D6. Understanding and analyzing the peaks (case study about steel assembly)

The results of a calculation performed on a surface finite element model (plate or shell type elements) may present stress peaks (or singularities). The presence of stress peaks is not annoying if they are located in areas out of interest with respect to the objectives of the study and if their presence is justified.

It should be kept in mind that a stress peak, i.e. a very high stress, must concern two or three nodes, or even a single node at most (but the structure may nevertheless present several stress peaks).

When dimensioning an assembly of plates which are welded together (metal bridge box at a support for example), the realization of a finite element model is necessary to correctly take into account the diffusion of stresses. And of course, from the same model, the stresses in the plates can be extracted to proceed to the dimensioning of the assembly of these plates.

Nevertheless, the general idea will remain to always keep a critical eye on the results obtained. They will have to be analyzed properly before they can be considered reliable with regard to the objectives of the study carried out.

This analysis of the reliability of the results often comes up against the interpretation of the possible presence of stress peaks.

The purpose of this paragraph is to give clues to help the modeler who is responsible for assessing whether or not a stress peak is a problem.

The appearance of stress peaks can have different origins, of which the main ones are:

the presence or omission of details such as connecting fillet;
meshing inconsistencies;
setting up loads and boundary conditions.

D.6.1 Modeling – Details

Before embarking on the surface modeling of a metal plate assembly, it is essential to know and master the software's CAD tools and its meshing capabilities.

It is customary when creating geometry to neglect certain details. Two cases among others:

Connecting fillets - if the connecting fillets of an opening in the web of a beam are not shown, stress concentrations will inevitably be all the higher that the web loads are important and the angle is acute (case of non-perpendicular opening edges);

Note 1: The modeling of a connecting fillet will no longer create a stress peak, but a simple stress concentration. Stress concentration charts are based on this type of modeling.

Note 2: In fracture mechanics, the crack model characterized by a zero angle is a special case used to model crack propagation which is based on the notion of stress intensity factor.

Transverse stiffeners - the main beams of a bridge require transverse stiffeners at the support zones. The modeling of these stiffeners is often necessary in view of the forces that can transit in this zone and locally stress the web. According to the bridge’s rules, these stiffeners have a particular geometry and too often this geometry is oversimplified during the modeling process;

Real geometry / Simplified geometry

The stress transition may not be affected, but the mesh of the stiffener will have to be controlled so as not to end up with degenerated elements that can create singularities. And at the tip of the stiffener, a stress peak may appear which in case of misinterpretation may lead to false conclusions. See also § C.3;

Details such as connecting fillets, mouse holes, chamfers, etc. may therefore not be modeled if they are located outside an area of interest. The time spent modeling details may not be negligible, but if the objective of the simulation is to calculate a stress or a deformation in an area with such details, it is essential to model them and, moreover, to associate a representative mesh to them.

Non-representative mesh / Representative mesh

In the absence of detailed blueprints of the constructive details to be modeled, we will rely on the constructive provisions and bridges rules, which, in terms of metal assemblies (connecting fillets, local plates, stiffeners, etc.), provide a basis generally leading to a satisfactory diffusion of efforts. For example, the Commission for the standardization of metallic and mixed construction (CNC2M) recommendations for the dimensioning of steel beams with openings in the web according to NF EN 1993 specify that, for a rectangular opening, the radius of the connecting fillets must be bigger or equal to twice the web thickness without being smaller than 15 mm, or that an isolated opening with a maximum dimension less than 10% of the web height of the beam is not considered significant (this opening must nevertheless be taken into account when checking the section).

In some cases, the consideration of details cannot be neglected (see also § C.2.2). For example, during a fatigue verification of the connections of an orthotropic slab, simplified calculation models described in the design regulations may be used. However, these models are safe and, if the fatigue strength is not justified with these simplified approaches, two possibilities are available for the designer:

either modify the geometry of the assembled parts, which is often difficult in the execution phase;
or perform a more refined calculation on a plate finite element model.

