经常问的问题

After a FEMFAT analysis, detailed local results (e.g. Haigh diagram, S/N curve, equivalent stress history for MAX) are output as standard for the critical node.

Due to boundary or contact conditions, it is possible that this node is not of interest to the user. This is why FEMFAT offers several possibilities for requesting this output for a specific node group.

The first and simplest option is the targeted output for an individual node. This can be found in the FEMFAT menu “Analysis Parameters”, see Fig. 2. To do this, select the option “Particular Node” and enter the desired node label.

For several nodes, it is possible to request enhanced output via the “Detailed Results” group in FEMFAT. The definition can be made in the FEMFAT “Groups” menu as shown in Fig. 3, e.g. for a range of node labels. FEMFAT generates this group when the “Detailed Results” button is clicked.

Attention: This group is not the analysis group because it only contains the nodes for the additional output.

Furthermore, detailed output items such as the local equivalent stress history or partial damage history are written to external ASCII files for the DETAILED RESULTS group in a MAX analysis.

These files can be imported into EXCEL, for example, and there be processed further. In addition, these data are also written to the fps file. Consequently, it is possible to display the local equivalent stress history in the VISUALIZER, for example.

If for a FEMFAT design only a small part of the FE model is to be assessed or, if after a calculation has already been carried out the critical points are to be analyzed again with different parameters (different surface finish, different material, ...), it is important that in addition to the nodes to be evaluated all neighboring nodes and elements are also included in the new calculation group, so that the averaged element stress at nodes and the gradient calculation in FEMFAT can be performed correctly.

If, for example, the red node (Fig. 1) is to be correctly calculated, the stress values of the adjacent elements have to be included in the group too for enabling a correct determination. The stress value at the FE nodes “connected via an element edge” must also be correctly determined (stress averaging) to enable correct determination of the relative stress gradients.

1. Generate the group with the nodes to be considered.
2. Enlarge the group by adding all elements connected to this node.
3. Add all the nodes connected to these elements and the elements in turn connected to them to define the calculation group. If the node under consideration derives from a parabolic element, make sure that at least the adjacent corner nodes are also included in the calculation group (Fig. 2).

It is, of course, also possible to select a larger calculation group for a detailed area than that shown in the illustrations.

Surrounding nodes and elements can be quickly and easily added in the FEMFAT group menu using the “Nodes/Elements related with Elements/Nodes from Group xx” option (Fig. 3). 

Only two items of basic information are required: the material group and the ultimate tensile strength of the material. It is possible to choose from 12 material groups in the material generator (10 iron and 2 aluminum material groups; see FKM guideline).

The material generator is based by default on the FKM guideline and generates material data for a survival probability of 97.5% for a specimen diameter of 7.5 mm.

After selection of the material group, the complete material dataset can be generated by entering the ultimate tensile strength.

An analysis can now be performed using such a dataset. It must be mentioned, however, that when using these material data, conservative results can be expected. The following data are advantageous in order to increase the precision:

• Tension/compression alternating strength σTA
• Tension/compression pulsating strength  σTP (defined as upper stress in FEMFAT)
• Bending fatigue strength σBA

This makes it possible to find the mean stress sensitivity of the material using the relationship

M =2*σTA / σTP - 1

Furthermore, the support effect is defined by the ratio V= σBA / σTA (important for analyses with gradient influence in FEMFAT). The following steps apply if only one of the values mentioned is known:

1. Determination of the values V and M of the base material.
2. Modification of all values on the basis of, e.g. the known tension / compression alternating strength: σTA.

Example:

Material group, general structural carbon steels, UTS = 500 N/mm², Yield = 300 N/mm2, σTA = 250N/mm².

Step1: Selecting the material Group

Figure 1

This influence stands for the determination of the local, static material properties, taking the stress gradient, isothermal temperature and technological parameter influences into consideration.
In the first step, the ductility for the "stress gradient" influence is estimated based on the elongation at rupture of the material (see Fig. 1), which subsequently determines the maximum achievable value of the local ultimate stress limit.

