Module weld

In order to check and validate weld node analysis results, any possible source of errors are written as WARNING messages to the message file during automatic stress correction.

WARNING messages may occur. They only point out to the user that unusual conditions occur at the weld element or weld node in question, but need not be a direct cause of a false result.

WARNINGS during weld environment examination:

Table 1: WARNING messages during weld environment examination

ERROR messages on the other hand indicate false results or a false interpretation at the weld node concerned.

These occur because of gross breaches of the regulations of the weld modeling guidelines and can generally be rapidly remedied in the preprocessor without renewed FEM stress analysis. They are intended to point out to the user that conditions occur at the weld node in question that are fundamentally erroneous. Erroneous weld nodes are subsequently treated and assessed as normal base material nodes. Analysis of further, correct nodes is not influenced by this.

ERRORS during weld environment examination => weld nodes are treated as base material node.

Table 2: Error messages during weld environment examination

Warning messages in the message file due to automatic stress correction

If, under certain circumstances, such WARNING messages occur it means that the "Automatic stress correction" (if activated) could not act at the node label in question. The corresponding weld node is then assessed without automatic stress correction, i.e. the element stress tensor of the current weld element is used. Such a WARNING message has no effect on the subsequent analysis of the remaining weld nodes.

 Error in automatic stress correction => weld node is analysed without stress correction.

Error no.	Designation	Description
W11431	Weld modeling error	Either all nodes of a quadrilateral shell element were defined as weld nodes or an element with a weld material label possesses no weld nodes.
W11432	No stress result for the element	The weld or neighboring element has no stresses.
W11433	No neighboring element	No neighboring element was found when searching for the assessment point, e.g. if the assessment point lies outside the entity.
W11434	Neighboring element not the required element type	The neighboring element must be a linear or parabolic shell element.
W11435	Varying element thicknesses	The thicknesses of the neighboring and the weld element differ.
W11436	Geometry not suitable for stress correction	When stress correction is performed for a coarse FEM mesh, the stress at the assessment point is found by linear interpolation between weld element and neighboring element. For this interpolation to provide correct results, the geometry of the FE-mesh will be checked: 1.) FEM mesh must not be too distorted at the seam. The angle shown in the following figure is adopted as a measure of the distortion. WARNING 11436 is issued if this angle is greater than 41° for stress correction of coarse FEM meshes. 2.) If the weld element and the neighboring element have different shell orientations, WARNING 11436 appears. 3.) If the angle between the element normal of the weld element and the neighboring element is greater than or equal to 90°, WARNING 11436 appears.
W11437	The weld FEM mesh is too fine.	When stress correction is performed for a coarse FEM mesh, the stress at the assessment point is found by linear interpolation between weld element and neighboring element. If the FEM mesh at the seam is very fine compared with the neighboring element, the interpolation could give unrealistic stresses. The ratio of the distances to the element center points should not exceed a limit of 100 (D/2R < 100, see figure below)
W11438	No nodes found near the assessment point belonging to the relevant neighboring element	If the distance from the weld seam of the center point of a neighboring element is greater than the distance of the assessment point, the node of the neighboring element with a minimum distance to the assessment point is used for weighted stress averaging. If this node with the smallest distance to the assessment point is not found, WARNING 11438 is written to the message file.

Table 3: Error messages arising from automatic stress correction

Warning messages in the message file due to force-based assessment using the SSZ/MSZ method

If the SSZ or MSZ method was selected as the evaluation method, FEMFAT tries to determine the line loads based on the weld element node forces and to calculate structural stresses from them. If the line loads cannot be determined the element is automatically analyzed using the FEMFAT 4.7 default analysis method based on the FEM stresses. A WARNING message is then written to the message file (*.msg).

WARNING messages for the SSZ/MSZ method: 

 Table 4: WARNING messages for SSZ/MSZ method

For simple weld fatigue assessments, the stresses acting on the finite elements defining the weld are often used. In this case the evaluated stresses are largely a function of the element size. Figure 1 shows the distribution of the normal stress perpendicular to the weld for a lap joint with four different element sizes. It can be seen that the maximum stress is a function of the element size on the one hand, and that, on the other hand, the stresses are almost identical at a relatively small distance.

With the aid of the automatic stress correction in WELD the user can specify the assessment distance D from the weld where the stresses are identified, regardless of the element size. The minimum sheet thickness at the joint is used by default; i.e. the assessment point is near the weld transition zone. First, a neighboring element to the current weld element is searched for. If the center point of the neighboring element is at a greater distance than the assessment point, the stresses of the weld element and the neighboring element are interpolated.

