Fatigue Analysis of Welded Connections in Solidworks FEA 1

[toothless48]

Hello all,

I have been tasked with modeling a pair of parallel I-beams, which together support a steel plate that rests between their flanges. Since, ultimately, a bus will be driven over the steel plate, the I-beams are not sufficiently stiff to support the plate in their unmodified state, they will have to be made stiffer, potentially through the use of perpendicular gusset plates. This assembly must pass for infinite life under the AISC fatigue standards.

When I modeled the gusset plates and ran an FEA analysis, the model presented stress concentrations around the fillet weld of the gussets (that material is in bending, like a "pooling" effect in the flange between plates, which is to be expected. However, the stresses that pop up are very high, up to 25 ksi.

My question is, since the AISC fatigue limits are supposed to be for purely elastic analysis (without stress concentration factors), and the FEA accounts for stress concentrations, how should I interpret my results? I do not want to simply hand wave the stresses away, because they do not seem like "typical" concentrations that would come up in normal AISC applications. Should I be holding the FEA results to the AISC numbers? That seems like over-engineering, and may be costly.

My secondary question is, when looking for these stresses in welds that are hard to hand calculate, can I just model the weld as a separate component (like a path extrude), and bond it to the two pieces that I am trying to join?

Many thanks from a lost intern.

Mike
Oceaneering Entertainment Systems

 

[rickfischer51]

Ignore the stresses. Some of them are artifacts of the model, and the others are accounted for in the code allowables. Get nodal force and moment reactions from your finite element solution at the edges of the stiffeners, put them in a spreadsheet, and calculate weld stresses per your code of choice.

You do not hold FEA results to the AISC numbers. You compare stresses calculated per the AISC code to the AISC numbers.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[toothless48]

Thanks a lot, rick, I appreciate the advice.

 

[corus]

Fatigue evaluation is normally carried out on nominal stresses, ie. away from stress concentrations. You could use the FE results but plot the stresses up to the welds and 'linearize' them to remove that peak stress component due to the stress concentration effect.

 

[wnmascare]

Did you input Young´s modulus and Poisson ratio for the welds? If so, what were the values you inputted?

Classical literature on machine design, like Shigley, Norton and Juvinnal, say that the weld material is usually the stiffer material of the joint. Thus, in an attempt to account for this peculiarity in the numerical
model, I have adopted a higher Young’s modulus for the welds. In this case, I usually use E = 530.3 GPa and v = 0.2, which were values taken from "Chee, N. C.;Bakar, A. R. A. Finite Element Modeling of Arc Welded Joints, Jurnal Mekanikal, n° 23, June/2007".

What do you guys usually do when you model welds? Do you input a larger Young´s modulus for the welds or just give them the same regular Young´s usually used for steels?

Thanks in advance!

 

[rickfischer51]

Where in Shigley does he say that? I've seen authors say the weld is stronger, but never stiffer. How could it be stiffer? Its the same material, with I believe a similar crystal structure.

I dont model welds or take stresses from welds, for the reasons given above. Any given code has a method for calculating weld stress and a method for determining the weld allowable. The methods were developed as part of a system. If you mix and match stresses and allowables, you're looking for trouble.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[marty007]

There is a paper written for the International Institute of Welding (IIW) that discusses this local area when it comes to determining local (hot spot) stress that is titled:
RECOMMENDATIONS FOR FATIGUE DESIGN OF WELDED JOINTS AND COMPONENTS

Essentially it talks about extrapolating the stresses either linearly or quadraticly from a certain distance away from the weld.

Cheers.

 

[BlasMolero]

Hello,
In this example a welded joint is modelled by Shell plate elements to perform a fatigue analysis in the welded joint. To meet the FKM standards (which are identical to IIW guideline) for fatigue calculation of welds according to the hot spot concept the mesh has to be created in a special way. The lines where the nodes are located are parallel and in a definite distance to the weld toe. The stress tensor needed for weld calculation is automatically created by stress tensor extrapolation.

http://youtu.be/T_XSmx9GpmA?list=UUxNPbMZyg1T4V2KaHRB8_JQ

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[wnmascare]

Thank you guys for your prompt replies.

Actually, I don´t ask for stress-strain calculation in the welds, when I include them in my FEM models. But, I need to input their basic mechanical properties, like Young´s modulus and Poisson ratio. Because the welds are the strongest material of the joint, I´ve always used a higher Young´s modulus, based on the reference I mentioned previously.

Best regards!