composite structures , inserts

[a.eliah.cameron]

Hello, I have some questions general questions about composites as well as some more specific.

A but of a rundown om what I'm looking at. A composite tubular section with internal supporting structure.
1) when applying a laminate is it posable to have the surface selected the outer face,(by default is is the centre plane)

2)how does the internal supporting structure interact when a thickness in applied. With the model attached there is visual overlap (when displaying cross section, I am using shell elements). Is there a way, without remodelling, to have a continuous outer skin with the internal structure butting up to the internal surface.

3) At the moment the internal structure is the same material but when changed the mesh doesn't line up (cant use continuous meshing because not solid. 

4) more complex -  I would like the internal structure to penetrate the external skin for mounting, how would this be modelled? 

5) There is also an error I haven't sorted out yet

Any help would be greatly appreciated, I'm fairly new to Nastran/laminates. Reference material, already set up files (laminate) and general laminate material property's would also be great for a bit of exposure excluding the tutorials.

thanks,

E 

[John_Holtz · Accepted solution]

Hi @a.eliah.cameron . Sorry for the delay in responding.

1. Represent the outer surface? Yes. Under the "Idealization > Laminate > Bottom Fiber Distance", you can control where the simulated solid is located relative to the mesh. It appears that you have a symmetric laminate, so the question becomes this: is it easier to draw the surfaces at the midplane? Or is it easier to draw the surfaces at the top (or bottom, or any combination), enter the proper Bottom Fiber Distance, and enter the correct Element Normal direction? After all, if the surface is drawn at the outside, you want the bottom to be in the proper direction!
2. The mesh is what is being analyzed, not the fake thickness cross-section display. The tiny bit of overlap that occurs mathematically does not change the results. (Likewise, the tiny bit of missing material at the corner opposite the overlap is not changing the results.) The typical way of analyzing plates/shells is to create the mesh at the midplane. Although this makes the internal stiffener slightly larger in area (by half the thickness of the outer shell), that does not matter in the grand scheme of a shell analysis. The most important aspect is the bending of the outer shell, and that is best represented by modeling the outer shell accurately (either by at the midplane or at the top/bottom surface with the appropriate offset to simulate the mesh at the midplane).
3. Continuous meshing? Actually, continuous meshing is designed for shell models, not solid models. In some cases it works when the edge of the internal stiffener (B) touches the outer surface (A) in the middle of the face. That does not work in your model. But using the stiffener to split the outer surface does work with continuous meshing to connect the stiffener to the outer surface. "3D Model > Modify > Split".
4. Internal stiffener pokes through outer surface. It does not do this in reality, and it may be tricky to fake it in the model. I assume the real surface has holes to the "ears" to stick through. That would be an option but I think it is overkill for a shell model depending on whether the ears are glued around the perimeter of the hole or not. Another option is to just let the plates magically pass through each other. The third option is to split the stiffener into 3 plates: one internal plate and two external ears.
5. Error. In another message, you indicated the analysis gave an E5000 error which indicates the pieces are not connected together. If continuous meshing is not used, then contact needs to be defined to bond the parts together. 

Figure 1: Model showing the outer surface (A) and internal stiffener (B). (This image has been photoshopped to show the model better!) The solid lines around the outer surface are a split in the outer surface; the solid lines are not the edge of the stiffener. In other words, surface "1" is a different face than surface "2".

John

[a.eliah.cameron]

Thanks @John_Holtz went above and beyond what I expected as a reply, Very much appreciated. 

If i have a closed surface with internal structure, is the a way to hide the outer shell elements to see the internal shells (a cut plane to view the inside). Currently its all under one idealization, would i have to separate to multiple idealizations to hide the external to see the internal, or is there another way?

Separate to this i was wondering if you could have a look at the wishbone attached and give some feedback/help. you referenced "nastran beam solid" in previous messaging and I'm struggling to get this to work on one end of the wishbone(can be seen when looking at solid von mises stress). As well as this I am trying use 'surface contacts' with offset bonded to separate the two as a Block will be places in-between the two.

Attached file 1 shows the connection issue when run 

Attached file 2 shows what I'm intending to analyze, note that the "block" connection I don't what to be a ridged connection only stop the compression between the two members.  

EDIT: Is there a cleaner way to split the solid surfaces? I have done this to represent the 'Pipe' profile. Realistically I would have split the area where the weld is located not the interface of the areas. The split midsection of the solids was to ensure that a node was located at the location the line element met the solid is this necessary or is there other ways to achieve the same thing.

[John_Holtz]

Hi,

---

If i have a closed surface with internal structure, is the a way to hide the outer shell elements to see the internal shells (a cut plane to view the inside). Currently its all under one idealization, would i have to separate to multiple idealizations to hide the external to see the internal, or is there another way?

"Results > Options > Section View" to create a slice plane. A better method would be to create an assembly and put the different pieces in different parts. Then you can use "Results > Options > Part View" to choose which parts to show. (The idealizations created in the Nastran environment are not related to being able to hide or show parts.)

Separate to this i was wondering if you could have a look at the wishbone attached and give some feedback/help. you referenced "nastran beam solid" in previous messaging and I'm struggling to get this to work on one end of the wishbone(can be seen when looking at solid von mises stress). As well as this I am trying use 'surface contacts' with offset bonded to separate the two as a Block will be places in-between the two.

You should not be worried about the calculated stress around the pipe "connection".

• The beam to solid connection is a low accuracy approximation. The stress around the "connection" is not accurate.
• The mesh is too coarse to give an accurate result, even if the approach of connecting the beam to solid were an accurate method.

If the pipe-to-pipe connection is an area of concern, you should model it as solids, not solid and beam. (You can use the beam elements to represent most of the length of the 480 mm long pipe between the blocks, but make the pipe at the connection to the blocks a solid part.

Attached file 1 shows the connection issue when run 

Attached file 2 shows what I'm intending to analyze, note that the "block" connection I don't what to be a ridged connection only stop the compression between the two members.  

Both models have a problem with the rigid connector being attached to a surface that also has a constraint. This is where the error message about a constraint conflict comes from. The rigid connector cannot control the displacement of the nodes when the constraint is controlling the displacement of the nodes. (Nastran does not like that.) It looks like the model needs to be updated by using "Manage > Update > Rebuild All". Then you can check each connector to make sure the face selection is correct.

EDIT: Is there a cleaner way to split the solid surfaces? I have done this to represent the 'Pipe' profile. Realistically I would have split the area where the weld is located not the interface of the areas. The split midsection of the solids was to ensure that a node was located at the location the line element met the solid is this necessary or is there other ways to achieve the same thing.

You should be modeling the solid connection. A split is not required.

John