In the next step, the corresponding ultimate stress value is calculated based on the known tensile strength (rel. gradient = 0), the ultimate bending stress (rel. gradient = 2/specimen thickness) and the previously determined relative stress gradient (see Fig. 2). The "limit line" (red) is given by the factor from the first step.

The ultimate stress is reduced in analogy to the equations in the FKM guideline for the isothermal temperature influence (default method "FEMFAT 4.6"). If a user-defined temperature influence is used, FEMFAT uses the corresponding polygon from the material definition (temperature -> strength reduction to ultimate stress).

Moreover, the technological size influence can additionally be taken into consideration for large wall thicknesses/diameters; it is also taken into consideration in accordance with the FKM Guideline.

If this new group is selected for the analysis, the result at FE nodes in the original group (which has been copied at the beginning) is correct.
If several groups have been defined, e.g. for the definition of the surface roughness, temperatures and so on, it has to be considered that before the start of the FEMFAT calculation or the generation of the MAX scratch files, the correct calculation group has to be activated. This can be checked very easily by “CHECK INPUT DATA”, because the active group for calculation is mentioned there again.

Six equivalent stresses are available in FEMFAT basic, in MAX this increases to 11 equivalent stresses. Generally speaking, the user need not be concerned with selection of the correct equivalent stress. The BASIC and MAX modules use the "Automatic" default setting. This is recommended by the ECS for all cases. Using this setting, the equivalent stress adopted is decided on the basis of the local material at the respective node. If a (brittle) gray cast iron is being dealt with, both BASIC and MAX employ the normal-stress hypothesis in conjunction with the critical cutting plane method.

If calculations are performed in FEMFAT MAX using the default "Automatic" setting, a scaled normal stress is formed in the cutting plane for all materials with the exception of gray cast iron. The use of a scaled normal stress solves what is known as the "sign problem", which may occur with most other equivalent stresses provided in FEMFAT MAX but which are now no longer recommended. The sign is required to form an equivalent stress history, in order to take both tensile and compressive stresses into consideration. However, this can lead to unphysical leaps in the equivalent stress history for non-proportional loading, depending on the selected equivalent stress, and thus to inexact and highly conservative damage results.

A special advantage of automatic selection is the possibility of combining a variety of materials during a single analysis run.

The scaled normal stress offers a procedure that eradicates this problem and that works just as efficiently as the "simple" normal stress without scaling. By applying a scaling factor to the normal stress the material ductility (brittle/semi-ductile/ductile) and the type of loading (tension-compression/bending, shear/torsion, hydrostatic stress state) can be incorporated in the analysis and be adequately considered even for non-proportional loading. A particular advantage of this scaled normal stress also lies in the fact that the triaxial stress states within the component or at compression-loaded component surfaces can be easily evaluated. The generally minor damaging effects of hydrostatic stress states are correctly modeled.

The use of invariants (von Mises' and max./min. principle stresses), on the other hand, does not allow consideration of arbitrary material ratios. We therefore no longer recommend the use of these equivalent stresses. They are still provided for historical reasons. 

The picture (Fig. 1) above shows the signed equivalent stress history of a cylindrical specimen, subject to a cyclic compressive load of small amplitude in conjunction with a high static torsional load (a prime example of non-proportional loading). The discontinuities are a consequence of signing and graphically represent the problems involved.

The picture (Fig. 2) below, in contrast, shows the same test setup analyzed using the scaled normal stress. It shows the scaled normal stress for the critical cutting plane. The stress cycles now display a realistic stress amplitude.  

FEMFAT so far used to calculate the stress gradient along the finite element edges by considering the stress gradient between two neighbouring nodes.

In most cases, the maximum stress gradient is perpendicular to the surface. Since parabolic tetrahedron elements are typically used in the meshing of a complex shaped structure, there are often no finite element edges perpendicular to the surface. This can lead to less accurate results.

The new method ("Vector Reconstruction") uses the stress gradients along the finite element edges to reconstruct the maximum stress gradient. This is done independently of whether there is an element edge in this direction or not.

Note: this new method is the default setting for BASIC, TransMAX and SPECTRAL as of FEMFAT 2022.

