Under Analysis Settings, set the desired values for:
Mean Stress Correction (default = None).
Multiaxial Assessment (default = Auto). Multiaxial Assessment provides information about how the stress state varies throughout the loading history. There are three assessment options:
- If is selected, no multiaxial assessment results are produced and the Combination Method setting is exposed (see below).
- This method is a more recent development that provides a more robust measure of the biaxiality and non-proportionality of the local loading (stress state).
- mode uses a two-pass approach, which overrides the Combination Method setting. The option is not compatible with analysis.
Combination Method (default = Abs Max Principal). The analysis engine uses the information from the load provider to create a stress tensor history σij(t). In order to make a fatigue calculation, you need to reduce this stress tensor to a scalar value so that you can cycle-count it and compare the resulting cycles to the local S-N curve. This process is called stress combination. The available options for combined stress parameters are as follows:
- The Absolute Maximum Principal stress is defined as the principal stress with the largest magnitude.
- The Signed von Mises stress is the von Mises stress, but forced to take the sign of the Absolute Maximum Principal stress. and analysis do not support this method.
- The normal stress is calculated and rainflow is counted on multiple planes. The critical plane is the plane with the highest predicted fatigue damage. For stresses flagged as 2D, the planes on which the normal stress is determined have normals that lie in the plane of the physical surface (in the x-y plane of the 2D stress results coordinate system). The orientation of each plane is defined by the angle f made with the local x-axis.
Elastic-Plastic Correction. If the Analysis Type is set to
Strain Life, the Elastic-plastic Correction option is exposed. Choose betweenNeuber,Hoffmann-Seeger, orNoneoptions. TheNoneoption should be used when plastic stress or strain are present.Note: The
Noneoption is only available for Ansys Mechanical Premium or Ansys Mechanical Enterprise license.For Stress Life analysis, if the .rst files used for loading contain plastic results, check the results carefully. The add-on notifies you by issuing the warning message: "FE contain plastic stress/strain results, which are invalid for SN fatigue. Check results carefully."
For Strain Life analysis, if the .rst files used for loading contain plastic results, use the
Noneoption or check results carefully. The add-on notifies you by issuing the warning message: "FE contain plastic stress/strain results. Set the Elastic-Plastic correction to None for accurate results. This option is not available with PRO license. Check results carefully."Note: For the Analysis Type, if MultiAxial Assessment is set to , then the Elastic-plastic Correction used by the nCode solver will be , regardless of any manual setting. A different Elastic-plastic Correction method for this scenario would only be considered for the calculation.
Large Displacements (default = No). If an FE model has been solved with large displacements then this must be taken into account when performing stress transformations such as when resolving the stress to the surface or calculation of averaged nodal stresses. This option should be set to when large displacements are present, and in order to use this option the model displacements must be included in the FE results. The default value for this option is and this option should only be used when necessary because it will result in a slower analysis. The Large Displacements option is not supported for the Analysis Type.
Stress Gradients (default = Off). This property has two possible values:
- no stress gradient correction is applied.
- a correction for stress gradients is applied if stress gradients are present.
When the option is set, the Stress Gradient Method option is displayed. This property has two possible values:
(default) - Stress gradient corrections are based on a scalar measure of stress (see Stress Gradients above).
- The stress gradient calculation can also be based on the absolute maximum principal stress. In this case, the gradient of the AbsMaxPrincipal stress is determined in the surface normal direction and this is normalised with respect to the AbsMaxPrincipal stress at the surface.
To visualize the stress gradient factors, insert an Other Results result object under the Solution and set the Result Type to . Note that the nCode Material Type must be defined through materials assignment, or the nCode solver will generate the following error message when trying to solve:
Material type not supported for auto stress gradient correction : 0
Solution Location (default = ). This option can only be changed for and analysis types. If Solution Location is set to , the nCode solver will look for stress results from solid elements. The stress tensor at the weld toe will be obtained by extrapolation of the surface stress from 2 or 3 points near to the weld.
