Abaqus slow convergence

[dorios]

Hello,
This Q is for Abaqus users (can email the input deck if you wish to have a look):

This is a simple bushing application with an inner Aluminium core that is rotated 90 deg using a spiderweb (using MPC).
The outer wall of the bushing is fixed (in cyl coord) and the bottom of both Al and hyper are constrained for symmetry conditions.

The hyper material was tested on a one 3D element and it is stable for all strains when used with Mooney Rivlin. The dat file shows a very good fit of the test data to the M-R polynom.

I do not understand why the convergence is so slow (job still running ); there are some distorted elements at the upper (sharp) edge of the hyper material but I do not see it as a primary concern.
I used hybrid el's for the hyper material, the unsymm storage should be switched to automatically ( therefore I did not use it unsymm=yes).

(did not use stabilize yet)
thanks
much appreciated

[Jorgen]

Here are a few ideas:

- How large is the bulk modulus compared to the shear modulus? Did you use hybrid elements?

- Try with the C01 parameter in the M-R model set to zero (i.e. then the model becomes the Neo-Hookean which is always stable).

You should be able to get great convergence with a hyperelastic material model.

Jorgen

[dorios]

- yes I use c3d8rh (hybrid el's)
- I use M-R test data rather than M-R coeffic. but when looked at *.dat file at the stability limit, it is stable for all strain for all tests (which I knew because I performed 1 element data fit)
- it reaches 0.348 time step (of 1 which is 180 rorartion of the internal surface).. so it rotates 62.65 deg
Now, the message file shows that the convergence is slow because of the volumetric (strain) compatibility which is related to the usage of hybrid solid elements which introduce an additional dof called pressure stress (additional constraints "volumetric strain compatibility).
I am trying to relax the criterion on this constraint by using
*controls, parameters=constraints
5.e-5,

otherwise I just need a very fine mesh where the elements distort a lot during rotation (immediate vecinity of inner shaft

[dorios]

Jorgen

FYI

M-R does not have a c20 and besides, I said that I provided "test data" which allows abaqus to calculate its own M-R polynom constants.

[Jorgen]

I tried your input file and I believe that the convergence problem is caused by large element distortions! The problem is not likely caused by the material model.

To overcome the problem you will need to either: (1) create a new mesh that can better accommodate the large distortions; or (2) remesh and restart the model at different times during the simulation.

Best of luck,
Jorgen

[dorios]

true, I realise that.It is not a material issue. The fit is very good and stable at all strains. The Q was how to get it further without remeshing.

well, I managed to get it further (to 90 deg rotation as opposed to 62 previously) by using C3D8h elements instead of c3d8rh and also by using "stabilize" and the unsymm solver.
90 deg rotation of the internal bush is enough for my purposes (I don't have abq explicit).
thanks
dorios