FEA Stresses - Stress Concentration

[strainstress]

Hi,

I am trying to figure whether a 14Ga SST sheet can support the weight of a large heating element. I modeled the sheet with Shell element and the heating element as beam element (See attached) and connected the shell and beam at a point.

The gravity load on the heating element creates and point moment at the shell resulting in high concentrated singular stresses. Refining the mesh keeps increasing the maximum stress. I understand that this is due to stress singularity of a point load.

My question is : Given that the elastic stresses are unrealistic and I cannot perform a plasticity analysis, what option do I have to verify the design ? How do I interpret the elastic results with singularity ?

Thanks,

StrainStress

Attachements :

http://files.engineering.com/getfil...5ffd-4561-b3e0-cd87dde570f5&file=Close-Up.bmp

http://files.engineering.com/getfil...d2-9070-a21f30639f40&file=Heating_Element.bmp

http://files.engineering.com/getfil...f-83089e9940d2&file=Von_Mises_Stress_Plot.bmp

 

[rb1957]

you have local stress peaks as a result of a point load being applied.

you could use the element average stress, which will blunt the peak, and support the local attachment with some hand calcs ... what's distributing the load in the real world ? how's the plate reacting this loading ?

Quando Omni Flunkus Moritati

 

[strainstress]

Thanks rb1957,

Element Average Stress too increases as the mesh density is increased. In that case how do I decide which mesh density is acceptable.

In the real world, there will be some plasticity to redistribute the load, but without the plastic analysis, how do I figure how much plastic strain will be developed in the plate, to check for it acceptability.

"Support the local attachement with some hand calcs" ....Can you point to any reference which talks about concentrated moment on thin plates ?

Thanks for your help.

 

[rb1957]

"how do I decide which mesh density is acceptable" ... one that gives an answer you can accept and believe !

there's no point analyzing plastic stresses from a linear FEA. in the real world there'll be a washer and some such distributing the load into the plate. stresses at the edge of the washer should be elastic, this is as close as i'd go to the loading point in the FEA.

inside this i'd use hand calcs, for example shear stress through the thickness around the perimeter of the washer. i expect that the out-of-plane load is being applied from the far side, ie pulling through the thickness, rather than a tension "pressure" being applied to the near face.

Quando Omni Flunkus Moritati

 

[jhardy1]

There's no point in refining your plate mesh down to mm-scale elements to try to resolve stress singularities, if the plate itself is several mm thick (they're formulated for thin plate theory, don't forget!), and if the real physical features are comparable to (or larger than) the mesh size.

E.g. you can't expect thin-plate elements to give you meaningful stresses down to mm-scale, if you are going to model the loads and restraints as node point loads, and the physical connections between the components are comparable to or bigger than the plate elements themselves.

http://julianh72.blogspot.com