Stress assessments

Go to content

Stress assessments

femdesigner
Published by James G. in general · 30 May 2024
Ok so you have results but are they showing the product is ok or not? Again this post relies heavily on pressure vessel design codes, which tend to be the most advanced when dealing with FE results. 'Codes' is hereafter shorthand for 'design codes' rather than 'FE codes'.

Simulation of known results for future prediction
For some products you have an existing design that you know works - possibly by testing or by use - and you want a redesign to reduce a known problem - eg cracking after a certain lifespan, reduce weight, cost etc. In that case it is easy to model the existing part and compare overall stresses with any new design so if stress is less - especially in the area of concern - then your new design is better and vice-versa. This is how pistons are designed. Sometimes there is just no suitable design code for your part/assembly so you have to rely on early tests and then show that you can identify the the high stressed regions by FEA, which gives confidence in future designs.

Elastic stress linearisation and categorisation
For a new product which is especially large and loaded in a way that may be dangerous for bystanders you probably have to do a bona-fide, documented stress assessment. Traditionally stress assessments were based on stress linearisation. We often expect to see linear stresses through a thickness, eg average hoop stress = pressure x radius / thickness for a thin cylinder, average stress = force/area, bending stress = 6 x moment / thickness-squared. Finite element results though usually include stress concentrations at sudden changes of geometry and these can be removed by linearising the individual component stresses into membrane and bending equivalents, rotated along a stress line, converted into principal stresses and finding an equivalent stress or stress range from the Tresca or von-Mises yield criterion. This was a quick and dirty method to avoid doing plastic analysis when computers were less powerful than now but it is still used (see EN13445, Annex C or ASME VIII division 2, part 5).

When this method was first conceived all FE models were in 2D or 2D-axisymmetric where this technique was relatively easy to use and logical; there was an issue dealing with shear stresses which are parabolic through a thickness rather than linear but this could be handled. The larger problem was assessing what was a Primary (load-limited) or Secondary (displacement-limited) stress because they were subject to different stress limits and the FE results did not separate these out for you. With the advent of 3D models the principal difficulty is finding a line which could be regarded as an effective 2D section. Moreover you only have a line so how do you know which rotation angle around it is correct for stress rotations? Strictly-speaking it should be a plane that is linearised but that is highly impractical. Different users can easily produce different assessments. And of course sometimes a linear stress is not to be expected through a section, eg in thick cylinders.

Therefore stress linearisation is not recommended for 3D parts - such as those prepared from a solid model. Instead we should preferentially use plastic limit analysis (see EN13445, Annex B or ASME VIII division 2, part 5) which is discussed in the following paragraph. Stress linearisation has become more used than previously for fatigue analysis due to fatigue curves now containing stress concentrations at welds and this will be discussed in a future article. There is also the question of placing a limit on low-cycle fatigue (plasticity on both loading and unloading phases of a cycle) and ratchetting (runaway growth from cyclic plastic srain) which are very difficult to accurately simulate in plastic analysis. In both cases, elastic stress assessment by stress linearisation may be a viable alternative. This will also be dealt with in a later article.

Plastic limit/strain analysis
Limit analysis uses the elastic-perfectly-plastic material model with small strains. Current design codes still prefer ths model because of the basic inadequacy of kinematic hardening models for cyclic loading (discussed here). The method is still relatively simple but takes longer to run. The upside is that there is almost no subjectivity so you can set it and forget it and get a fail/pass answer at the end. The object is to find the collapse load. That is, if plasticity goes from one side to the other of a thin part then it will collapse and this will happen at a certain load. You then place a safety factor on this load - typically 1.5 and that will be the maximum allowable working load.

This method is too simplistic for a part with multiple combined loads and also requires multiple runs to find the load just prior to collapse so both EN13445 and ASME have allowed the use of partial safety factors which factor-up the applied loads rather than factor-down the resultant limit load and if the plastic region has not extended through the thickness the part has deemed to have passed the code. There is also a plastic strain limit which is simply 5% in EN13445 but found by an equation in ASME. Testing has shown that pipes will initiate cracks at around 9% plastic strain which may lead to fast fracture long before the collapse load is reached.

The ASME method puts all the safety factors on the loads while EN13445 splits them between the loads and the yield stress. There is also a further reduction in EN13445 of 0.866 on the yield stress to allow a Tresca-style limit with a von-Mises-based plastic flow rule (ie most of them). For a material with an unclear elastic limit a proof stress is acceptable (0.2% for ferritic steels, 1% for austenitic steels).



Femdesigner Ltd
840 Ibis Court Centre Pk
Warrington, UK


Back to content