In order to take into account the vehicle traffic effects (longitudinal and transverse effects, influence lines), it may be necessary to model a fairly substantial length of the structure. On the other hand, the detail modeling zone may be limited.

D.6.2 Modeling - Surface model creation and meshing

It is also important to have a good understanding of the software's meshing possibilities. Most types of software can automatically mesh a plate assembly.

The user's intervention can then be limited to the definition of a few parameters such as the average size of the elements or their shape (quadrangular, triangular). It is better, however, to be able to control the mesh by choosing the order of the surfaces to be meshed, by imposing finer mesh sizes in some zones, in order to avoid the presence of degenerated elements.

Example of degenerated mesh

In a complex assembly, due to the shape and number of parts assembled, the risk of mesh inconsistencies is high. To reduce this risk, several points should be considered, as a reminder:

The analysis and the perception of the mechanics of materials operation of the assembly by the engineer prior to the modeling are strongly recommended. Some reinforcements and details that have only a very localized effect on the overall behavior of the assembly can be omitted, thus reducing the number of interfaces between plates;
To avoid mesh discontinuities, all plate intersections must appear. For example, in the case of modeling an I-beam, each of the flanges will appear composed of two identical surfaces on both sides of the web. At the intersection of each flange with the web, a single line common to all three surfaces (the two surfaces constituting the flange and the web surface) must be present;

Elementary surface decomposition of an I-beam

do not hesitate to decompose the extended surfaces into several quadrangular shaped surfaces, the meshing will be facilitated as well as for example the application of loads like as pressures;

The work structure can present panels with a deformed geometry. The software can allow the creation of deformed surfaces, within a certain limit. Therefore, depending on the deformation, the initial panel will have to be decomposed into several sub-panels (the common boundary between two sub-panels being made up of the same entities). During the meshing process, elements resting on a deformed surface will also show warping. Depending on the software, the warping limit allowed for a CAD surface (on which the finite element mesh will be supported) may be different from that allowed for finite elements. In any case, it is always possible to approximate warped elements using successive triangular flat surfaces.

Example of panels with deformed surfaces

The assembly to be modeled may have cylindrical tube intersections. If during meshing elements without a middle node (4 node elements) are used, the mesh will present facets; the larger the size of the elements, the larger the size of these facets. This "facetization" can therefore be reduced by increasing the number of elements. The use of mid-knot elements can also be a good solution, provided that the software used allows the mid-node elements to follow the curvature of the CAD surface (or CAD line).
if a tube is connected to a plate, pay attention at the connection, to the compatibility of the types of elements used (for example connection of elements with 4 and 8 nodes). In some cases, discontinuities in the results may occur (see § C.6.3);

D.6.3 Modeling - Loading and boundary conditions

One of the frequent causes of the appearance of stress peaks is the presence of point loads or point blockages.

If a point load (respectively a point support) put in place is outside the area of interest, the presence of a stress peak is not annoying. On the other hand, if it is in the area of interest, rather than a point force, it is better to apply the force on several nodes (respectively block several nodes).

As described in the previous chapters, in reality, point forces and point supports do not make physical sense (note, however, that in a wire beam model, point supports do not create peaks).

Practical application:

Let us consider a HEB beam modeled in plate elements. A stress peak would appear, if the stress torsor in a section was applied at a node. It is better to get closer to reality, by transforming the stress torsor into normal and tangent stresses (as linear forces, if any) and proceed as follows:

the normal effort will be distributed over all the nodes of the end section;
the shear force will be distributed over all the nodes of the web of the end section;
the moment will be decomposed into two forces distributed over all the nodes of the two flanges of the end section.

Normal force / Shear force / Bending moment

The same will be done to model the beam supports. Let us consider the two following cases:

bi-articulated floor beam (end web angle connection) subjected to a distributed load. We will consider two cases differing by the boundary conditions; `

1st case: at each of the ends, installation of a point vertical blocking (the transversal blocking of two nodes is carried out to stabilize the beam in rotation around its axis).

1st case - boundary conditions/longitudinal iso-stresses (in MPa) - the peak stress area is circled

2nd case: in each extremity the vertical and transversal blocking of the nodes of a web part is performed in order to get closer to reality.

