Dynamic global - static local analysis of big structures

[ahkrit]

Hello!

I am looking for an efficient way of analysing bigger structures. The global analysis is a dynamic analysis, in which a local part, joint should be calculated in a local analysis in different time steps.
What would be the most efficient way for such analysis?

I tried submodeling, unfortunately it does not work as good for exact time steps and for the fine meshed local model it is not possible to analyse the full dynamic step.

Tried substructuring too, there the issue is that contact cannot be defined inside of substructure.

Any suggestions?
I am wondering how it is usually done in practice. Must be a proper solution to that.

Thanks!

 

[FEA way]

It depends on the case (what kind of structure and what kind of response you want to evaluate). In some situations, it's possible to e.g. model the larger region of the structure using beam or shell elements and then transition to solid elements used locally. Sometimes rigid elements and other simplifications can also help reduce the size of the model.

 

[ahkrit]

This is a floating structure consisting of longer closed or open section profiles connected different ways at the ends (bolted, riveted or welded).
Fully dynamic response is simulated and the joint (beam end connections) stresses i would like to calculate with local static analysis.
Submodel seems to be a nice option for that, but only if i run the full dynamic analysis locally. If i use "Node-based submodeling using the field import interface" it has unfortunately bigger differences comparing to dynamic analysis.

All the simplifications are included in global model, that is not the problem. The issue is how to get local stresses in given time steps.

 

[NRP99]

You can take out the global forces and moments at the cut section of global model and apply it in the local model. Or you can extract the dynamic response at the cut sections in global model and apply it to local model.

This is exactly what sub-modelling does and instead of forces and moments, displacement are applied at the cut section. Its not clear why you are not getting the exact same results with sub-modelling. It should work. Are you properly applying the BC's, defining exact steps like global model?

 

[FEA way]

There is also stress-based submodeling in Abaqus but it’s limited to static analyses. However, it can calculate stresses more accurately for models with load control and significant difference in the stiffness of the submodel and global model (in the region of the submodel).

 

[ahkrit]

I have to correct myself. Node-based submodeling does work, even with Fiel import interface option, taking out one time step from a dnyamic simulation.
So that works.

Now my question is what i think @NRP99 you were also reffering to with "take out the global forces and moments at the cut section..."
If we model a structure which has what ever bolted or riveted joints. Can it be modelled as rigid coupling or should be the stiffness of the joints included in the global model?
Because if we do apply displacements as boundary conditions on the local model i believe we really need that, would that change if we apply SF and SM as boundary conditions?
So basically, do we need the local stiffness of the joints included in global model anyway?

Thanks!

 

[FEA way]

Based on the Saint-Venant's principle, you should keep the boundary of the submodel away from any regions where the response changes. But as long as you take this into consideration, you can safely introduce additional features (such as holes and fasteners) in the submodel. As I've mentioned before, stress-based submodeling may provide better results when submodel has significantly different stiffness.

 

[ahkrit]

Sorry if I was not clear but my question is if a given joint`s stiffness has to be included in the global model?

I cannot use submodel as i have beam model(and it is not my goal nor my question). I am trying to solve the global model with beams and apply SF and SM values on local model.
If you look athe image below you can see two types of the global model. One where the full length of the connected profiles (as beams) modelled with kinematic coupling connected at the ends. On the other side where the local part of the joint is hidden(modelled with shell and connector elementes). This i often cannot see or did not find any documentation, examples that the stiffness of a joint is always included that way. Question is why? if it has some difference in SF values as you can see on the picture.

 

[FEA way]

All right, so you are talking about analyses without the use of submodeling technique but with manual division into global and local model.

It might depend on the type of structure. If it's large and with lots of such joints (like a transmission tower) then you won't be able to account for their effect on the entire structure anyway. But if it's small and has a few joints the stiffnesses of which may influence the global response then such a detailed modeling approach might be a good idea. Still, I don't think it's very common.