question marks


  • Do I sacrifice precision when applying filters?
  • In FEMFAT there are 3 options available for accelerating the analysis using "filters":
    1.Node filter: Only those nodes for which both the stress amplitude and the mean stress exceed a given value (% of the material endurance stress limit/tensile strength or absolute stress) are analyzed. That is, analyzed nodes do not suffer from a loss of precision, uncalculated nodes have no result (or dummy value).
    In BASIC the von Mises stress of the amplitude or mean stress tensor is used (see BASIC manual). In MAX differential stresses are adopted for certain critical times (see MAX manual).

    2.Cutting plane filter: In order to reduce the computation time when using the critical cutting plane method cutting planes can be filtered in MAX, i.e. they can be excluded a priori before the actual analysis. This can lead to a loss in precision. However, the filter is defined by default so that this very rarely needs attention. Three filter methods are available (see MAX manual).

    3.Rainflow amplitude limit: Load cycles with small amplitudes can be excluded in MAX, because they often only represent a very small proportion of the total damage. This can also affect a considerable acceleration in the analysis if the Rainflow matrix is dense at small amplitudes.

    Further possibilities for reducing computation time include:

    •Manual definition of a small analysis group (nodes + elements) –> no loss of precision.
    •Reduction in Rainflow classes in MAX –> generally means loss of precision.

  • How can detailed results for one or more nodes be requested in FEMFAT?
  • 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.

  • How can FEMFAT process my ABAQUS odb files?
  • To import ABAQUS odb files into FEMFAT the so-called odb libraries function as a translator between the two software products. The current odb libraries are automatically installed when installing the new FEMFAT version. These libraries are available as compressed files for a variety of hardware platforms on our homepage at (registration necessary).  

    It is recommended to always install the odb libraries corresponding to the ABAQUS versions to be employed, otherwise the odb files have to be updated by FEMFAT. Speaking of installation – the uncompressed odb libraries belong in the FEMFAT installation folder, more precisely in the odb folder created there automatically during installation. (Example: …\femfat53\platforms\winnt_61_x86-64_64bit\odb)

  • Which Abaqus versions are supported by FEMFAT?
  • Both FEMFAT 5.4 and FEMFAT 5.3 support Abaqus versions 2017, 2018 and 2019.

  • What does "Detailed Result Group" mean?
  • 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.


    Fig. 1

    If, for example, the red note (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.


    Fig. 2

    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). 



    Fig. 3

  • What does material generation look like in FEMFAT?
  • 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.


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

    Step1: Selecting the material Group

    Figure 1 

    and entering UTS leads to the result  in figure 1.


    Modification of the yield  strength (300 instead of the suggested 284.5) and alternating strength (the material generator modifies σBA in the correct ratio depending on the selected material group). We calculate the mean stress sensitivity as


    Consequently, the fi nished material dataset looks as follows:

    Figure 2

    Replacement in the formula for mean stress sensitivity using the values M = 0.075 and the known alternating  strength of 250 N/mm² gives the new pulsating strength of 465.1 N/mm².

  • What does the "Modified Haigh Diagram" influence mean?
  • 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.


    Fig. 1


    Fig. 2


    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.

  • What is the minimum amount of data needed for an accurate FEMFAT analysis?
  • The calculation group can be defined by the user with the help of his preprocessor (IDEAS, MEDINA, PATRAN,..) or with FEMFAT.
    FEMFAT gives analysis results for FE-nodes only, but needs the surrounding elements for their stress data and the accurate stress at adjacent FE-nodes which makes the necessary data for an analysis tremendously larger than just a few FE-nodes. To analyze one FE-node  FEMFAT  takes the stress gradient into account, why the accurate nodal stress (averaged from their adjacent elements) of all surrounding FE-nodes in direct connection are needed.

    The manual way to handle this, is to make a copy of the relevant group in FEMFAT and let it “grow” by two rows of elements and one row of FE-nodes by using the group dialog functions “add elements related to nodes of group” and “add nodes related to elements of group”.


    The automatic „one click solution“ is the button “Complete”(for Analysis) which does pretty much the same than the three clicks from manual solution.


    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.

  • What is the Stress Amplitude Filter good for?
  • To speed up the FEMFAT analysis the user can define a stress
    amplitude filter. There are two possibilities:
    • relative stress amplitude filter [%]
    • absolute stress amplitude filter [MPa]

    For the relative stress amplitude filter FEMFAT needs a percent value, which is related to the material alternating endurance limit (tension). By default, the relative stress filter is 40%, then all nodes will be analyzed for which the amplitude stress is higher than 40% of the material endurance limit (alternating strength for tension) and the mean stress is bigger than 40% of the UTS.
    For the absolute stress amplitude limit the user directly types in the stress limit [MPa].

    For example the user chooses 30 MPa, all nodes having a lower stress amplitude than 30 MPa will be filtered.
    Therefore take care, if there is a very high mean stress and small amplitude stress at nodes. In such case we recommend to switch to the absolute amplitude stress limit.