2nd case - boundary conditions / longitudinal iso-stresses (in MPa)

The stress peaks appearing in the 1st case are thus due to the presence of a point nodal reaction. However, by observing the results only on the central part of the beam, we find identical results to those of the 2nd case.

1st case - central part - longitudinal iso-stresses (in MPa)

bi-supported beam (supports under the bottom flange) subjected to a distributed load. First, only the beam (type H) is modeled and boundary conditions are applied such that, near each of the two ends, the nodes of the bottom flange are blocked in the vertical direction.

Case without stiffeners - boundary conditions / Longitudinal Iso-stresses (in MPa)

Case without stiffeners - vertical iso-stresses (in MPa)

Stress peaks appear at the lower flange/web intersection despite the fact that vertical blocking was performed on several nodes. The problem here is more of a design problem. It is common practice to install transverse stiffeners perpendicularly to the supports (see design regulations for the transverse force resistance of the beam web and checks for local buckling). If we take the model by adding transverse stiffeners perpendicularly the supports, the peak stresses perpendicular to the supports disappear.

Case with stiffeners - boundary conditions / longitudinal iso-stresses (in MPa)

The stress peaks appearing in the absence of stiffeners are therefore due to a design problem. However, if we observe the results only on the central part of the beam, we find similar results to the case with stiffeners.

Cases without stiffeners - central part - longitudinal iso-stresses (in MPa)

D.6.4 Results analysis - Model validation

Once the modeling is complete, having best followed the advice given above, the calculation is executed. It is necessary to carefully analyze all the messages that can be generated by the software. Usually, an error message will block the solver, unlike warning messages, which must be carefully analyzed and interpreted. It is recommended not to ignore these messages without having carefully evaluated the possible consequences, even if it means calling the editor's hotline.

It is important to understand the possibilities offered by the software for the display and the types of results. The following is a non-exhaustive list of parameters that should be considered:

the coordinate system in which efforts and moments, displacements or constraints are displayed: is it the global coordinate system of the model, local coordinate system of the elements, nodal coordinate system?
Sign conventions for efforts and stresses;
the convention used by the software for naming forces and moments: for example, some software calls My the moment around the Y axis, while for others it corresponds to the moment parallel to the Y direction. This is particularly true when using torsors supplied by a third party;
the different stresses: directional stresses, principal stresses, Von Mises equivalent stresses;
the type of stresses displayed and how they are calculated: node or element stresses, mean surface or facesheet stresses;
the possibilities of stress extraction at Gauss points;
the relevance of the stress display scale, which can distort the results interpretation.

In the example below, stresses well above the elastic limit appear on localized peaks.

Example of a scale not adapted to a stress analysis

An upper bounding of the scale, possible with a lot of software, makes it possible to show the areas impacted by overruns:

Scale bounding

The software's operating parameters being well understood, before any exploitation of the results and analysis of possible remaining stress peaks, it is advisable to carry out some simple checks to validate the calculation model:

control the vertical load calculation (support reactions) in order to ensure that all the introduced loads are at the level of the declared model supports;
control the configuration of the global deformation of the structure;
Control the magnitude of the displacements and their compatibility with the boundary conditions imposed on the structure and the applied load(s).

Finally, these are the fundamental checks that must be done for any finite element modeling (see § E.2 Self-~~checking)~~checking).

D.6.5 Results analysis - Acceptance of residual peak stresses

As mentioned above, it is possible to use a model with stress peaks if we are certain that these peaks do not disturb the outcome of the objectives of the study. In any case, it is up to the engineer to evaluate whether or not a stress peak is disturbing or not, using his or her experience and critical thinking.

Modeled zone without consideration of design details

The implementation of connecting fillets or local stiffeners is intended, among other things, to ensure a better diffusion of efforts. The constructive provisions and the bridges regulations in terms of metal assemblies are in accordance with this.

Therefore, the non-modeling of a constructive detail will probably result in a stress peak.

