Interference Fit Modeling

[markborges]

Hi All,

How do you model an interference fit in abaqus standard? I have a bushing pressed into a plate--pretty simple, tet 4 elements (once I get it running midnodes will be added).

Contact surfaces have been created from the element faces, normals checked. Contact pairs created, node-to-surface, no adjustment, small sliding. Surface interaction defined w/ friction.

On the "contact interference" card I have v defined as -.1. As i understand, this will allow the initial penetration. Op new is defined and that is it. my result shows a highly strained bushing w/ diplacemenst as high as .5mm. This is fine, but I get the same result for two different bushings. One w/ interference and on w/o.

I also get the exact same result if I use the shrink option. It acts as if there is some default interference that it is applying.

My preprocesser is Hypermesh 9.0

Any suggestions?

 

[vumat721]

I would recommend not specifying "v" on the contact interference card and let Abaqus figure it out automatically based on the initial overlap of the two surfaces. I'd also recommend using finite sliding instead of small sliding. So you would have:

*Contact Pair, interaction=IntProp-1
surface1,surface2

...

*Contact Interference, shrink
surface1,surface2

 

[markborges]

Ok, I think that I got it to work....
contact pair, interaction, name, small sliding
slave surf, master surf

surface interaction, name,
surface behavior, pressure over closesure=hard

contact interference, amplitude=name, op new, type contact pair
slave surf, master surf, -.xxx, _, _,_

This way I get .006 ue. I think I was just missing the surface behavior info.

With your method (I assume w/o a clearance card), I get .014 ue.

So, I got something, it seems to respond to small changes; but I am not sure if it is correct.

Thanks for the input.

Mark

 

[vumat721]

Both methods should give you the same result if the underlying material in each body remains elastic while resolving the interference (and there is no friction). You might want to try both methods with brick elements (e.g. c3d8r) which are much more reliable in a mechanical analysis.

Just to be sure, your two parts start off overlapping? i.e. your bushing is a bit bigger than the hole in the plate that you've placed it in? (And, this is possibly ignorance on my part, but what's a "ue"?)

 

[markborges]

just got your post, sorry "ue" is my abbreviation of micro strain. Yes, on my test model, I had the interference modeled in; ie., overlapping surfaces.

On my large model, which has ~25 contact surfaces and four press-fit bushings, I have been getting problems w/ convergence. I've been using the method that I outlined above. Most of the problems came from small gaps between sliding parts. Once an intermediate step was added to close this gap I had some success. Now that I have a working model, S4 and Tet4, I tried to convert it to 2nd order and I am not able to get convergence. Any ideas?

Mark

PS I do have friction and on my test models, I had the same friction on both.

 

[vumat721]

I would definitely recommend trying a linear brick elements (c3d8r) before trying to simplify your model to shell or tet elements. But there are so many other variables, nobody can say why you're getting errors without seeing the model and results...