ChannelMAX has two special features in this respect: firstly, the method "Vector reconstruction reduced" is used as default. Thereby not all samples of the load-time curves are used, but only those at which minimum and maximum occur in the respective load time histories of the channels. Furthermore, in ChannelMAX, if a "Vector Reconstruction" method is selected, additionally the gradient is formed analog to TransMAX based on the superposed, time-dependent stress tensors.

If FEMFAT job files (*.ffj) older than v2022 are used, the old gradient method "FEMFAT 2.4" is automatically activated.

FEMFAT provides the user with a variety of options for checking input during analysis preparation or following the analysis. These are:

FEM-Model

• Number of imported nodes & elements (Caution: some "exotic" element types are ignored).
• Dimensions of model (unit correction to mm may be necessary)
• Minimum/maximum shell thicknesses
• Visual control in VISUALIZER including group definition; groups can be displayed in the main program as a label list.

Material Data

• Numerical control of the data in the material menu
• Graphical control using the Haigh diagram, S/N curve and cyclic σ - ε diagram
• In the node characteristics menu by browsing in the node labels for checking all properties (material, roughness, temperature, surface treatment,...)

Stresses

• In BASIC maximum principle stress of the element with the highest v. Mises equivalent stress
• For MAX, visual control of the stress sequence or the unit stresses is available in the VISUALIZER.

Menu Item "Check Input Data"

This function is available immediately prior to starting the analysis that allows a number of input data to be double-checked, in particular, whether the stresses and the material strength form a plausible relationship in terms of the required analysis result (endurance safety factor, damage life in the finite life domain, static safety). Implementation of these checks is strongly recommended, see figure below.

If you need help for generation of new materials, please do not hesitate to contact the FEMFAT support at femfat.support.mpt(at)magna.com

Today’s commercial simulation tools provide the possibility of simulating the casting process and of predicting the associated inhomogeneous structure conditions within the component. This gives, amongst other things, a distribution of the secondary dendrite arm spacing (SDAS), the solidification time, the cooling rate or the microporosity. It is possible to import these distributions into FEMFAT and to consider their influence on the endurance stress limit. Here, the solidification time and the cooling rate can be converted to an SDAS by means of an exponential approach. The currently implemented dependence of the endurance stress limit on the SDAS is optimized for aluminum sand and gravity die casting. However, the influence of the SDAS on the endurance stress limit can, if known, also be given by the user as a value pair table for any material. A new material dataset with the number 220 was created for this purpose. Nevertheless, it is also possible to consider microporosities or other structural parameters. In FEMFAT, the distribution of any structural parameter can be imported via the same interface, instead of an SDAS distribution. The only requirement is that the values are node-referenced. The file format thus corresponds to (node-referenced) temperature data. Moreover, for an operational strength evaluation, the influence of the specified structural parameter on the material endurance stress limit must be known and be defined by means of a table (dataset 220) in the material file (*.ffd).

The influence of cast structure in FEMFAT is already being successfully implemented by BMW in their engine development process, e.g. for cylinder heads.

The technological size in FEMFAT considers the material endurance stress limit which decreases with increasing component dimensions. The imported shell thickness, which is averaged at the nodes in FEMFAT, is used as the technological size for FEM shell entities. For FEM solid entities, on the other hand, the user must explicitly specify the technological size as a numerical value in [mm] in the node properties. You can activate the technological sice influence factor in the menu "Influence Factor".

The sample thickness is also included in the analysis, where it should be noted that the sample thickness at five points is included in the material data, i.e. in the strength data for tension, compression, bending and shear, and again in the general S/N data. However, only the value from the general S/N data is used in the technological size influence!

Details from the FKM guideline 

With the size influence activated in FEMFAT, an influence factor on the material alternating stress limit is calculated, in accordance with the FKM guideline [1, 2]. The "effective diameter" used in the equations there is identical to the "Technological size at 3D nodes" entered in FEMFAT for the node properties of the component.

In the following figure the influence of the technological size on the endurance stress limit is shown for various material classes. The corresponding FEMFAT material classes are given in brackets.

