Offset for beam element to place stiffeners on thin shell elements

Nordlicht

Dear all,

I'm searching for a possibility to create beam elements as rectangular bar or general section on shell elements to model fast metal sheets with stiffeners on it. The challenge is to give them an offset to move them in the correct position. To define additional notes for the beams is an option but this is time consuming. Does somebody has an Idea to handle this smarter?
Is there a function which can be used?

Thanks for your support.

disla

Hi Nordlicht,

Beam elements can't be offset. What I normally do is to align the closest set of nodes to the final stiffener position using Node's Coordinates/Mesh tools menu. Then, select the aligned nodes and press line/surface to get the common line and extrude it to build the desired stiffener shape. It is easier than drawing the stiffener and then merging or stablishing the contact. It would be a stiffener made of Shell plates. It also works on curved shapes.

disla

For complex stiffening paterns or double curved shapes you can also draw your stiffener profile on a node and then Sweep it along a path drawn on the shell surface. Of Course you will need connected nodes along the path.

Nordlicht

Hi disla,

thanks for your quick answer and your expert tip. I have tried to follow your instructions and it runs very well.
But with respect to Mecway support an offset for beams should be implemented to speed up the design work for the model. Even if you have to update the structure according to the calculation results it would be easier to change.
An other challenge is the end connection of your provided solution. If you simply extrude the profiles have sniped ends. You need to connect them to the end structure to get the correct calculation results. But this seems to be actual the only way to solve.

Thanks for your feedback.

WBR Nordlicht

disla

You are welcome,

Right, I normally work with cylindrical shells, so the end tips end connected without effort. In your case, if you are working with flat shapes or chutes like the ones used in mining for example, the sweep technique will be better providing an extra node so you can turn around the corner.

Beams offset would be a nice improvement, but I think shells provide superior information like flange/web buckling.

Nordlicht

Dear Disla,

thanks again for your feedback. Beams offset will be improve the program in the right direction.
I tested in the meantime several options to create modifiable stiffeners and came to the conclusion that your first hint is the best for my type of models.

I also accept that the end connection of faces are not connected correctly. See pictures
So in this case they are defined with sniped ends. This is fully okay when the structure is designed in this way.

My way to create a fixed end connection:
If the stiffeners connected by a bracket the grid has to be refined and a bracket can be added by a Element type "tri3" or "tri6". For sure this not comfortable but feasible.

Maybe you have there other ideas?

Thanks again for your time.

WBR

Nordlicht

disla

Hi,

I normally don’t stiff from the inside (except for the trays on distillation columns as they are the stiffener and the tray support at the same time)
In my applications there would be product accumulated on top of the stiffener and it is not ok.
In your case I would proceed as shown in the picture with an additional final refinement. It is directly handmade extruding.

disla

The file with quadratic elements (>1000 nodes) looks much better.

cwharpe

Hmmmm. Aspect ratio of triangles look a little sharp, but results were comparable to a full quadrilateral model.

When modeling shells, I try and use the largest element size possible, then refine from there.

cwharpe

<img

disla

@cwarpe

Looks great!

@Nordlicht

Your chute looks symmetric. If your box is a rectangle, you could apply symmetry and you only need to model one corner.

disla

Hi,

I must correct my previous post. There is a way to offset beams when using the ccx solver and adjust stiffeners positions.

I requires custom cards but it is not complex.

First go to the Element Properties in the Mesh Tools menu and set the proper direction of the V axis for your beam.

Create an additional custom card containing the same *BEAM section description generated in the inp file and add at the end an OFFSET parameter.

For example:

*BEAM SECTION,ELSET=Stiffener, MATERIAL=Steel ,SECTION=RECT, OFFSET1=-0.55
0.05,0.005
0,1,0

*BEAM SECTION CARD will change depending on your problem but should all look very similar.

1-Component name (Stiffener in my example) , Material (Steel in my example), Beam type (RECT in my example), OFFSET1= (as required)
2-Beam dimension1 (V direction) , Beam Dimension2 (W direction)
3-V axis direction (Dimension1).

Offset can be applied in two directions . OFFSET1 in V direction and OFFSET2 in W direction.

OFFSET has dimensions of the dimension of the corresponding direction.

I have attach two examples. Shapes are limited to the beam sections available in ccx.
I still have to test if results are right but it looks fine at first sight.

EDITED: Just in case Omit keyword block *BEAM SECTION to avoid unexpected conflicts with the cards generated by MECWAY. Files Updated


For more details check the ccx manual. (7.3 *BEAM SECTION)

disla

The offset card allows to build custom beams in ccx extending considerably the available sections.
I have tested with a custom build IPE160 but I don’t really think it is worth the effort unless one builds a library or needs a specific custom profile.
This kind of assemblies requires a bunch of nodes to get reliable results compared to the internal for example. Some of the elements are not very accurate.
Shear ZX Stress seems to show discontinuities in-between elements.

Never know, maybe someone finds an interesting usage (probably as custom Stiffeners ,composite beams, or more detail on stresses inside the elemnts) . I have attached the tested IPE160 file and the comparison results for a punctual load. Good result is obtained with 312 nodes compared to the 5 nodes with the internal solver.

Andrea

I looked at this model
I noted a strange behaviour of shear stress. It's unreliable in therms of value and distribution.
Maybe is better to use shell elements.

disla

Shear ZX Stress seems to show discontinuities in-between elements.

Right.

EDITED:Reduced integration doesn't seem to have this problem.