However, the modeling of the constructive detail does not exempt us from the presence of a stress concentration all the stronger that the mesh of the local area of the detail is thick. Sensitivity tests on the size of the elements can be performed in order to get a good understanding of the displayed results. Stress concentration charts can also be useful.

Examples of stress concentrations at singularity level

Stress concentrations peaking at values above the elastic limit of the material may be acceptable at the ULS if they are very localized and in facesheets. However, their justification may sometimes require an elasto-plastic calculation, especially if the area of stress exceeding the elastic limit is transverse (risk of plastic hinges). If the software allows it, this elasto-plastic calculation is performed considering a bi-linear behavior law of the material. Appendix C (informative) of EN 1993-1-5 authorizes a limit value of the maximum deformation of 5% for the zones in tension. For areas in compression, it is advisable to remain vigilant with regard to local warping phenomena.

Zone with a mesh singularity

The meshing of the areas of interest must be adapted to the fields of expected stresses or deformations.

If the mesh is poorly adapted with, for example, abrupt changes in size, stress jumps from one element to another are to be feared. Faulty discretization will result in significant discrepancies between simulation results and reality. These discrepancies can be reduced by carrying out a sensitivity study of the mesh: the mesh is considered satisfactory when the refinement leads to a small variation of the result; for example, a variation of less than 5% for element sizes divided by 2). But be careful, it is not because a result seems to have stabilized at 5% that we approach the reality at 5%.

It is not necessary to refine the mesh over the entire model. Most of the software allows to display error maps to locate areas with high stress jump. Some software even allows to automatically correct the mesh to reduce these deviations (adaptive mesh).

Zone with punctual effort or punctual blocking

We have previously presented the effects of the implementation of a punctual effort or blockage.

However, even if care has been taken to distribute the load over several nodes, stress concentrations may occur with maximum values above the elastic limit of the material. This situation may nevertheless be quite acceptable depending on the purpose of the study and modeling. Take the case, for example, of the modeling of the attachment zone of a suspender cable. The stress from the suspender is distributed sinusoidally over the nodes of half the circumference of the bore (hole).

We obtain a stress concentration around the axis bores with a maximum value of 558 MPa, a value well above the elastic limit of 400 MPa. However, this maximum value is not to be compared with the elastic limit. The stress concentration here is due to the diametral pressure and the regulations indicate that the diametral pressure resistance of the plate is equal to 1.5.t.d.fy. Since the thickness t of the coping and the bore diameter d are taken into account in the modeling, 558 MPa should be compared to 1.5 x 400 = 600 MPa.

D.6.6 Synthesis

If the stress peaks are due to singularities (reflex angle, interface between two different materials, point loads), they can be neglected ... if the state of stress in the proximity of the singularity is not part of the objectives of the FE study. Otherwise, it is necessary to improve the modeling (by replacing the reflex angle by a connecting fillet, replacing the zone of discontinuity between behavior laws of different materials by a transition zone in which the parameters vary continuously, replacing a point force by a contact pressure on a non-zero surface).

If these stress peaks appear in areas outside the proximity of a singularity, we should do a successive mesh refinement of these areas to know the more realistic stress level.

As far as smoothing is concerned, there is no simple and direct method. The reader will be able to look at what is practiced for fatigue calculations, in the case of a large stress gradient in the weld proximity in connections, with the application of the hot-spot geometrical stress method (see bibliography (ref. Hobbacher)).

Concerning the value of the maximum stress obtained, it must be compared to the limit value specified by the Calculation Standards. For steels, the Eurocodes standards define the value of the elastic limit according to the grade of steel and the thickness of the plate or tube; for example, for a tube in S355 steel with a thickness of 35 mm → elastic limit = 345 MPa according to EN 10210.

Any exceeding of this limit:

must therefore be justified. And this may be paradoxical, but it is easier to justify a stress overstepping in the case of a singularity than in the case of a current zone;
must also be acceptable. If the elastic limit is exceeded, plastic deformation will occur. An elasto-plastic calculation will give information on the rate of deformation (for structural steels, the Eurocode EN 1993-1-5 specifies a maximum principal deformation limit of 5%). The standard specifies the ULS criteria that can be used. For zones in tension, it is a question of reaching a limit value of the main membrane deformation (limit of 5% recommended) and for structures sensitive to warping phenomena, reaching the maximum load.

