Simulation of fillet-weld "toe" with specific weld features

2017 August update -- convergence investigated - significant finding(s)

(14 August 2017)
"Convergence" of these models has now been tested.

If you want to know about stress concentrations around

you do need to know what the convergence-tested outcomes are.

Jumping straight to the findings: graph of outcomes , as a "PDF".

Back when I did these original simulations in May 2016, it was early in "playing with" Finite Element Analysis modelling, finding whether I could make it work for me with practicable effort (yes), using the "restricted" "free trial" version of LisaFEA.

A recent query came to me about a completely different matter, but involving stress concentrations at geometric features.
The quickest way to illustrate the concepts for that case was to re-run these simulations at increasing refinements, and show their outcomes.

This allowed me to inspect an assertion.
For sharp stress-raising features which are of paramound engineering interest, if you Finite Element model them, the stress gets ever higher with increasing discretisation / mesh-refinement. That is, there is never "convergence". The answers do not get more similar with increasing refinement, clearly coming to a final single constant answer.

That is

The new treatment of these models, applying mesh refinement seeking convergence, is presented here: fillet-weld toe-geometry simulations with increasing mesh refinement .

Returning to original May 2016 webpage:

Re-interpret the Section "Comment on what the models show" given above information...

Welding context

The "weld toe" is where the outer face of the weld deposit meets the metal being welded. This is general to all welds. Fillet welds are described eg on Wikipedia , where the weld toe is labelled. The form of fillet welds is well presented by The Welding Institute (UK) - which mentions weld toe but does not label it.

Welds typically suffer a very low fatigue endurance - way below what a piece of metal with no welds on it would offer.
The dominating explanation was identified in 1967 [Signes, Baker, Harrison and Burdekin]. The edges of welds - the weld toes - have unfortunate fine-scale crack-like features, right at the point where the change-of-section, the shape discontinuity of the weld, is causing a stress intensification.
These toe-intrusions comprise both cold-laps over the "parent plate", plus slag inclusions in the metal at the weld edge
(conjectured to be caused by the coolness near freezing point of the weld-pool at the weld edge, causing slag inclusions to freeze in place in the "pasty" metal rather than be swept clear and ultimately rise to the weld pool surface as slag).

Toe intrusions of laps and slag inclusions with associated fatigue-cracking, identical to those shown in the Signes Baker Harrison Burdekin 1967 publication, can be seen in my work of 2011, for "standard" welding conditions.

"T" (shaped) fillet welds have particularly low fatigue endurance due to the geometric stress intensification factor of going from the parallel plate to the rising weld reaching to the side-attaching plate.

I found the 1967 Signes Baker Harrison Burdekin work when investigating why it did not always have to be so that welds had low fatigue endurance. As I was finding in my weld-and-fatigue tests.

My objectives for weld-toe situations modelled by FEA simulation were:

Toe-groove (misleadingly called "undercut") is caused by welding conditions giving high weld-pool fluidity. As I found in tests (and was to discover a few others already know), this deprecated "flaw" is associated with high fatigue-life / fatigue-endurance.

The shapes representing the three conditions will be seen in the FEA simulation programme outputs.

The FEA solution

The FEA solutions are 2-D, declaring (enforcing) plane-strain.
That is a perfect match for these simulations, as welds are long compared to the cross-section. Leaving computing resources free to discretise the cross-section well with a fine mesh. Particularly with local refinement in the region representing the weld toe.

The modelled plate upon which the fillet weld is made is 16mm thickness. Given the model has 8mm thickness from the plane-of-symmetry.

The shape of the object simulated is simplified, compared to a real T-fillet weld. The stress-field around the weld toe is a local phenomenon, so any model which passes realistic conditions to that studied region is good.
Plenty enough of the weld fillet height is represented in the solution to enable stresses to "flow" as they would beyond the weld toe, into the weld fillet.

The material properties of steel have been represented in the model: 200GPa Young's (elastic) modulus and Poisson's Ratio of 0.3.
Stating what has previously been implicit: the plate metal and weld metal have identical properties in the model, as "steel". Forming a single object of homogenous isotropic properties; whose shape and applied-loading-state determine all variations investigated. In a linear-elastic model, this homogenous property of elastic modulus and Poisson's Ratio is realistic.

The mesh strategy

The mesh shown is for the "blueprint" case.
For the other two cases, the overall mesh is the same. The local mesh modification to represent "toe intrusion" and "toe-groove" is to be seen in the subsections for those simulations.

