Shrink-fit shaft coupling FEA with Strand 7

[scatman2244]

Hi All,

Recently I have dealt with some interesting fatigue failures of couplings installed on torque arm mounted conveyor drives. The conveyor pulley shaft and the low speed shaft of the gearbox are connected via a shrink fit coupling (Stuewe FKH 560-180 for example). Since the drive overhangs and is only supported by a torque arm, the coupling experiences a bending moment as well as normal torque transmission. This fully reversed bending moment is the causes fatigue failure on the coupling at the root of the boss and flange, drive side.

Using Strand 7, I have started to investigate this situation using a full 3D brick model. In an attempt to simulate a shrink-fit, a small gap (0.032 mm) exists between the coupling bore and the pulley and gearbox shafts. I've then defined zero-gap beam elements via attachments between side A of the coupling and the pulley shaft, and side B of the coupling and the gearbox shaft. Within the coupling, an axial distance of 5mm exists between the ends of the two shafts to prevent interference.

Just to try and get a working model, I've fully fixed (restrained 6 DOF) the free end of the gearbox shaft and defined the shrink pressure and bending moments in different load cases. My load increment table has the first increment as just shrink pressure (1 for shrink pressure, 0 for bending moment), while the second increment introduces the bending moment (1 for shrink pressure, 1 for bending moment). The bending moment case is just a global pressure -Z equally distributed across the free endface of the pulley shaft.

Despite my best attempts at this, the non-linear solver still has troubles converging and attaining a reasonable solution. If I run the simulation as described above, the shafts usually have massive axial displacements, indicating they are flying out from the coupling before it has a chance to grasp them. To achieve a "reasonable but slightly dodgy" solution, I have added axial restraints to the center nodes of the non-free end faces of the shafts, as well as 2 axial restraints to the coupling on opposing sides of it's circumference. I'm not comfortable with these "dodgy" restraints because they are generating substantial local stress reactions indicating the system is not behaving naturally.

If anyone here has experience with this, a similar FEA situation, or using Strand 7 contact elements, any advice offered would be greatly appreciated.

Cheers,

Peter

 

[Tmoose]

http://www.stuewe.de/media/products/flanschkupplungen_fkh_d_en.gif

The failure (crack) forms in the hub, under, or adjacent to the clamping ring?

 

[scatman2244]

Tmoose,

It fails adjacent to the clamping ring, at the boss-flange fillet root. The boss experiences repeated fully reversed bending.

 

[IDS]

I havn't done any similar analyses, but I do use Strand7 contact elements frequently, and they can be sensitive to the chosen parameters. I'd suggest setting up a greatly simplified model and looking at the effect of adjusting the various options. You might also look at providing the axial restraint with a spring element, and gradually reducing the stiffness of the spring.

Are there any warnings in the output log?

I'd be happy to look at your model (or a simplified version) if you would like to upload it.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[IDS]

Another thing you might try is using a "normal" contact element, rather than zero gap, and selecting "use in first iteration".

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[scatman2244]

Thanks for the help Doug.

I setup a very simple simulation and had a play with the options available and I feel like I am on the right track with my model again. There a few outstanding issues, but they are to do with my mesh. It's quite interesting the amount of influence that setting the initial stiffness of the contact elements has, for the simple simulation the results could be manipulated quite easily. For my proper simulation I left "update stiffness" checked, and was pleased that the final stiffnesses used by the solver were equal for all the contact beam elements.

For interest, I used zero gap elements, since I only want resistance upon interference. To prevent the solver from advancing too far in the first iteration (where the elements are not employed, unlike normal contact), I enabled load scaling in Automatic Sub-incrementation (this is found in the nonlinear static analysis dialogue box -> defaults -> sub-steps). This "eases" in the load so that large deflections aren't experienced in the first iteration.

Cheers mate