Shell Model - Flexible Panel With Outer Frame

Paul

Hello,

I am trying to model a thin curved panel with a relatively thick outer frame. The assembly has a hinge interface on one side, and I am interested in how much deflection there is at the other side caused by the weight of the components. I tried making a shell model of the assembly, which worked well for linear analysis, but I am having a hard time getting it to solve when I transition to a nonlinear model which is needed due to the large deflections. I am using the elastic option for the bonded contact in the nonlinear case, and I am getting "nonpositive Jacobian determinant" in some of the elements of the main shell.

I've also tried replacing the frame components with solid bodies, but I have been getting errors with "Too many cutbacks" when I do this.

Any feedback, or suggestions would be greatly appreciated.

Thanks,
Paul

Overall Assembly Image:


Frame Image:


Mecway Shell Model:

Victor

Keep in mind that elastic bonded contact moves the slave nodes onto the master faces, so it might severely distort the mesh with the master so far away. Distorted elements cause non-positive Jacobian determinant. Try using the frame face as master and the immediately adjacent panel edge as the slave. Also, arrange the mesh with a gap because contact applies to the expanded (due to thickness) faces of shells, not the midsurfaces.

I wouldn't use bonded contact though. I'd extrude the frame mesh from the edges of the panel. That should be more reliable and easier to set up.

If convergence fails with "too many cutbacks", there might be rigid body motion. In particular, the bonded contacts might not have worked. Do modal vibration to look for 0Hz rigid body modes if they're not obvious.

Paul

Hi Victor,

Thanks for the quick response! I tried offsetting the frame pieces to account for the thickness. This worked with the straight side pieces, but when I added the curved top, I'm getting the Jacobian error again, I'm assuming it might be related to the fact that the shells are not perpendicular to each other. I used this angled surface to match the moments of inertia of the true geometry.

I am also trying to capture different material properties and densities between the frame, and the panel. Is there a way to do this with the mesh extrude method you are describing?



Section Properties:

Paul

Updated model with offset surfaces for reference.

Victor

Yes, the extruded elements can have different material properties. After extruding, select them, right click one, and Add elements to new component.

Here it is with appropriate master and slave surfaces and it solves successfully.

Paul

That's perfect, thanks again Victor. My apologies for missing your note on using the edge in your first response. Is there a quicker way to select that edge to add it to the contact? The only way I'm aware of is to use the "Paint Selection" tool or the "Rectangular/Circular Selection Tool" and carefully select all of the edges, but this gets challenging as the mesh density increases.

With the extruded elements option, does breaking the elements out into a different component break the physical link between it and the component it came from? I tried this earlier today, but ended up having to redefine the mates again anyway or I would get rigid body motion.

disla

.

Victor

To select edges, you can orient the view along the edge, select the nodes which are all together, then switch to select faces mode.



Extrusion keeps the extruded elements connected to the original ones and components don't do anything in the solver except having materials associated with them.