There may be times when a static analysis in Abaqus/Standard aborts due to contact not being established between bodies in the assembly initially, or due to absence of other active interactions (such as couplings, connectors or constraints) between them. Convergence issues due to rigid body motion may occur in such cases. When there are no “connections” or no mechanism to transfer load between two instances in the assembly, one may see a warning message that says:
“There are
An easy way to identify these unconnected regions is to run a datacheck, with the following arguments in the command prompt:
“abaqus job=
An output database file (.odb) will be generated, and element sets will be created by grouping each of the unconnected regions. These element sets can be viewed using the display group feature in the visualization module of Abaqus/CAE or Viewer. The various unconnected regions will show up as MESH_COMPONENT 1, MESH_COMPONENT 2 e.t.c.
A message (as shown below) will also get printed in the message (.msg) file showing how many nodes each of these unconnected regions have.
In some cases, even though contact is defined between two or more parts, it may not have been established or closed in the initial state - in such cases, the regions will still be considered as unconnected. You can check the initial contact status by requesting for the output CSTATUS. If the contact status shows ‘closed’, then contact has been established, and you may not get the warning related to unconnected regions. If the contact status shows ‘open’ for a particular surface, it means that contact has not been established in that region yet.
You can then take appropriate action based on this information, and if required, fix the model to ensure interactions are active.
There may be other approaches that Abaqus users employ for unconnected regions in a model – such as doing a frequency extraction/analysis,and then looking at mode shapes to check for disconnected regions. The approaches described here are are just some of them.
