I always have some slip at the edge of my contact

[remit]

Hello,

I am training on a simple model to understand how contact works in Abaqus. You can see the model and the mesh on the imgaes.

It is an elastic cylinder on a rigid plane. I apply a uniform pressure on the top of the cylinder. The contact is defined like this : hard direct for normal behaviour, penalty with mu=100 for tangential behaviour. I know it is a high value but it was to see if it could solve my problem.

Even in this configuration, I have a slip region at the edge of the contact. I have tried to change a lot of things but it stays the same. I cannot understand why. Is it a numerical problem ? Also, I don't understand why the contact zone is larger than the cylinder diameter...it is always like that but it goes better when I use a finer mesh.

Thanks a lot

 

[akabarten]

Hi,

Is it a numerical problem ?

Nope, it is a visualization problem.
Abaqus/Viewer shows colours for elements and CSTATUS output is related to nodes.

Just think in this way, sticking is value of 1.0, slipring is value of 0.5 and open status has value of 0.0.
Each value is plotted with different colour, blue for 0.0, green for 0.5, red for 1.0.
Elements close to small cylinder from one side have nodes with open status (0.0) and on the other side with stick status (1.0).
It means over element we are changing value from 0.0 to 1.0 and somewhere in the middle is value of 0.5.
Value of 0.5 is slipring (something between open and stick status) and this way you see ring of green colour.

It seems to be a stupid but ask yourself if I one element has open status from one side and close status from other side what colour should I plot (blue or red) ?
Abaqus/Viewer makes something in between and plot transition from blue to red over element area.

Hope now you get the picture.

Regards,
Bartosz


VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[remit]

Hello Bartosz,

thanks a lot for your reply it is very helpful. I understand now.

But I still I don't understand why the contact zone is larger than the cylinder diameter...Do you have any idea ?

 

[corus]

The contact zone isn't larger than the cylinder, it's just using contours between 0 and 1 in the elements adjacent to the contact region. Use a different mesh size and you'll see the contact zone apparently change with the element size.

 

[remit]

OK. I understand now your first answer also explained that.
Thanks a lot.