  • When/Why FEMFAT basic, ChannelMAX or TransMAX?
  • FEMFAT basic

    for proportional loading that can be described by two states and a constant component (e.g. assembly).

    Advantage: the analysis speed is very fast because FEMFAT basic holds the data in RAM.

    Examples: Conrod, cylinder head, gearbox casing, shafts etc.

    Input data required:
    • Upper/lower stress or amplitude/mean stress
    • Constant stress (optional)
    • Load spectrum for damage analysis



    The loading consits of stresses due to unit load cases and the corresponding load-histories. The system response (except local plastic deformations) must be linear because of the linear superposition of the unit load cases.

    Examples: wheel mounts, axle frames, body work, crank shafts

    Input data required:
    •One stress result per channel (load direction, modal shape)
    •One load-time sequence per channel



    Most general form of the load history. The system response can be completely non-linear; number of time points limited to hundreds (thousands).

    Examples: cylinder block and other components with complex contacts.

    Input data required:
    •Sequence of computed stress states over time

  • Why are several equivalent stresses available?
  • 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. 

    Fig. 1

    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.  

    Fig. 2

  • Why does the protocol file (*.pro) show different damage results to the postprocessor result file (*.dma)?
  • If these are only minor differences they may be the result of rounding errors in the protocol file (4 decimal places) or the visualization in your postprocessor.
    A further possibility is the use of the test track length input in "Output modification" (see below). These modifications only apply to the dma file, the factor is not calculated for the protocol file.

  • How helpful is the Result Manager?
  • The Result Manager provides options for better result visualization of FEMFAT results. For example, it is possible to perform a minimum/maximum search of several FEMFAT results. Additionally, an equation editor is available beside the simple linear combination option for individual results.
    The damage results can be merged here by way of user-defined equations. This allows simple computation of the utilization factor of welds according to the FKM guideline, for example.
    The result is immediately available to VISUALIZER in the fps file or can be exported in the usual result formats.  

  • What does 'Influence of rotating principal stresses' mean?
  • In some loading situations, e.g. in crankshafts subject to combined bending/torsional loads, a local change or rotation in the directions of the principal stresses may occur with time.

    Tests using combined bending/torsional alternating loads and 90 degree phase shift have shown that for ductile materials (tempered steel) the critical cutting plane method overestimates the lifetime (e.g. see FKM report "Multiaxial Fatigue Analysis, 2002"). In FEMFAT max it is possible to correlate the lifetime using "Influence of rotating principal stresses".

    The local S/N curve is reduced as a function of a statistical degree of multiaxiality lying between 0 (= proportional load with constant direction of principal stresses) and 1 (= heavily nonproportional load with directions of principal stresses changeable with time).

    The influence thus results in a reduction in lifetime in ductile materials.
    No impact is defined for brittle cast materials (gray cast iron, cast Al, cast Mg).

    Rotating bending with torsion

    We recommend activating the influence of rotating principal stresses. However, in certain cases, e.g. where high constant stresses are involved (bolt pre-stresses, residual stresses), the results may be conservative. 

  • Which options are available for FEMFAT batch Jobs?
  • The Batch Job feature is intended to allow FEMFAT to run in the background automatically with no interactive input on the user interface. It is especially helpful to use batch jobs when a number of FEMFAT analyses must be carried out (e.g. engine run-up). Typically, a FEMFAT job in the batch mode is invoked
    using the following call:

    …/bin/femfat –job=jobfilename (Linux)
    …/bin/femfat.bat –job=jobfilename (Windows)

    This standard call can be expanded using additional Parameters which offer the user a wide range of possibilities. For example, it is possible to specify a separate scratch Directory for the individual jobs,

    …/bin/femfat –job=jobfilename -scr=Scratch_Directory

    …/bin/femfat.bat –job=jobfilename -scr=Scratch_Directory

    or disable individual modules (here: PLAST):

    …/bin/femfat –job=jobfilename -noplast (Linux)
    …/bin/femfat.bat –job=jobfilename –noplast (Windows)

    A detailed overview of all available parameters can be found in the “FEMFAT_Introduction.pdf” manual. This manual is contained in the installation directory in both German and English along with all the other module manuals.

  • The file userdefparam.dbs cannot be found – What should be done?
  • The background for this message is that during the Definition of the new working directory in the ini file, a path was selected for the material import which does not contain the userdefparam. dbs file.

    This database makes it possible to adapt fundamental properties which are material-class specific (slope exponent of S/N curve, material-dependent exponent, exponents for gradient
    influence, etc.).

    If you have not made any modifications in the database, then you can ignore this message and click “OK”. In this case, FEMFAT uses the database with the respective default values
    from the installation directory.

    If you have modified the userdefparam.dbs file and wish to use it, then you must either copy the database to the specific working directory or change the default import path for materials
    in the FEMFAT settings to reflect the corresponding save location.