Finally, it should be remembered that an FE calculation (unless certain very specific calculation options are activated) does not take into account phenomena other than shear lag, for example instability phenomena such as warping and plate buckling.

Numerical application: Illustration of chapter D.6 - Peaks in angles, mesh incidence and fillet incidence. Link to the file.

Illustration of Chapter D.6 - Peaks in angles, mesh incidence and fillet incidence.

Authors: D. Guth (Arcadis) - P. Mangin (CTICM) - v0 – Jun 25th ,2020

Input data

The modeled structure is a simple flat angle bracket made of 10 mm thick steel (dimensions in m on the view):

We apply a load of 100 kN/m to the upper horizontal edge.

We do not take into account warping phenomena - this is a "simple" mechanics of materials model.

We start with a mesh size of 10 x 10 mm² and refine the mesh in the peak areas, as shown in D.6.

"If the stress peaks are due to singularities (reflex angle, interface between two different materials, point forces), they can be neglected ... if the state of stress near the singularity is not part of the objectives of the FE study. Otherwise, it is necessary to improve the modeling (replace the reflex angle by a connecting fillet, replace the zone of discontinuity between behavior laws of different materials by a transition zone in which the parameters vary continuously, replace a point force by a contact pressure on a non-zero surface).
If these stress peaks appear in areas outside the proximity of a singularity, we should successively refine the mesh of these areas to know the most realistic level of stress.”

Results

We will also find that the more refined the mesh is, the more the extreme stress will increase.

2.1) Calculation without fillets (right angle) - successive mesh refinements

Mesh =10x10 mm² to start - each successive view represents a x2 mesh refinement, at the angle where the peak appears.

Zoom - Von Mises stress in the angle:

Let us set an arbitrary elastic limit of the material at 460 MPa: we present below the extent of the zone having a stress above this elastic limit - about 10 mm long

The curve below gives the evolution of the stress peak according to the mesh thinness.

This curve reflects the fact that at a singularity, the stress peaks will increase singularly (literally)with the mesh thinness.

If this zone is of no interest with respect to the study's objectives, we admit the presence of a stress peak at the singularity. It should be noted that if this zone is not of interest, it is not necessary to refine the mesh of this zone. Nevertheless, it is always disturbing to display iso-stress with a stress peak at 753 MPa.

If the recipients of the calculation note have some experience, they will admit this singularity. Some may ask for an elasto-plastic calculation, if the value of the stress peak is too excessive (of the order of 2x the elastic limit of the material).

For information, for an S460 steel, an elastic stress peak at 750 MPa should not produce excessive plastic deformation (we would remain below 5%, the limit value recommended by Eurocode EN 1993-1-5).

If this area is relevant to the objectives, it is necessary to model the connecting fillet.

2.2) Fillets Implementation r=50 mm

The Wiki indicates that the minimum fillet must have a radius greater than or equal to 2 times the thickness of the part - here r=50 mm> 2x10 mm - ok.

Note.

The fillet consists of a succession of straight segments.
The mesh at both ends of the fillet shows FE that do not have an optimal aspect ratio, due to the connection angle that tends towards 0.

Base mesh 10x10 mm²:

It can be seen that the increase rate of the peak value is lower at each refinement than in the previous paragraph.

Arbitrary filtering at 460 MPa does not show an overflow area:

Let us assume that we have an elastic limit at 440 MPa, filtering at 440 MPa:

(dimensions in mm)

If the material’s elastic limit is 440 MPa, a stress peak at 459 MPa is perfectly acceptable for an SLS analysis (for a Fatigue analysis this would not be the case but this is another approach).

At this stage, there is no need to further refine the mesh. We can see that the value of the peak stress tends towards a realistic value.

Results

The curve below gives the evolution of the stress peak as a function of the mesh thinness and according to whether or not the connecting fillet is taken into account in the modeling.