Abaqus Inertia Relief

[StressAsh]

I currently have an Abaqus model and it is giving me the following errors:

The model has no boundary conditions for inertia relief. This may cause at the most 6 numerical singularity warnings during each equilibrium iteration in the analysis. The displacement solution will be postprocessed to remove unconstrained rigid body motion. However, any extra numerical singularity messages may indicate other problems; please rerun the analysis with statically determinant boundary conditions

Inertia relief load will not be applied to elements that do not have a mass or inertia property associated with them, for example, acoustic elements, springs and dashpots; do not have finite boundaries, for example, infinite elements; or do not support fixed boundaries, for example, elements with foundation loads. In this model such elements are identified in the set irloadn.

This model contains gap/coupling/dashpot/spring elements and/or kinematic constraints which may cause unbalanced internal forced/moments associated with internal boundary conditions, E.F., ground node in spring1 elements. These internal forces/moments are not balanced by inertia relief loads. They appear as reaction forces/moments if sufficient boundary conditions are present; otherwise they appear as unconverged residual fluxes in the .msg file.


These three errors I cannot seem to fix. When I add boundary conditions I get a new error stating that the model is overconstrained. I have added contact initialization to remove over closures and gaps which does not solve the gap error. I have done a modal analysis and all regions are connected. There are structural couplings connecting masses to the model but no kinematic connections.

Any ideas would be awesome!
Thanks

 

[FEA way]

Here are some hints regarding the use of inertia relief that should help you:
- this feature has some limitations: it won’t balance internal forces from elements such as springs, dasphots and kinematic constraints (couplings, MPCs, surface-based ties). What’s more it won’t work when there are unconnected regions (even with contact defined for these regions - only tie can be used in this case)
- due to these limitations you should apply additional boundary condition and ties to balance internal forces and eliminate rigid body motions between unconnected regions
- when you apply boundary conditions in analysis with inertia relief, you should select only unconstrained directions (those without BCs) in the inertia relief definition
- inertia relief requires specification of material density or mass/inertia values

I can advise you how to apply proper BCs in your analysis but I would have to see your model.

 

[StressAsh]

Thank you for the hints to the boundary conditions. I will change the inertia relief and add a boundary condition in the free directions. Is there a way for Abaqus to show where the gaps or internal forces are? I do not have any unconnected regions.

 

[FEA way]

Those gaps mentioned in the error message are not literal gaps in the model. They are gap elements used in contact.

Unbalanced internal forces and moments appear as unconverged residual fluxes in the message file, as stated in the documentation. So basically you will only know they exist from warning messages but you can’t visualize them.