Seal compression into groove in 3D

[Pluckkk]

Hi all

In one of my 3D analysis, I have to compress a seal into a groove which is formed between 2 parts
First step is ok, push the ring into the groove
2nd step is to remove the "pusher", ok also
But the third step ... When I compress the upper part, at some point the contact "explodes" because the rubber extrudes into the groove

- Analysis is done using explicit solver (I attempted to do in in static this failed) with stable time increment to accelerate to calculation (but not too much)
- Rubber is neo hookean
- I tried all types of contact between the 2 parts (included general contact), same problem
- I tried ALE adaptative meshing with C3D8R elements for the seal, same problem
- Analysis is 3D, 36° sector with symmetry BC's

Any thoughts ?
Thanks

 

[Dave442]

how did you define the material properties? specifically, the compressibility?

 

[Pluckkk]

Hi Dave442, For material properties I have Neo Hookean rubber so C01 = 0.73 and D1 = 0.001 which takes into account incompressibility

 

[Dave442]

It's a while since I did this so maybe check the numbers for yourself but your parameters yield an equivalent poisson ratio of 0.4995. If I recall correctly, Explicit is not suited to modelling incompressible behavior (infinite wave speed). An upper limit of K0/G0 of 100 is suggested in the documentation to avoid high frequency noise and excessively small increments. From your parameters, K0/G0 ~ 1400. (Getting Started with Abaqus -> Materials -> Hyperelasticity -> Compressibility).

I would suggest returning to Standard and using the hybrid elements to model the incompressible behavior. If that's not an option you could add compressibility in explicit and make a judgement call. Other options I would consider are refining your mesh (it looks quite coarse) and trying softened contact?

What was the issue with the static analysis out of interest?

 

[Pluckkk]

Thanks for the advice I did not remember this help section. I will try to add some compressibility and relaunch to see. If I refine the mesh this leads to huge time increments that's why I try to avoid it
What is it you define as "softened contact" ? Is it using penalty contact method or linear normal behavior with a contact stiffness or something like that ?

In static I must re-try because I am using a different seal now, buyt anyway I started in explicit because the following steps won't work in static also ...

 

[Dave442]

As you add compressibility in your explicit analysis you will reduce the material wave speed and increase the stable time increment, so you should have more wiggle room for your mesh. By softened contact I meant to avoid using "hard" contact for the normal behaviour. Instead you could try using an exponential pressure-overclosure relationship for your normal behavior to allow some penetration - might help?

 

[Mustaine3]

In Explicit I would also recommend to refine the mesh and maybe add some mass scaling, to keep the stable time increment up. No need to use soft contact in Explicit.