question marks

Module weld

  • How do I interprete the warnings and errors in FEMFAT 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:

    Error no. Description
    W11461 All element nodes are declared as weld nodes at the shell element in question. This indicates to the program that welds are analyzed at all element edges of this element. This does not correspond to the requirements of the modeling guidelines.

    This can lead to an interpretation error, in that additional welds are considered at weld edges that are not intended as such in the structure. The damage result or the endurance stress limit safety factor at the nodes in question may for this reason be too conservative for certain stress conditions.
    W11462 Although the weld node in question was declared as simple weld node (C100-C102, C106 or C107), it possesses differing joint types or weld types. The load flow across the neighboring element given in the weld database can therefore not be taken into consideration.

    Where simple welds are involved, the program checks that all neighboring weld elements belong to one joint type and weld type. Only in this case is it possible to consider the load flow across neighboring elements.

    WARNING 11462 can be subdued by declaring, where necessary, weld nodes as combined weld nodes (C103-C105, C108 or C109).
    W11463 At least one element, which was not declared as a weld element, is connected to the simple weld node in question. That is, the material property label of this element is not between 100 and 499.

    In principal, it is possible to attach elements other than weld elements to a weld node. However, the stresses in these elements are ignored during the weld assessment.

    WARNING 11463 can be subdued by declaring weld nodes as combined weld nodes (C103, C104, or C105).
    W11464

    More than one defined neighboring element was found for the node in question. The load flow across the neighboring element can therefore not be considered. 

    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.

    Error no. Description
    E11451 There is no assessable element at the weld node in question. The node therefore cannot be evaluated as a weld by FEMFAT.

    This is generally due to an error in coloring of the weld nodes in the FEM preprocessor. Because the node is not connected to a shell element assessable as a weld, it is of no further meaning for the FEMFAT weld evaluation.
    E11452 No neighboring weld element was found for the weld node in question. The node is subsequently treated as a base material node.

    This indicates a modeling error in terms of the weld modeling guidelines. A minimum of one weld element must be connected to a weld node.
    E11453 No neighboring weld element, connected via an element edge, was found for the weld node in question. The node is subsequently treated as a base material node.
    E11454 No neighboring weld node, connected via a weld element edge, was found for the weld node in question. Therefore, no spatial weld course can be calculated, as the weld has a length of 0.The node is subsequently treated as a 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: 

    No. WARNING message Description Assessment method
    W11401 Error when determining the web plate angle ALFA. The normal vector of the web or base plate could not be determined. The web plate angle is calculated based on the normal vector of the base and web plate element. These normal vectors are determined with the aid of a non-weld node of the relevant weld element. Such a node could not be found. A default value ALPHA = 45° or 90° is used. SSZ/MSZ method
    W11402 Error when determining the web plate angle ALFA. Too few input data for cosine calculation.COS(ALPHA) could not be determined from the Inproduct when calculating the web plate angle from the element normals. One normal vector is zero. A default value ALPHA = 45° or 90° is used. SSZ/MSZ method
    W11403 Error when determining the web plate angle ALFA. If the angle between the normal vectors of the base and web plates is smaller than 1.14° is, this WARNING message is given.A default value ALPHA = 45° or 90° is used. SSZ/MSZ method
    W11404 Error when determining the web plate angle ALFA. Relevant elements for calculating the angle were not found.Web plate and base plate are identified based on the MAT labels in accordance with the modeling guideline. The MAT labels must also be listed in the weld database for the SSZ entries (ZA, ZB or ZC identifier).A default value ALPHA = 45° or 90° is used. SSZ/MSZ method
    W11420 at element withlabel ….. If the web plate angle is too small (1.14°<ALPHA<15°), then the element is evaluated as a lap joint. SSZ/MSZ method
    W11421 The sheet thicknesses at the SSZ joint could not be determined.The weld evaluation is stress-based (standard WELD method)! Both sheet thicknesses at the joint could not be determined or are zero. Check that the modelling guideline was adhered to. FEMFAT 4.7
    W11422 Sheet thickness 1 at the SSZ joint could not be determined.Thickness 1 is set to thickness 2! Sheet thickness of side 1 could not be determined or is zero. Check that the modelling guideline was adhered to. SSZ/MSZ method
    W11423 Sheet thickness 2 at the SSZ joint could not be determined.Thickness 2 is set to thickness 1! Sheet thickness of side 2 could not be determined or is zero. Check that the modelling guideline was adhered to. SSZ/MSZ method
    W11424 SSZ geometry parameter outside of allowable range. The geometry parameters are checked for plausibility. If the value is outside the permissible range (see Table 25), the default vale from the database is used SSZ/MSZ method
    W11425 at element withlabel ….. The MAT label of the element is not associated with a SSZ joint. The MAT labels associated with a SSZ joint are stored in the weld database with the ZA, ZB and ZC identifiers. If the MAT label is not entered there the element is not recognized as a SSZ joint and evaluation is stress-based. FEMFAT 4.7
    W11426 at element withlabel ….. The forces at the nodes are all zero or very small. If all 6 components (3 forces, 3 moments) of the force vector are zero or are very small, evaluation is stress-based (default WELD method). FEMFAT 4.7
    W11427 at element withlabel ….. The MAT label of the element is associated with a SSZ joint but allocation to a joint side failed. Check that the modelling guideline was adhered to. The element evaluation is stress-based. FEMFAT 4.7

     Table 4: WARNING messages for SSZ/MSZ method

  • How is mesh-dependency reduced during weld evaluation using WELD?
  • 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. 

  • What needs to be observed when expanding the WELD database?
  • 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.
       


          

  • What standards can be used for the analysis of weld seams using FEMFAT weld?
  • 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.

  • What settings are required for importing grid point forces?
  • 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
        

  • Why is „Not Analysed“ displayed in the results display for weld nodes in VISUALIZER for individual result positions?
  • 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.