different plate thickness modelling advice

[mech_eng_p]

Hello,

Sometimes I am struggling with element sizes of finite element models, especially when the plate thicknesses vary a lot.

As an example i added a attachment.
A plate, thickness 60mm, is welded to a pipe (diameter=200mm, wall thickness is 12mm).

I chose element size 15mm, because of other connections (not visible)

The pipe will be connected to the plate by a double sided filled weld.

questions:
1) when the thickness of the plate is 60mm and the element size is 15mm. the plate "over-lapses" 2 full elements of the pipe. Is this advised?
2) the plate will be welded with filled weld. Would a solution be to disconnect the plate from the pipe and add rigid elements to the location of the filled weld?

3) Is there any advice to make a nice analysis of this situation?

Hope somebody could help me out.

Thanks!

 

[rb1957]

if you're modelling with shells you have a small problem. I'd use a plain strain element for the very thick situation, or model the thickness with several elements (parallel plates). Or model the thick plate as 3D solids. Getting correct results of the interface would be tricky with a single plate element for the thick plate.

another day in paradise, or is paradise one day closer ?

 

[NRP99]

As rb1957 says, I would also advise you to use 3D solid elements rather than 2D-shell elements for getting accurate intersection stresses. Shell elements are advised only for thin sections where the ratio of pipe diameter/thickness d/t>=20 and for flat plate if t/b< 20, where b is smallest side. Plane strain elements can be used. But if you have assembly of different orientation parts, this approach also is not useful. Besides, to capture bending effects of the plate/pipe/vessel properly you need sufficient no of elements divisions along the thickness.

1) Not advised. See above. For more info check-

https://caeai.com/blog/understanding-and-using-shell-element-results-part-i

2) You can constrain the pipe without modelling plate but at the sacrifice of the flexibility of junction. As a result stresses will be higher at that location than with plate model.
3)See above.

 

[mech_eng_p]

Thank you RB1957!
Solid elements is indeed an option.
How would you suggest to connect the multiple -30- thick plates with eachother? RBE2?

I know that getting proper results is quite tricky. That's why I asked the question overhere

Also Thanks NRP99.
If you are talking about the ratio for plates: t/b with b=smallest side. Is b the element size or plate size?

I never used plane strain elements. I will look into that. How would you advice to connect this element to the weld location of the pipe? 2 RBE2's?


I think I will go for the solid mesh for the 60mm thick plate and rbe2 connection at the filled weld to the pipe.
Thanks so far!

 

[rb1957]

"I think I will go for the solid mesh for the 60mm thick plate and rbe2 connection at the filled weld to the pipe."

that sounds like a plan ... remember to link all freedoms (3D elements only have translation but the plate has all 6).

another day in paradise, or is paradise one day closer ?

 

[A-Run]

Hi Mech_eng_p,

"How would you suggest to connect the multiple -30- thick plates with eachother? RBE2?"
In "LS-Dyna", I would use "node to surface tied" contacts to "weld" the plate to the tube. If you choose the nodes of the solid plate (I agree with solid representation) as slaves to the master surface of the tube, you will correctly capture all DOFs of the plate. However, if you choose to sit shell nodes to solid (in some other area of your model may be), make sure to select correct type of contact formulation to take into account all DOFs of slave shells (*Contact_.._Shell_Edge_to_Surface). This is as per the suggestion from rb1957.

Alternatively, you can choose to create mesh so that the solid plate nodes are shared with the shell tube in-order to connect them.

PS: Be sure to check the documentation of the solver you are using to find out how many through thickness elements you need in your solid plate to get correct bending behavior. In LS-Dyna, ideally it is 3 elements through thickness for hexa elements with ELFORM 2.


Thanks,