Modelling of welded corner of shell elements

[netjack]

Dear All,
Many structures are made of plates that are welded together. How are we going to model these structures in FE. Assume that I am using shell elements. And I have 90degree corner (crosssection is L shape). I used to use same nodes at the corners of the shell elements (coincident). However, some indicate that this model is softer than real case (due to missing in-plane rot stiffness in plate elements). Is it true for shell elements too? In order to model it better, it is advised to use beam element at the corner. What is your recommandation?

netjack

 

[Tankman650]

Netjack,

It depends on what you are looking to solve and the geometry of your structure.

If you are concerned with the stress concentration at the weld, you should model the fillet weld in your model. That will give you a more accurate stress value. By ignoring the fillet weld, you stresses will be higher(conservative).

If you are not concerned with the weld stresses, ignoring the thickness of the fillet weld is no problem if the width of the weld conpared to the length of plate is very small.

Say you weld two 10" plates and use a 1/4" fillet. The ratio is .25:10. That indicates the difference of stiffness of including the weld should be insignificant to actually not using the weld thickness.

On the other hand, if your plate lengths perpendicular to the weld were 1", the stiffness of the weld will be a factor and should be considered in a model to reduce the conservative assumptions.

 

[netjack]

Thanks tankman,
I understand your point for weld radius. However, my question is general about shell elements and their behaviour at sharp corners. Assume that I have box beam modeled with shell elements. I am interested in global stress values instead of local ones. Is it enough just to use only shell elements or do i have to add some stiffness to the 4 edges.

 

netjack..
regarding your first message ,I would say that though shell elements have inplane dof(called "drilling dof",the stiffness of shell element associated with this dof is not real stiffnesss and it is of negligible value.So ,in reality,there is no "inplane rot stiffness"even in the case of shell elements.I mean the shell cant resist any inplane twisting moment.

regards.

 

[tld23]

I have posted on this befor in thread727-20838, the answer is repeated below:

It is not normal to include welds in analyses. This is because most
structures are designed to codes or standards which require nominal or
hotspot stresses. The codes then take into account the strength/weekness of the welded connections.

Most models would only require joining at the intersection to transfer load. The stresses at the intersection WILL NOT be accurate so they should not be used - they may well be very high but unrealistic. Be guided by the code on how to interpret the results or alternatively see the rererence listed below.

Niemi E; 'Stress Determination for Fatigue Analysis of Welded
Components', Abington Publishing for the IIW, 1995, ISBN 1 85573 2130.

Sometimes if the weld is large compared to the components being joined the stiffness of the weld itself needs to be accounted for. Often beams are used to add this stiffmess, the beams representiong the weld bead.

Finally the devil is in the detail and will depend on the assessment criteria that you are using. If you are doing a limit load analysis the welding residual stresses may be important. If this is a fatigue assessment the residual stresses are usually taken into account by the assessment code.

The bottom line is that you may have to try modells with and without the extra stiffening and make an assessment as to their effect

TERRY