Best way to mesh large surface with small holes 2

[ecFem]

Hello,

I would like to start a discussion about the best way (mesh quality vs number of elements vs results accuracy) to mesh a large plate with a lot of small holes.

The thing is that I have a large plate (2000 [mm] x 1350 [mm]) which contains a lot of small holes (diameter 3.2 [mm], see image below).

If I use 10 [mm] elements in order to avoid having a small element size and thus, hundreds of thousands of elements, the mesh is really awful.
Even with 5 [mm] elements this happens and the amount of elements is considerably larger. Worth is mentioning that what I showed in the image is just a part of the model; therefore, I cannot put as many elements as I want.

So I said okay, I don't consider the holes, and then I take the position of the center of the holes and I create RBE3 + BEAM elements. The thing is that there is no API for doing it and it will take me a lot of time to do it, and I would have to use only beams to connect the elements, without the possibility of using a spider + beam representation of the fastener.

Worth is mentioning that the idea of using contact is not applicable in my model, I must represent the fasteners.

My question is then open to discussion, experience and suggestions : What is the best trade off in this case ? What would you do ?

Do you have / know any API for doing it ?

Thanks in advance !

Cordially,
EC

 

[SWComposites]

Noooooooooo!!!!!!!!!!

Do not model the fastener holes. Just no. Its not needed, results in rubbish stresses at the holes, is a pain, etc.

You don't need RBE3's if you simply model the fastener locations with a single node. Then you just need to connect the coincident nodes with CBUSH elements (assuming you are using NASTRAN). And the easiest way to do it (assuming you have coincident nodes on the attached members, though you can also do if the nodes are not exactly coincident if careful) is to make a group of all of the nodes at fastener locations, export those nodes to Excel, sort the nodes by locations, then the two coincident nodes are in adjacent rows, then create a column to generate the CBUSH elements using Excel text string commands, then copy/paste/export those CBUSH elements back into the model.

Then you can use the CBUSH loads output to analyze the bolted connections.

 

[rb1957]

please don't model every single fastener ! It looks like you have a large single piece of panel with several stiffeners and such supporting. Mesh that, in as much detail as you like. Fastener forces should (in this type of structure) come from the element results ... shear flow along an edge divided by number of fasteners.

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[SWComposites]

rb, yes, that is a good approach but requires thinking ....... sigh .......

 

[rb1957]

yeah, I'm olde school ...

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[ecFem]

Thank you both for your answers ! They were really useful.

Cordially,
EC