Static simulation of thrust bearing

[Anonymous]

I am trying to perform a static stress simulation on a model of an axial thrust "ball" bearing.

I can simulate this apparently successfully BUT only if I define the contacts between the balls and the surface of the races as "sliding" contacts. This will correctly simulate BUT only if the load is applied in the axis of the bearing. If I apply the structural load at a small angle relative to the axis of the bearing (10 degrees) then the results are incorrect. As would be expected the load is no longer evenly applied to the balls, those on the loaded side of the bearing are subject to increased contact pressures, stress and deformation, BUT those on the unloaded side, because  a sliding contact does not allow the bodies to separate, are subject to a "negative load" ie. the balls are stretched ( with corresponding surface pressure stress and deformation) . So it would seem obvious that to simulate this correctly the contacts should be defined as "separation" , however if I change these contact conditions to separation, the simulation fails with an error:

Error: STIFFNESS MATRIX SINGULAR OR NON-POSITIVE DEFINITE
Cause : A singularity or non-positive definite has been detected in the stiffness matrix during the
preconditioning phase of the iterative solver.
Action : Investigate the model for a lack of constraint. If using shell elements, either set the
K6ROT model parameter to a value between 1.0 and 100.0, or set the SHELLRNODE model
parameter to ON. Also, check for elements with bending stiffness (line and shell
elements) improperly connected to elements without (solids). If you are unable to
locate the source of the singularity, consider using the sparse direct solver.
Error: Solver Error
Error: An error occurred while solving the model.

I have no idea what this means.

Altering or applying additional constraints (which in themselves would prevent proper modelling) does not alter the error message generated.

Does anyone know how to simulate an axial thrust bearing when subjected to a (slightly) non axial load?

Thanks

Andrew Sansome

[John_Holtz]

Hi Andrew,

The error message is indicating (in its own mathematical way ) that some parts of the model are under-constrained, and so they are free to float off into space.

The problem with separation contact models is that until the software knows what the displacements are, it does not know what points are in contact. And without knowing which points are in contact, it cannot calculate the displacements. It usually assumes that all points are in contact at the beginning, calculates the displacements, and then begins correcting which points are in contact and which ones are not. During that iterative process one of the parts can become "free to float off", and the solver cannot recover from that condition.

Something like a ball bearing is particularly difficult because the contact between the ball and race is theoretically a single point. If a node is not close to the point of contact, the contact may be missed.

There is an option "Remove rigid body modes" that you can try. ("Manage > Settings > General > Remove rigid body modes".) This option tries to stabilize the parts that are not held properly by constraints. Note that there are some specific requirements for the model in order to use this option. I suggest you click the "Learn More" link next to the command to make sure you set up the model to fit the requirements.

Also, be sure to set the separation contact "Penetration Type" to "Symmetric" for all of the contact pairs. This will increase the likelihood that contact will be detected between the parts.

If the model still does not converge, feel free to export the model to an archive file (*.f3d) and attach it to your post. Someone will take a look at it.

[Anonymous]

Thank you, I'll give that a try in the first instance.

Andrew

[Anonymous]

Sir

I have followed your instructions (having read the notes on removing rigid body modes) but without success.

I have followed the guidance, one component constrained, but have applied balanced loads to the model. "Remove rigid body modes" is checked but still no  success.

Whilst I have learnt a great deal over the past ten days from the Autodesk tutorials and support community, I am still clearly missing something important. I would be very grateful if you would have a look and point me in the right direction.

I have attached the F3d file.

Thanks in anticipation

Andrew Sansome

[Anonymous]

Can any of the technical support specialists help with this simulation?

I would be very pleased to discover where I am going wrong.

Andrew Sansome

[John_Holtz]

Hi Andrew,

I took a look at your model. Frankly, I am surprised that you were able to get the model to converge under any loading condition. There are so many parts that are held strictly by the contact that any little side load can send a part flying off into space.

From what I have been told, a nonlinear static analysis does a better job with contact, so may be an option. That analysis type ramps the loads from 0 to full load over numerous steps, so it may be able to converge if the initial load is small enough, and then gradually ramp up to the final state. But since it is still a static analysis, the potential exists that there is no static solution from a mathematical viewpoint.

The better solution would be a dynamic analysis in which the inertia of the parts prevent things from flying off into space. Fusion does have a dynamic solver (Event Simulation), but it is for events that occur really fast -- on the order of milliseconds or tenths of a second (0.001 to 0.1 order of magnitude). Does your model fit that requirement?

The other option would be to add a part that connects all 36 (did I count correctly) ball bearings together so that you at least minimize the number of parts that can move independently. Think of a stiff wire that passes through holes in the balls, like pearls on a necklace. Then you can use a constraint that prevents the ring of balls from rotating around infinitely in a circle. (That is probably what was causing the instability. Any slight force that causes a ball to move clock-wise forces the next ball to move clock-wise, and there is nothing to stop all of the balls from doing that.)