Shell thickness

Andrea

I'm doing a calibration study for Nonlinear buckling of a welded lifting beam. Because of dimensions I have to model it with shell elements.
In the reference model there are two different thickness. I can't create two different components an apply "Tie surfaces" because could lead to issues on buckling analysis and nonlinear analysis. I have solved manipulating inp file.
Is possible to apply two different shell thicknesses via pre-processor  to only one component?

Benchmark 6.24 - Obtained buckling factor (first eigenvalue) 6.23

Victor

While you have to use different components for different thicknesses, they can still be connected by shared nodes without needing any kind of contact or tie. You can split one component into two by selecting the required elements and making a new component (right click a selected element -> Add elements to new component). Then modify its thickness independently of the first one. A weakness of that approach is that you have to do it after generating the mesh and if you remesh it, you have to do the splitting up again.

I'm not aware of bonded contact either with or without tie being a problem for linear buckling, nor of tie being a problem for nonlinear analysis. Can you elaborate on that?

Andrea

The problems were related to the geometry. In fact importing step file without partioning the faces (shared edge at the intersetion) the automesh doesn't creates shared nodes.

Problem related to contact is solution time and it has no sense for a welded component.

Victor

That's curious about the mesher creating mismatched edges. Perhaps because of 3 surfaces intersecting at one edge which is not something it's supposed to handle.

Bonded contact doesn't typically add much to the solution time unless the contact region really dominates the mesh. It doesn't do any iterations the way general open/close contact does. Though it will take a bit of time for the solver to set up the MPC equations between the faces.

We might be talking about different things. There's:

Bonded contact - Mecway generates constraint equations (*EQUATION in CCX) to tie the surfaces together. Only for linear analysis.

Bonded contact with TIE option - Mecway generates a *TIE card for CCX. Only needs linear analysis but can be used in nonlinear too.

Contact with PRESSURE-OVERCLOSURE=TIED - not exposed through the GUI. CCX does penalty contact but doesn't allow the surfaces to separate. This might be nonlinear and slower than the other two.

Andrea

I attach LIML file with mesh of the model: first with partitioned faces and the second without partitions.

Excuse me but I think that I created confusion because  the first time that I created the FEA model I didn't see the separated mesh. In fact under "Components and materials" compare only one part so I didn't check the mesh.

Victor

Here it is with the disconnected edges joined by bonded contact.

TIE doesn't work here. I think it's because the webs intersect the flanges. You might have to separate them by half the material thickness to use TIE.