[1] FKM guideline "Numerical Strength Analyses for Machine Components in Steel, Cast Iron and Aluminum Materials", 4th Edition, 2002, www.vdma-verlag.de.
[2] FKM guideline "Analytical Strength Assessment", 5th Edition 2003, www.vdma-verlag.de.

Enabling the isothermal temperature influence means that the local operating temperature is taken into account at all analyzed nodes (usually upper temperature).

FEMFAT provides various analysis methods for this:

“FKM guideline” method
The isothermal temperature only affects the dynamic strength values in the Haigh diagram (vertical scaling).

“FEMFAT 4.5” method
This option changes both the dynamic strength parameters in the Haigh diagram (similar to the FKM guideline) and the static strength parameters (horizontal scaling of the Haigh diagram). The same formulae from the FKM guideline are used for modifying the yield stress and ultimate tensile stress. The user is warned if the temperature exceeds the range defined in the FKM guideline, and the influence factor is extrapolated on the basis of the implemented formulae.

“User defined” method
In this method, the temperature dependent material data specified by the user is taken into account; this data can be defined in the menu “Material data -> Properties at higher temperatures”. The temperature dependent fully reversed endurance limit and the ultimate tensile strength must be defined as a minimum for this method.

“FEMFAT 4.6” method (default)
This option is based on method 4.5, but in addition the cyclic coefficient of hardening K’ of the cyclic stress-strain curve is reduced in a similar way as the ultimate tensile strength. This means that the isothermal temperature influence is also correctly taken into account in the mean stress rearrangement of linear elastic stresses according to Neuber (FEMFAT plast module).

Isothermal temperature influence on Rm, Re and K´

One can see from the curves that all temperature influences based on FKM produce conservative results.

If you are unable to find the required material in the material database, you can also generate the data for the calculation on a few familiar properties of the material. The user has 2 options.

The first is called the 'stress-controlled' method by FEMFAT. Here you only need to specify the material class (Fig. 1) and the ultimate tensile strength for the material. Based on the predefined ratios taken from the FKM guideline, the system will now automatically generate all the missing material characteristics needed for the calculation (Fig. 2).

To increase the reliability of our conclusions, it would naturally be better if one was able to also pre-define the ultimate yield stress, pulsating load strength and ultimate compressive strength/alternating stress limit from specimen test data. However, one should be careful when changing materials outside of the material generator since the FEMFAT calculation uses a number of different relations based on the material data, for example the 'k' factor used to measure the ductility of the material.

The second method for generating a material is called the 'strain-controlled' method. The user not only needs to enter the material class (as in fig. 1), but also the data for ultimate tensile strength, yield stress and E/N curve (unnotched, polished samples, fully reversed tension/ compression) (fig. 3).

Finally, the number of cycles at the fatigue limit is also needed. Next, for this number of cycles, the strain amplitude is converted into a stress amplitude (corresponding to the fully reversed endurance limit). The fatigue strength exponent b is used to determine the gradient of the stress S/N curve (k=-1/b). After the material characteristics have been determined, you should then check the following and change where necessary: Survival probability, specimen diameter, elongation of rupture, check Haigh diagram & S/N curve for plausibility.

Since FEMFAT version 5.0 it is also possible to estimate parameters of materials with pores inside. In many cases as e.g. in Aluminum die cast components, there are areas with pores and defects, whereas surface layers are pore free. In FEMFAT a boundary layer model is provided for correct fatigue assessment of such cast components. Nevertheless the necessary parameters for material with and without pores are often not known. A new dialog for defect definition is now provided (fig. 4). Based on a pore free material or a material, where the maximum defect size is known (which is relevant for fatigue failure), material parameters can be derived for any other defect sizes.

The remaining temperature-dependent material parameters can be estimated automatically by FEMFAT – although it is better to provide more temperature-dependent material properties, such as the pulsating stress limit, for example. This extended material can now be saved to the material database once again using the "Write to materials database" command and be used for subsequent analyses. It is adopted automatically for the current FEMFAT session. A nodal temperature distribution must now be defined as an "isothermal influence". Do not forget to activate the isothermal temperature influence in "Influence factors" and to change the method used to "user-defined".

