made the model simpler by using only a single segment of the TRB in Abaqus CAE.
During the loading stage, I am able to apply radial loading and find out the radial stiffness of the TRB segment but however, on the application of an axial load, the simulation fails. I am unable to find the problem as to why. Please find attached a picture showing the boundary conditions and the loading definition. The outer ring is constrained on the top and a kinematic coupling is used to constrain the inner surface of the inner raceway with RP2 and a radial load is applied on the same Reference point(RP2).
The load is also constrained in this picture with respect to the global y-axis for radial loads.
I have also tried to do that same by constraining the load in all directions except for the axial direction but the simulation still fails.
The step is set such that NLGEOM is on and the values for time step are 0.01, 1E-015, 1 with a time period of 1.
I have tried many different ways to get axial loading to work but was unsuccessful. It would be of great help to me if any if you could give me some ideas regarding this. Please feel free to ask if you require any further information.
Thank you!
Hello Bhargav Vedartham ,
First of all, the positioning of your components in terms of the global coordinate frame. is not that clear. Maybe you should have considered adding the compass of Abaqus in the image to be able to understand the different directions you mention.
If I were to simulate this problem, I would start by defining a cylindrical coordinate frame at the geometric centre of the whole structure. By doing this you would have defined a radial direction that is always perpendicular to the outer surfaces of the rings. All of the steps discussed below are based on this definition.
After that, I would partition all the parts on the rz plane (the plane that would cut your components into two symmetric counterparts). On this plane I would define BCs that allow the displacement only along the radial direction. Furthermore, it would be better if you could assign symmetry BCs on the outer component surfaces that lie on screen in front and in the back. The upper surface of the outer ring has been constrained relatively well (some degrees of freedom maybe should allowed, like the circumferential movement).
The use of a reference point is wise, but it would be better to connect it with the underlying nodes through a continuum distributed coupling constrain. This way you would induce forces on the connected nodes in the direction you want, i.e., the radial one.
In your description you do not mention any contact interactions between the roller and the rings, but I am sure you understand that they are needed in order to have a well structured finite element problem. Hard contact and friction-less tangential behaviour could be used as an initial approach.
Regarding the selection of an initial increment and a maximum one you may also refer to my suggestion here:
https://www.researchgate.net/post/How_to_choose_an_Initial_time_increment_in_a_abaqus
Finally, I would strongly suggest that you turn NLGEOM OFF while you are building your model and you applying BCs and constrains. Once everything is in place and is tested that it is working well, then you may turn NLGEOM ON and take into account any geometric nonlinearities.
Hope that this information helps.
You need to first understand how does it happens in reality. In reality the outer ring is pushed axially to preload the bearing and that is what you need to do in the simulation as well.
- Badges
- Science topic
- Similar topics
- Psychology
- Emotion