VON MISSES STRESS 5

[Dasboot]

THE VON MISSES STRESS IN A PLATE IS 12 KSI.
FOR A36 STEEL IS MY SAFETY FACTOR 36/12 = 3
OR 58/12 = 4.8
IS VON MISS BASED ON YIELD OR ULTIMATE ?

 

[Andries]

Hi Dasboot,

The Von Mises stress is not based on yield or ultimate stresses, which are material properties. The Von Mises stress is purely a function of the stress field at a point in the material. It is equal to the octahedral effective stress and is used to characterise failure in ductile materials, i.e. if the VM stress is greater than the material yield stress plastic strain is assumed to occur. See books like Dowling: Mechanical Behavior of Materials.

Andries

 

[rb1957]

as above von mises is "just" a combination of stress components.

it is better to use it as a limit stress, since it is based on elastic theory.

but from your post if your steel as a yield of 36 ksi and ftu of 58 ksi, then you have a limit (or proof load) MS = 2 (or RF = 3) and an ultimate MS of 3.8 (or RF of 4.8).

 

[cloa]

Use the minimum amount of uppercase in any post in any forum (including

http://www.eng-tips.com)

that you use. Can seem like shouting.

 

[JoshPlumSE]

Von Mises is usually compared to yield....

Also, keep in mind that for A36, the minimum yield is 36 ksi. You might be able to demonstrate (through testing) that the ACTUAL yield is considerably higher. I'm not sure how much higher it would be for plate, but for rolled shapes it is generally expected to be about 54 ksi!!

 

[Dasboot]

Your expert replies are much appreciated. I am a 'Port Engineer' (run/maintenance of boats) not Structural. The design engineer gave us a structural detail on a small deck pedestal. One of the gusset is showing a Principal stress of 14.027 ksi at the very tip of the gusset (screen dump attached). The maximum allowable stress on the specs is 12.8 ksi. The designer said it is ok since the Von Mises is only 12.783 ksi and just the very tip of the gusset is above the 12.8 allowed. Do we need to request thicker plates ?

 

[Andries]

Dasboot,

I wouldn't worry too much if the material is ductile. What you could ask the structural engineer is to show that the gusset will not buckle if the free edge is under compression.

Andries

 

[loki3000]

if the material is ordinary structural steel, it's ok, as it will simply deform at the tip and redistribute the stresses (if the spike is in the plastic zone at all...).

 

[rb1957]

i see this type of problem/question a lot. too often users latch onto the highest peak stress like a pit-bull, but there is some reality that bluntens these peaks.

it looks like a TET mesh ... TET4s are known to be overly stiff, maybe remesh with TET10s ?

it also looks like a single element centroid stress. i'd like to see a section through the web, to see if it is highly localised (and so redistributed by yielding) all trhu thickness (which reduces the redistribution).

if you're relying on von Mises (which is relying on the thru-thickness stress), how many elements do you have thru the thickness ? 3? (the pic looks like 1).

comments about the free edge of the web being in compression are good.

 

[EngAddict]

For a start who knows what the actual stress is with such coarse mesh.. probably much higher.

Is there fatigue requirements, as is usually the case on ships? This would mean the peak stress will need to be considered for cyclic failure using ABS or similar.

What about a check of the welds? The model assumes full penetration but most of the time gussets are only fillet welded. This will also be a critical concern if fatigue is an issue. Did they also supply hand calculations for the welds?

Peak stress aside, you also need to consider stress classification. Highly localised stress can 'shakedown' during the first few applications of load though local yielding. However, it cannot be known if this is the case or if it is just peak stress because the mesh is too coarse.

 

[Dasboot]

EngAddict,
My boss thought the mesh was too coarse also. What would be the 'optimum' size of the elements for these plates. The designer said the elements are 3x3x3" on average. We will ask him to remesh the gussets and 1" base plate. Should we have the pipe remeshed smaller also ?

 

[EngAddict]

I could state some really rough rules for the number of elements but they depend a lot on the type of element used and the FEA package.

Ultimately all you have to do is ask them to show you proof of convergence of their results. This will require them to refine their mesh until the stress stops increasing (assuming no singularities in the region where the measurements are taken).

 

[rb1957]

at a minimum remesh cloes to the hot spot.

if that mesh is 3" x 3", this thing is much bigger than i thought it was.

be aware, remeshing is certain to increase the peak stress, albeit over a smaller area, but this is FE detecting something which wasn't detectable with hand calc methods. convince yourself that the high stress is very localised and in the real world there'd be a tiny amount of plasticity.

if the gusset is welded, what are the properties post-welding ? maybe that's why you have such a low allowable ??

if you're still worried, you could test it later ??