  • For a FEMFAT spectral analysis, I get the warning “The defined spectral lines do not cover the common domain of all given (cross) PSDs…”.
  • The warning indicates that the frequency range of the PSD definition is greater than that which is covered by the transfer functions. Consequently, loads are analyzed in a frequency range of the PSD for which the dynamic behavior of the structure is unknown. This warning can be ignored or modifications can be made to the input data.


    But what happens if the warning is ignored? 


    At the basic level, a common SPECTRAL analysis is carried out. However, for those frequency ranges for which no sampling points of the transfer functions are available, the neighboring, most recently valid sampling point of the transfer function is taken and used for the additional, missing frequencies.


    It is recommended to avoid this error message by modifying input data. This entails checking the PSD definition for correctness in the first step and correcting it if necessary. If it can be assumed that the PSD definition is correct, natural frequency analysis and response analysis must be carried out at least for that frequency range for which the PSD is also defined. Figure 1 clearly illustrates this situation.


    Figure 1: Definition range for PSD and transfer function and the consequences


    A special point becomes evident in the graphic display of the equivalent stress PSD in the results evaluation if the warning is ignored: the originally defined frequency range of the transfer functions is displayed here. The PSD content from frequency ranges lying below or above this is added to the first or last sampling point, respectively.

  • What should be considered when using the user-defined temperature influence?
  • In many applications, elevated temperatures occur. In order to take these into account in the fatigue analysis, the isothermal temperature must first be specified in the node characteristics menu, either as constant value or as temperature distribution from FEA. In the next step, the influence factor „Isothermal temperature influence“ has to be activated.

    By default, the strength values are then reduced according to the „FEMFAT 4.6“ method based on the FKM guideline.

    In addition, FEMFAT offers the possibility to specify the material behavior at higher temperatures. The temperature-dependent behavior can be specified not only for the static and dynamic strength values but also for the S/N curve parameters, the Young‘s modulus and the cyclic hardening coefficient or exponent.

    However, despite all flexibility, it should be noted that not all of these input options are mandatory. The minimum requirement for using the user-defined temperature influence is the specification of the temperature-dependent values for the Young‘s modulus as well as ultimate tensile strength and alternating tensile / compressive strength. The remaining strength data are then – if not specified – automatically reduced proportionally to these values or kept constant, cp. also the following picture.


  • How to treat stresses of parabolic elements from ANSYS *.rst in FEMFAT? 
  • In the ANSYS * .rst file, no node-related results (stresses, strains, ...) are saved for the middle nodes of finite elements with parabolic shape functions. So that an analysis of these middle nodes can still be carried out in FEMFAT, the results of the adjacent corner nodes are used to determine values for middle nodes.

    For stresses this is done as follows:

    1. In the first step, the stress tensor at the center nodes is calculated component wise by arithmetic averaging of the stress tensor at the associated corner nodes. This is done immediately after reading the stresses in FEMFAT for each element with element node stresses. As a result, element node stresses are again obtained at the middle node, i.e. if the middle node belongs to several elements, the stress tensor differs from element to element.

    2. In the second step, FEMFAT requires node-averaged stresses for the base material calculation. These are determined either when the calculation starts (BASIC), when the VISUALIZER is started in the stress data dialog (BASIC) or when scratching (MAX, HEAT, SPECTRAL). The mean stress tensors of each element at the central node   are again arithmetically averaged component by component and the node-averaged stresses are obtained for the FEMFAT calculation:

    The analogous procedure applies for strains in HEAT.

    For node results, such as temperatures, the middle node values are read directly from the rst file.

  • How to use a job file in a batch job?
  • The default settings regarding influence factors and analysis parameters reflect our recommendations for the fatigue analysis. To follow your own “guidelines” in the department or in the group, you sometimes have to overwrite these defaults.

    We provided the first help with the templates in FEMFAT 5.1 (2014). They can be found in the FEMFAT installation directory / templates and include the weld sensitivity analysis, the recommended settings for GL 2010 and the evaluation of elastomers. 

    Calling and reading job files is easy with the icon on the graphical user interface  , but as such is not recorded in the ffj file. Instead, the read lines are appended to the current job file. 

    In the batch job such a call has to be inserted with the TCL / TK command "source" (the absolut path must be specified or a variable previously defined in the program must be used, as here "installation_path"):

    source $installation_path/templates/WELD_Sensitivity_Damage_gap.ffj


    The previously described use of variables with the "set" command to assign the "installation_path" the standard installation directory of FEMFAT 5.4 then looks like this:

    set installation_path „C:/Program Files/ECS/FEMFAT5.4“

    If a job in which another job was read is saved after this action, it is no longer the call of the template or the job that is saved, but the lines from the template! So you have to decide whether you want to keep / save the calculated job files or the previously prepared job file or both.

    Other TCL / TK commands that make it easier for you to design your jobs with FEMFAT can also be found in the templates for the WELD sensitivity analysis.

    However, we would like to point out again that manually edited job files are not the standard and can only be examined by our support with additional effort.