Initial distorion in rubber bushing around shaft - Ansys Workbench 13

[necktwist]

Hello the ultimate engineering forum, now that i have changed my focus from metallugry to fea - i need your help with rubber bushings in Ansys Workbench 13. I can get the solution to converge fine even with frictional contacts - no issues. However, i dont know where to start on the real distorted bushings and oval bar from bending.

Working solution: use perfect round shaft and round bushing, do not account for any bracket preload that will compress parts of the bushing prior to loading (during vehicle installation). - that works great.

Non working solution: how do i put a round bushing around an oval bar and obtain the proper compression in the rubber as the bracket tightens around the rubber busihng that is trying to conform to the oval steel bar? That is what i need for the initial condtion, and then i can apply the loads. the perfect round and even bushing pressure scenario above isn't real.

is there a bible or anything i can read on how to obtain this pre-loaded rubber. ps, NO I have not got non-linear large displacement to converge yet using actual rubber hyper elastic curves so for now i'm just practicing using a simple linear elastic material with a high poissons ratio and weak E. (looks cool flexing all around, freakin real hyper elasic is the next level up in difficulty.)

thanks for reading, hope i can help others here too.

 

[necktwist]

<fool>
i wrote 'distorion' in the title instead of distortion, of course no way to edit.
</fool>

 

[flash3780]

You could build a model of the oval shaft in the circular hole with ramped deformable contacts and let Ansys determine the final shape, no? I'd think a quarter-symmetry model would be sufficient.

 

[necktwist]

Yes thats a great idea. I will let ansys do the 'installing' of the bracket over the bushing.

I need the entire model because of the variable reactions from the opposite side of this part. Also its not real that i have a bonded joint, need to figure out my non convergence issues with frictional. trying to figure out code snippets using the /prep7 to get the non linear going (also used hex based mesh to no avail).

can't get this snippet to work

/PREP7

KEYOPT,9,4
KEYOPT,12,4
FKN=0.01
KEY,10,1
FINI

/SOLU

but hey, i'm going to take your advice and research the hell out of ramped deformable contacts since that seems logical. Thanks flash3780!!!

 

[necktwist]

turns out i needed keyopt 6,1 snippet under the 'geometry' section. that makes hyperelastic work (incompressible).. w/o that it would not converge.

then i needed keyopt 9,0 under the frictionless interface section, that actually tells ansys that i am not making a mistake, i want to solve that initial penetration or gap.

now the problem is adding friction, as soon as i add 1.0 friction coefficient, it wont converge. if i stick with 0.2 it will BARELY converge. whats up? any way to handle hyper elastic with friction?

 

[fuzzdoug]

i too find it difficult to include friction in any analysis with hyperelastic models.

i've recently been doing a lot of work with sealing applications.

i tend to keep the friction very low (0.1 to 0.01).
remember friction is actually very dynamic and dependent on a lot of things.
too many for any practical assumptions in this case.
if you set it too high, you could actually cause a lot of slipping and skipping.
this doesn't behave well in a static analysis.
solver will not converge w/ quick changes in velocity.
the stability options help...

try considering an augmented lagrange formulation and adjust FKN.
this formulation will try and control penetration AND the penetration tolerance for convergence.
just watch your penetration.

this may provide some insights:

http://ansys.net/ansys/papers/nonlinear/contact_tech.pdf

http://www.axelproducts.com/downloads/Friction.pdf

there are also a lot of good docs on

http://www.padtinc.com/

but, i can't seem to get on their site atm.

 

[necktwist]

Thanks for that info fuzzdoug. sorry i took so long to respond i did take the non linear class at Ansys in Ann Arbor, MI and I still can't get it solving.

I also pulled a help ticked and they are working on it.

FYI - Augmented helped but only solved it for a very small displacent. Also, you mention keeping the penetration down but my main problem sets are based on initial penetration of the rubber. Almost all automotive rubber is squeeze fit or stretch fit.