Fig. 2: Comparison of stress amplitudes from FEMFAT PLAST/ABAQUS

Summary:
Although a multi-axial stress state already exists in the notch, PLAST provides useful results up to approximately 15 kN (~ 0.3% plastic strain) for the local stress in the notch. If greater strains or stress multiaxiality are anticipated deviations may increase and a non-linear material law should then generally be employed.

Currently, structural data in the format NASTRAN op2/bdf, MEDINA, I-DEAS MS-Universal, ANSYS cdb are supported. The possible number of readable materials is 500.

If K´ and/or n´ have not been defined by the user, they will be automatically generated by FEMFAT based on the Uniform Material Law (UML) [1], as a function of the material group and the ultimate tensile strength Rm.
Remark: The Uniform Material Law was developed based on specimen tests for specific material classes to generate a correlation based on the material class and the UTS of the material.
[1] Bäumel, A. jr.; Seeger, T.: Materials data for cyclic loading, Supplement 1. Elsevier,
Amsterdam (1990).

FEMFAT break is a very practical tool for computing static safety factors from linear-elastic FEM stresses. For abrupt, infrequent loads (e.g. transmission jump starting, chassis-verge stone contact) it is recommended to perform a FEMFAT break analysis prior to the fatigue analysis. If an insufficient static safety factor results here (safety factor smaller than 1.0) the component is statically underdesigned.

The static safety factor is used to evaluate the local elongation capacity of the material until cracking under a monotonic load.

Please note that FEMFAT break cannot assess the global failure (fracturing, breakage) of a component (unless the material is highly brittle), but only the local material failure due to insufficient ductility. This means that initial damage (small crack) may be caused by high load peaks, which leads to further crack growth under subsequent operating loads, and finally to failure. In addition, it is assumed that the constant load is not applied highly dynamically; i.e. BREAK does not take strain rate effects into consideration. Influences in the BREAK module the notch influence is taken into consideration by means of the relative stress gradient. Required material parameters:

• Young’s modulus
• Static tensile strength Rm
• Static compressive strength
• Static shear strength
• Static elongation at rupture A5

FEMFAT basic provides the possibility of reading a third load case, designated as constant stress (σc), at the given amplitude and mean stress (σa, σm). These could arise from internal stresses or screw preloadings. When the constant stress effect (influence factors -> general factors; Fig. 1) is activated, the constant stress is included in the mean stress during the calculation. The difference with regard to the mean stress data set is in the definition of the load spectra, where only the mean stress is scaled with the “mean stress factor” (F_M) for each step. In the case of the fatigue strength analysis, the constant tensile stress with the R = const. option (one of the FKM overload situations) is taken into account as a shift to the right in the Haigh diagram (Fig. 2).

Besides the material, component geometry and stress conditions, the manufacturing process has a major influence on the fatigue behavior of a component.

In FEMFAT the following surface treatments are available:

• Shot peening (acc. to FKM, Eurocode or BS),
• Rolling (to FKM),
• Carburizing (to FKM),
• Nitriding (to FKM),

Here, the condition prior to nitriding can also be taken into consideration: Tempered or normalized

• Inductive hardening (to FKM),
• Flame hardening (to FKM).

 "Node properties menu" for the current group

For these treatments it is important that the Technological size at 3D nodes is given in "Node properties" (see image). This technological size is automatically determined from the mean shell thicknesses for shell structures. For example, the technological size is the wall thickness of a tube or the diameter of a shaft at the point where the surface treatment is carried out. Other influences, such as the relative stress gradient and the material strength are automatically taken into consideration by FEMFAT.

The Surface treatment factor provides a good option for incorporating experiences from testing into analysis. This directly alters the local endurance stress limit.

One common technological influence is the Surface roughness, which can be assigned to the current group. The S/N curves of the material data are generally defined for a smooth, un-notched specimen for alternating tensile-compressive loading. This means that a change in the surface roughness also changes the endurance stress limit, the slope and the endurance cycle limit of the local S/N curve at the node, including as a function of the material itself. In the methods listed under "Influence factors" one can also select between mean roughness depth Rz (to TGL or FKM) or the maximum roughness depth Rt (IABG) of the assessed component surface. The former TGL Standard - replaced by the FKM Guideline in 1994 - is no longer recommended. 

