How to mesh complex models 4

[huiying]

Hi,
I have a box with some components in them attached to the box by means of bolts, screws. Furthermore, the box has a cover with is screwed down to secure it. Because of the screws attachments, I have lots of holes in my model. Also, components are not of regular shapes.
Would like to know how whether
1. it is appropriate to delete away all the holes?
2. how to model the attachment interface?
3. how to ensure connectivity between the meshes in different components?

Thanks & Regards.

 

[sean01]

Huiying,

I think the options you have in this instance are as below - although the apply equally to shell and solid elements, I would personally stick to shells - particularly if you feel your 'box' is complicated to model !!!

(1) Model the holes as concentrics.
Here you mesh concentric circles of elements around the holes. Try to keep the diameter of the first concentric fairly small (+1-2mm) around the bolt hole - then increase the concentric size as you move away from the bolt hole. Three concentric rings should do it. You can then model the bolt, attach a force to it, and you with the right boundary conditions you will get some good info about clamping forces and energy distribution around the hole.

This style of modelling is fairly typical for fatigue analysis.

(2) Model the hole as its own element
Here you model the hole as its own element, then project the nodes/elements from mating holes/ faces onto one another. This is sometimes referred to as 'match meshing'. You then assign the elements representing the bolt holes unique material and property ident (most typically rigid) and then connect the matching elements representing the joints with an RBE 2/3.

Each method has its own advantages relative to the study being performed, although there is nothing to stop you combining the two methods (the only penalty being an increase in model and therefore solve-time proportional to the amount of holes) because you are a little vague as to what analysis you are trying to achieve - I think in general I would probably recommend the 2nd method.

With respect to your third point about connectivity - the 2nd method gives you good visibility in your chosen pre-processor that you capture all the required connectivities in the right places before solving. However, when you attempt to solve without everything connected - you will get an error message reported by the solver (for example - in NASTRAN search for the term FAT in the appropriate file).

Hope this helps

sean

 

[huiying]

Thanks for spending your time answering my queries, Sean!

Sorry for not being detailed enough in posting. I am actually doing dynamic analysis of base excitation (random vibration and transient analysis). The pre- i'm using is Patran.

I think the second method sounds more relevant to my analysis. But i'm still not so sure about that part which you say "project the nodes/elements from mating holes/ faces onto one another". i'm actually importing the model as a parasolid into the pre-, not building it up from scratch. Therefore, now i've a model of a box (or should i say case), with several components bolted down to it, and it has a cover which is also bolted down to it.

So is it possible to use "mesh matching" in this case? if so, can you pls elaborate on how can i carry this out?

Once again, thanks a lot for your time.

 

[jetmaker]

huiying,

For your problem, I would consider deleting holes, fillets, chamfers, and other small geometric features to simplify the meshing and run time. Then model the connection between parts as a simple rigid beam. Do this for the first few iterations until you have identified hotspots. This is a common approach for complex parts. Once you have solutions, you can then submodel parts, including all the detail you want.

What Sean is refering to nodal association. Begin by meshing the box, including the holes as concentric circles. Then project the nodes of the concentric circles onto the surface of the lid. Then associate those projected nodes with the surface/solid geometry of the lid. Now when you automesh the lid, it will force the associated nodes to be part of the new mesh generated. Note that automesh may have problems generating a mesh if the associated nodal pattern is not compatible with the mesh required to fit the global part geometry.

Hope this helps.

jetmaker

 

[izax1]

It depends on what you are after!
If your (or the designer) bolt design is safe, then I would say you disregard the bolt connections and model the structure as one part (piece). If you are not sure about the bolt design, I think a local (non-linear) analysis of the bolt area is the best way. The bolt design should ensure that the bolts get no bending and minimum alternating stress. If that is the case, the assumption of modelling lid and box as one piece is valid.

I am not sure if I understand the methods described above. It is important to understand bolt connections when trying to model it with FE. Bolt connections are highly non-linear with complex load patterns. You also have to remember that modeling a bolt as a rod (or bar)or with solids describing only the bolt cross section will give you a far too soft link, because the bolt is always preloaded and has zero length between the two bolted parts. As I said above, see to it that you have proper bolt connection (enough bolts, right size and preload) and model the two bolted parts as one piece.