ANNEX C FATIGUE STRENGTH ANAL YSIS
C.2.10 Calculation of hot spot stress by finite element analysis
From detailed finite element analysis of structures it may be difficult to evaluate what is “nominal stress” to be used together with the S-N curves, as some of the local stress due to a detail is accounted for in the S-N curve.
In most cases it may therefore be more convenient to use an alternative approach for calculation of fatigue damage when local stresses are obtained from finite element analysis.
It is realised that it is difficult to calculate the notch stress at a weld due to a significant scatter in local weld geometry and different types of imperfections. This scatter is normally more efficiently accounted for by use of an appropriate S-N curve. In this respect it should also be mentioned that the weld toe region has to be modelled with a radius in order to obtain reliable results for the notch stress.
If a corner detail with zero radius is modelled, the calculated stress will approach infinity as the element size is decreased to zero. The modelling of a relevant radius requires a very fine element
mesh, increasing the size of the computer model. In addition, a proper radius to be used for the analysis will likely be a matter for discussion.
Hence, for design analysis a simplified numerical procedure is used in order to reduce the demand for large fine mesh models for the calculation of SCF factors:
• The stress concentration or the notch factor due to the weld itself is included in the S-N curve to be used, the D-curve.
• The stress concentration due to the geometry effect of the actual detail is calculated by means of a fine mesh model using shell elements (or solid elements), resulting in a geometric SCF factor.
This procedure is denoted the hot spot method.
It is important to have a continuous and not too steep, change in the density of the element mesh in the areas where the hot spot stresses are to be analysed.
The geometry of the elements should be evaluated carefully in order to avoid errors due to
deformed elements (for example corner angles between 60° and 120° and length/breadth ratio less than 5).
The size of the model should be so large that the calculated results are not significantly affected by assumptions made for boundary conditions and application of loads.
C.2.10.2 Tubular joints
The stress range at the hot spot of tubular joints should be combined with the T-curve.
Analysis based on thick shell elements may be used. In this case, the weld is not included in the model. The hot spot stress may be determined as for welded connections.
More reliable results are obtained by including the weld in the model. This implies use of three- dimensional elements. Here the Gaussian points may be placed 0.1 rt from the weld toe (r = radius of considered tubular and t = thickness). The stress at this point may be used directly in the fatigue assessment.
C.2.10.3 Welded connections other than tubular joints
The stress range at the hot spot of welded connections should be combined with S-N curve D. The C-curve may be used if machining of the weld surface to the base material is performed. Then the machining has to be performed such that the local stress concentration due to the weld is removed.
The aim of the finite element analysis is not normally to calculate directly the notch stress at a detail, but to calculate the geometric stress distribution in the region at the hot spot such that these stresses can be used as a basis for derivation of stress concentration factors. Reference is made to Figure C.2-21 as an example showing the stress distribution in front of an attachment (A-B) welded to a plate with thickness t. The notch stress is due to the presence of the attachment and the weld.
The aim of the finite element analysis is to calculate the stress at the weld toe (hot spot) due to the presence of the attachment, denoted geometric stress, σhot spot. The stress concentration factor due to this geometry effect is defined as,
inal nom
spot hot
σ
SCF= σ (C.2.20)
Annex C Rev. 1, December 1998 Thus the main emphasis of the finite element analysis is to make a model that will give stresses with sufficient accuracy at a region outside that effected by the weld. The model should have a fine mesh for extrapolation of stresses back to the weld toe in order to ensure a sufficiently accurate
calculation of SCF.
FEM stress concentration models are generally very sensitive to element type and mesh size. By decreasing the element size the FEM stresses at discontinuities will approach infinity. It is therefore necessary to set a lower bound for element size and use an extrapolation procedure to the hot spot to have a uniform basis for comparison of results from different computer programs and users. On the other hand, in order to pick up the geometric stress increase properly, it is important that the stress reference points in t/2 and 3t/2 (see Figure C.2-21) are not inside the same element. This implies that element sizes of the order of the plate thickness are to be used for the modelling. If solid modelling is used, the element size in way of the hot spot may have to be reduced to half the plate thickness in case the overall geometry of the weld is included in the model representation.
Element stresses are normally derived at the gaussian integration points. Depending on element type it may be necessary to perform several extrapolations in order to determine the stress at the location representing the weld toe. In order to preserve the information of the direction of principal stresses at the hot spot, component stresses are to be used for the extrapolation. When shell elements are used for the modelling and the overall geometry of the weld is not included in the model, the extrapolation shall be performed to the element intersection lines. If the (overall) weld geometry is included in the model, the extrapolation is related to the weld toe as shown in Figure C.2-21. The stresses are first extrapolated from the gaussian integration points to the plate surface. A further extrapolation to the line A - B is then conducted. The final extrapolation of component stresses is carried out as a linear extrapolation of surface stresses along line A - B at a distance t/2 and 3t/2 from either the weld toe, or alternatively the element intersection line (where t denotes the plate thickness). Having determined the extrapolated stress components at the hot spot, the principal stresses are to be calculated and used for the fatigue evaluation.
Some comments on element size is given in the Commentary.
It is recommended to perform a verification of the procedure on a detail that is S-N classified and that is similar in geometry and loading to that is going to be analysed. If the verification analysis comes out with a different SCF (SCFVerification) than that inherent the S-N detail, ref. e.g. Table C.2-1, a resulting stress concentration factor can be calculated as
on Verificati
1 C.2 Table N S Analysis SCF SCF SCF
SCF= ⋅ − −
where
SCFS-N Table C.2-1 = Stress concentration in the S-N detail as derived by the hot spot method, see Table C.2-1.
SCFAnalysis = Stress concentration factor for the analysed detail.
It should be noted that the hot spot concept can not be used for fatigue cracks starting from the weld root of fillet/partial penetration welds.
Figure C.2-21 Stress distribution at an attachment and extrapolation of stresses
Annex C Rev. 1, December 1998
Figure C.2-22 Examples of modelling