The model applies a plane-of-symmetry in the "horizontal" "XZ" plane of the represented shape
(the "XZ" plane's dimensions are left/right and in/out of the plane of this screen in all these models).
This is seen in the "zero Z displacement" and "zero Z-axis moment" constraints placed along the lower edge of the mesh in these two images of the same mesh. These are represented by the red "cone-shaped" and "trumpet-shaped" markings, respectively.
Applied loads are shown by the green arrows, seen at the left-hand-side and right-hand-side ends of the mesh.

Applying the plane of symmetry enables modelling only half the weld; where in this case I have chosen to model only the half above the continuing plate's central plane (more loosely; "centre-line").
The geometry and stress-states are identical about the plate's central plane; giving a balanced symmetrical response to the stress-state in each half. That balance makes the "zero Z displacement and zero Z-axis moment" correctly characterise the plate's central plane.

The mesh concentrates via local refinement on the represented weld toes.

Comparability and evaluation of the three models

The images for each model are obtained at the same "zoom" - they show identically the same region.
Comparing between models, the "zoom" is about the same. That can be verified from the displayed coordinates of the highlighted node in the mesh view, which is around 2mm from the fillet-weld toe (there isn't a node at (2,0,0) for the "toe-groove" simulation - the next available node on the (x,0,0) plane is "Node 97" at (2.414,0,0)).

The modelled plate is 16mm thickness, as previously mentioned.

The applied stress in the "parent plate" - the represented plate to the right-hand-side is always "1000". Therefore the stress intensity can be evaluated by dividing the displayed stress by 1000.
eg, for the first of the three cases shown, the "as-blueprint" case; the highest stress intensity for the "Stress XX" case is 1.987X the ruling stress in the plate (1987/1000), which is seen just to the plate side of the weld toe. Please be aware that these solutions are inherently approximate - so it would be reasonable to say the highest stress intensity is "about 2.0 times the force/area stress in the plate".

The three models are each present the order

The toe-intrusion case has an additional "mesh open cracks view", intended to reveal meshing defects, but usefully showing the modelled crack in this case.

PLEASE NOTE - I have not convergence-tested these models (yet!), nor had them peer-reviewed - so they should not be taken as authoritative.

Subject to this caveat - any comment about what the simulations might show is in a final subsection after the three individual modelled cases are shown.

As-blueprint

This is the as-designed case. As if the weld had a perfect 45degree mitre and a flawless intersection, otherwise featureless, with the plate metal being welded.

Thus, it is the reference case.

Toe-intrusion

The toe-intrusion is modelled as a 0.5mm long sharp-tipped crack, intruding along the plane of the surface of the plate, at the weld toe.

Toe-groove

Toe-groove is modelled as being 0.5mm deep.
Its form is semi-circular radius. It transitions into the weld bevel at the 45degree bevel angle, at the plane of the plate surface. With these geometric constraints, this results in a toe-groove which is 2.4mm wide (reasonably realistic for such a deep obvious toe-groove).

Comment on what the models show

Subject to the previously mentioned caveat that I have not convergence-tested these models (yet!) nor had them peer-reviewed - so any comment must be tentative...

So far these simulations do not show a big reason why in real life welds with toe-groove can have very high fatigue-endurance several times higher than expected - whereas representative real welds with toe-intrusions have the reference familiar low fatigue-endurance.

Considering von Mises (deviatoric) stress; the maximum stress intensities shown, all in the weld-toe region, are:

These are not huge differences. Nor should they be trusted too much.

Setting aside the impartial scientist and engineer personality; one feels gratified that the crack-like toe-intrusion case has the highest stress intensity factor, but feel disappointed that the semi-circular toe-groove does not have the lowest stress intensity factor.

It is commonly commented about FEA that when modelling a sharp feature, the finer the mesh the higher the maximum stress intensity (it doesn't really converge well).

Stress intensities around specific local features are best evaluated according to mathematical formulae derived for these cases. Noting all work on the "Stress Intensity Factor", often given the symbol "K" in engineering literature.
For real engineering structures with complex geometries leading to stresses which can only be quantitatively evaluated by computational modeling, the "Stress Intensity Factor" is being applied upon a realistic regional stress level indicated by the FEA model (???).

In these models I've "cheated" - I've made the regional stress obvious and so easy to immediately calculate that it can be done by mental arithmetic - as the force/area stress, with forces and areas chosen to give simple numbers (stress of "1000", etc).
But that has not overcome that local stress-intensifying features are not trivially modelled (???).

So the final note is - enjoy the pictures, but leave alone any attempt to read value into them :-)

(14Aug2017 - per re-evaluation with increasing mesh-refinement - there is significant value in these simulations and their findings are known to accord with known physical / real-world behaviour)



(R. Smith, 17May2016, 14Aug2017)