FEMFAT also includes an option for taking the Tempering condition into consideration for tempered steels. If the tempering condition changes (= new ultimate tensile strength) all governing material parameters are adapted to the new tempering condition. Following this, do not forget to activate the process influences in "Influence factors" (surface roughness, technological parameter influence, tempering influence...)!

By the way, this conversion can be carried out very conveniently using the FEMFAT Results Manager in which the above-mentioned case differentiation for the safety factor can be made automatically with the help of the formula Editor.

The time information (unit: seconds) can be defined in a number of ways. Either the step time from the stress, strain or temperature results can be used (which makes more uncommon step time definitions necessary) or a separate table is imported as a text file. This can be performed on the "Time information" tab.

It is possible to simulate the repetition of the load sequence in TransMAX by definition of “Number of Calculation Sequences” greater than 1. If a factor of 100 is given for 10 time points, it corresponds to a total number of 1,000 time points. The increase in this factor is useful for damage calculations, in order to reduce the effect of the Rainflow residuum on the result (not necessary for the Default Rainflow Counting Method).

Caution: When calculating the endurance safety factor, the factor does not affect the result and should remain unchanged (default value 1)!
This repetition factor can be changed as required without necessity to recreate the scratch files, because the duplication of the time points only takes place during the calculation.

As the number of time points is directly corresponding to the calculation time, the repetition should be selected with caution, e.g. in the 10-100 (see figure).

Figure 2: 1000 samples (original load list), 211 samples (compressed list)

This method is especially efficient if only small areas of the structure are to be analyzed: because many stress directions often only cause very minor stresses at the respective location, these channels can be highly compressed or even deleted, resulting in a substantial reduction in computation time. The import of the load-time histories and the compression are both very fast. This procedure can therefore be easily repeated (for several critical locations).

After the FEMFAT analysis, the user finally comes out with a damage distribution taking account as far as possible of non-linear contact effects.
This method can also be used with multi-axial loads. However, in this case, contact states may appear less accurate due to the non-linear transfer effects of multiple channels. This effect is rare however since in most cases only a few directions of the applied force dominate at a particular moment.
In any case, what matters is the correct working point, which is located close to the existing peaks in cases of practical relevance (the reason for this is simply because the largest peaks in load usually cause the highest partial damages).
You should be careful with initial pre-stresses: such stresses should be deducted from the operating load states and an additional constant channel defined.
In summary, what we have here is a practical method which offers sufficient accuracy in most cases, and which offers enormous time benefits (up to several orders of magnitude) compared over analyzing of many non-linear stress states together with a TransMAX analysis.

The cosine and triangle Signal allow specifying the number of sampling points per wave, the amplitude, the mean leveland a phase shift. The total number of samples is not queried until the load histories are scratched, if no load data are imported from interfaces. Typical applications for constant signals include bolt pre-stresses. Cosine signals can be used for rotating loads for example (2 load channels with 90% phase displacement).

​​​​​​​Option 2 – Compress load history

One procedure for eliminating less relevant channels is the loadtime data reduction provided by ChannelMAX. To do this, the settings “for the most critical channel” and “with consideration of channel stress” must be selected in the compression menu (see Fig. 2 top). The advantage here is that channels with small stress portions are completely deleted. In addition, data points between the minimum and the maximum are eliminated, as well as small amplitudes below a user-defined limit which only cause a minor damage share (Fig. 2 bottom). Beside the advantage of taking phase shifts into account, a considerable reduction in computation time results.

Option 3 - VISUALIZER

The FEMFAT VISUALIZER provides an option for also visualizing the corresponding load factors multiplied by the stresses from the unit load case for individual nodes (from the “Detailed Result Group”), in addition to the equivalent stress history, damage history and partial damages. After clicking any point in time with a large damage increase, for example, a diagram containing the corresponding stress values per channel is displayed. They are sorted according to size for clarity. From this, in turn, it is possible to derive which load channels contain a high damage component.

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.

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.

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.

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.