Linear load + boundary conditions

[azou]

I am trying to model a shaft supported by two bearings, ball and roller bearings, one at each end. This shaft is loaded in the midle (linear load) by a static load. I used a 3D solid emlement solid95. The problem that I apply a linear load as a linear pressure but at the end of the calculation, the deflection of the shaft is 0 every where and I get a message in the error file saying that the line where the load is applied is not associated to the meshed area and cosequently it has not been accounted for. I can apply a surface pressure on the top of the shaft but it doesn't replicate the real case. Anyone has a suggestion...!!

A second point is more for verification concerning boundary conditions, As I said the shaft is supported by 2 rolling bearings, ball and roller bearings. For the ball bearing, I have constrained the surface displacement in all directions (ux, uy and uz)to be 0 and for the roller one I constained the displacement only in 2 directions allowing a displacement in the axial direction. If u have any comment, please let me know it.

Azou

 

[Drej]

> the deflection of the shaft is 0 every where and I get a message in the error file saying that the line where the load is applied is not associated to the meshed area and cosequently it has not been accounted for. I can apply a surface pressure on the top of the shaft but it doesn't replicate the real case. Anyone has a suggestion...!!

Rather than applying a pressure on a line, apply a force directly to the nodes. Select the line (lsel,s,p), then select the nodes attached to the line (nsll,s,1) then apply the force (f,all,...). This is assuming the nodes are attached to the lines. From your error message I wouldn't be surprised if the line isn't associated with the FE model.

> For the ball bearing, I have constrained the surface displacement in all directions (ux, uy and uz)to be 0 and for the roller one I constained the displacement only in 2 directions allowing a displacement in the axial direction. If u have any comment, please let me know it.

I think you may be overconstraining your model here. I would recommend you rotate the nodes at the bearing locations into a cylindrical coordinate system and apply the boundary conditions with this coordinate system in mind. It's hard to know exactly how the bearings are acting without a more detailed explanation. If you search this website (see the search facility above) I think you should find more information on how to model bearings.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[cbrn]

Hello,

only two words about how we account for bearings at my company:

1) simplified analyses (conceptual design, first-pass evaluations):
- cylindrical CSYS with axis on the shaft axis, circle of nodes constrained in UX. The circle is axiallyplaced such that:
* if the load configuration is such that both sides of the bearing are loaded with forces of the same magnitude order, axial position is at 50% of the bearing length
* if the load acts prevalently on one side of the bearing, axial position of the restrained circle is at 66.6% of the bearing length, towards the load's side
- UZ constraint on all the nodes belonging to the axial thrust bearing
- UY constraints on a "reference", when a torque is applied (midplane of a gear, or midplane of a lever, etc...)

2) detailed analyses: all nodes belonging to the bearing's surface are duplicated at a distance "s" equal to the bearing's radial characteristic value (Lubriflon thickness for example), and COMBIN14 elements are established between them, having stiffnesses calculated according to the real bearing characteristics. Then, external bearing nodes themselves are duplicated and additional COMBIN14 are set to simulate bearing structure's stiffness.
Same concept is used for thrust bearings.

Hope this can help...

Bye!

 

[azou]

thank you guys for yoyr input. I appreciate it.

Azou