If the center point of the neighboring element is at a lesser distance than the assessment point a search algorithm is started. The algorithm searches along an interpolation plane perpendicular to the weld for an element with an element center further from the weld than the assessment distance, and with the smallest distance from the interpolation plane.
     

All elements attached to the node with the smallest distance to the assessment point are then used to acquire a weighted mean for the stress components:
        

Stress component for evaluation of the current weld element (transverse, longitudinal and shear component)
   
Stress components (transverse, longitudinal and shear
components with regard to the local weld coordinate
system) of the i elements at the assessment Point
  
Distance of the element center of element i from the
assessment Point
   
Number of elements utilized for evaluation of the current
weld element at the assessment point

An analogous procedure is also adopted for weld ends parallel to the weld. 

Because FEMFAT weld uses an ASCII format database for weld assessment it is also possible for the user to adapt the database to their requirements or to expand it if a special weld type is not supported.

The database includes notch factors, weld S/N curves, weld Haigh diagrams, etc. During analysis FEMFAT differentiates between the shell membrane and bending stresses. This makes it necessary to enter notch factors for both types of loading when expanding the database.

The notch factors are usually computed using a Radaj model (1 mm rounding radius for root/toe and 10 mm sheet thickness), which is subject to various membrane and bending load cases. The factors acquired are related to evaluations perpendicular to the weld direction.

When evaluating Radaj models it should be noted that the stress component in the direction of loading is adopted (notch factor = notch stress/nominal stress).
   

The factors from a similar joint can be adopted for the weld end, or they can be determined by means of a 3D model (structure analogous to the Radaj model).

Once the evaluated notch factors have been entered the equivalent element list must be appropriately expanded for joint types with neighboring elements (e.g. T-joint), see the example below:

$ Substitute element allocation

$ ------------------------------

$ T-joint, one-sided fillet weld with root undercut

$ ---------------------------------------------------------------

R 201 202

R 202 201

R 203 204

R 205 206

R 206 205

If the nodal forces based SSZ/MSZ method is used in addition to the standard FEMFAT method, the new MAT labels should also be entered in the SSZ parameter list.

The SID labels must be adapted to make the newly defined welds available in VISUALIZER. Ensure that the predefined SID ranges are used (see FEMFAT weld manual).

Now the small, detailed model displayed in VISUALIZER as a visual feedback must be entered in the database as a polygon and the image stored in *.gif format. This image must be added to the "weld_images" folder, which is located in turn in the WELD database folder.
   

The FEMFAT installation package includes the ECS standard (notch stress concept) as well as the WELD databases according to BS7608, DVS952 and Eurocode 3 & 9.

In addition to this, there are further databases available on request for standardcompliant weld analysis according to
• DVS1608 & DVS1612,
• IIW,
• FKM (nominal or notch-stress based).

Please keep in mind here that the databases offered contain a selection of FAT classes and/or joints.

If the desired FAT class is absent, we would be happy to assist you in enhancing the WELD database.

Due to the fact that the S/N curves of the standards reference nominal stresses but FEMFAT processes structural stresses, the results will lie on the conservative side in many cases.

If the nodal forces are to be imported for a FEMFAT spot (JSAE method) or FEMFAT weld (SSZ/MSZ method) analysis, the corresponding check box (see figure) must first be activated. This option prevents excessive memory use. Note: Node forces can currently be imported from NASTRAN op2, Abaqus otb and MEDINA bof.
   

GUI for the node forces in BASIC
    

GUI for the node forces in MAX
    

For the output and display of results at weld nodes, there are three result positions available in the VISUALIZER:

Visualization of the analysis results as a middle or end node,

Visualization of the results at the weld root or at the weld toe,

Visualization of the results of the individual stress components (Normal stress perpendicular to and parallel to weld, Shear stress, Equivalent stress).

Basically, the critical values for each of the three categories are first displayed when invoking the results. The user-defined selection of the evaluation positions can be made via a drop-down menu.

However, it should be noted that all results for root & toe are not available for all involved sheets / elements at one weld seam node. Only those weld toes and roots are calculated for which notch factors have been defined in the WELD database. The values of the most critical element are then displayed according to the settings.

This means, for example, that if the critical element has no weld toe at all (because it lies on the side away from the seam like an element of type 202, pictured right), then the value is also not available. In VISUALIZER, when „Toe“ is selected for such a weld node, „Not Analysed“ is displayed, cp. the example of a T-joint below.