{"id":29326,"date":"2018-05-20T01:44:48","date_gmt":"2018-05-20T01:44:48","guid":{"rendered":"\/forum\/forums\/topic\/bonded-contact-between-rigid-bodies\/"},"modified":"2018-05-20T01:44:48","modified_gmt":"2018-05-20T01:44:48","slug":"bonded-contact-between-rigid-bodies","status":"closed","type":"topic","link":"https:\/\/innovationspace.ansys.com\/forum\/forums\/topic\/bonded-contact-between-rigid-bodies\/","title":{"rendered":"Bonded Contact between Rigid Bodies"},"content":{"rendered":"

Deepak Maurya<\/a> has been working on a simulation of spinal bones and the disks separating them. Bone is a couple of orders of magnitude stiffer than disk material, so one model represents the bones as rigid bodies while the disks are flexible bodies.<\/p>\n

<\/p>\n

Some protrusions from the bones slide on each other, so he has used frictional contact between them.  Some diseases of the spine fuse those bones together.  To simulate that, the frictional contact is changed to bonded contact.<\/p>\n

<\/p>\n

Deepak asks why there would be any deformation in the disk if the rigid bones are connected with bonded contact. Rather than work on his very large model, I have a very small model.<\/p>\n

<\/p>\n

It has two rigid bodies with a flexible block between them. The block between them is bonded to each rigid end body. One rigid block is fixed and the other has a force applied. There is also a frictional contact between the rigid bodies.<\/p>\n

<\/p>\n

\"\"<\/p>\n

<\/p>\n

If the frictional contact is changed to bonded contact, this is the result.<\/p>\n

<\/p>\n

\"\"<\/p>\n

<\/p>\n

The flexible body has practically zero deformation.  Is this what you are seeing?<\/p>\n

<\/p>\n

If not and the deformation with bonded contact is similar in magnitude to the frictional contact case above, then that is likely due to some conflict in the model, an over-constraint that makes it impossible for the solver to satisfy all the constraints at the same time and so some constraints are ignored in order for the solver to continue.  When this happens, there are always WARNINGS in the output file such as this:<\/p>\n

<\/p>\n

<\/p>\n

  *WARNING*: Some rigid target elements (e.g.810) in real constant set 5 
 overlap with other MPC\/Lagrange based elements (e.g.1123) in real      
 constant set 10 which can cause overconstraint.                                         <\/p>\n

\n<\/p><\/blockquote>\n

<\/p>\n

The problem with a complex model is that there are likely to be many warnings, but most of them do not represent a true conflict. For example you can have separate contacts on adjacent faces of a block that gets bonded into a corner. The nodes on the edge of the block belong to two contacts at the same time, so a warning may be issued, but there is not an actual overconstraint.<\/p>\n

<\/p>\n

The ANSYS 19.0 archive for the model above is attached below.<\/p>\n","protected":false},"template":"","class_list":["post-29326","topic","type-topic","status-closed","hentry"],"aioseo_notices":[],"aioseo_head":"\n\t\t\n\t\n\t\n\t\n\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t\n\t\t