When Solution Location is set to , some additional properties need to be set:
Offset Type: Defines whether the hotspot stress extrapolation is dependent on the plate thickness. Set this to to calculate the offset based on weld thickness. Set it to to offset points by a fixed distance in mm.
Extrapolation Points: Whether to use linear (two-point) or quadratic (three-point) extrapolation.
Maximum Weld Depth: The maximum weld depth in the units of the .rst file (length). Only visible when the Offset Type (above) is set to .
Mesh Quality: Whether to use linear (two-point) or quadratic (three-point) extrapolation. Only visible when Offset Type is set to and only considered when Extrapolation Points is set to .
Offset Method: Defines which method to use to specify the offset values used in the hot spot stress calculation. Set this to to use software-defined distances and ratios. Set it to to specify a user-defined, comma-separated list of distances or ratios.
Offset Values: Comma separated list of two or three distances (mm) or ratios. Only valid when Offset Method is set to .
Weld Definition File Name: The name of the weld definition .xml file. When the Weld Definition File Name is loaded, the number of weld lines is detected and these are populated in the tabular data so that they can be mapped to the corresponding material.
Maximum Weld Depth. This option sets the maximum depth to go into the model when defining the results locations within solid elements. It is therefore only available for the analysis type. If the value is set to zero, the maximum depth will be the total thickness at each weld location. Any value entered must be > 0.
Scale Factor (default = 1).
Calculate Safety Factor (default = No). This option sets the back calculation method. This safety analysis method corresponds to the Scale Factor back calculation mode in DesignLife and should not be confused with the stress-based factor of the safety analysis engine.
This method corresponds to the Strain Life glyph's back calculation capabilities to assess how the stress should be increased or decreased to meet the target life. This is called a back calculation because you know the fatigue life and want to calculate the stress level, which would normally be an input parameter. This type of back calculation provides quantifiable stress or strain reduction targets for redesign or countermeasures.
The back calculation method is also possible with a Duty Cycle (see Create a Loading Event) as follows:
If EventProcessing is set to , then back calculation is done separately for each event.
Then, if OutputEventResults is set to , a scale factor is reported for each event. The scale factor result for the whole duty cycle is taken to be the lowest scale factor from any event.
If EventProcessing is set to one of the combination methods, then back calculation is done over the whole duty cycle.
Note: If Calculate Safety Factor is set to and there is a duty cycle, the Combination Method cannot be set to .
Certainty of Survival (default = 50.0). The certainty of survival is a real number that specifies the certainty of survival based on material data scatter. The certainty of survival (in %) allows statistical variations in material behavior to be taken into account. As mentioned in the nCode DesignLife guide, the usual application of this is to provide a more conservative prediction to ensure a safer design. The variability in material properties is characterized by standard error parameters, which should be determined when fitting material curves to Strain-Life and Cyclic Stress-Strain test data. The certainty of survival values are converted into a number of standard errors using the lookup table and this is used to adjust the cyclic stress-strain and strain-life curves, as described previously.
This value must be >= 0.00003 and <= 99.99997.
Safety Factor Analysis Settings:
Factor of Safety Type. This property is specific to the analysis type.
For Haigh curves, the safety factor can be calculated based on a constant R ratio or a constant mean stress. The calculation of the safety factor is based on the distance of the mean stress/stress amplitude from the Haigh constant life line.
The available options are as follows:
- The distance is calculated by starting from the zero stress amplitude axis and going vertically through the point to intersect the line, keeping the same mean stress.
- A line is drawn from the origin through the stress point and extended until it intersects the Haigh curve.
- The distance is calculated by starting from the zero stress amplitude point and going vertically through the point to intersect the line, keeping the same minimum stress on a plot of maximum vs. minimum cycle stress.
- The distance is calculated by starting from the zero stress amplitude point and going vertically through the point to intersect the line, keeping the same maximum stress on a plot of minimum vs. maximum cycle stress.
Target Life. This property is specific to the analysis type. This is the target life that is used to calculate the allowed stress value used in the safety factor calculation.
When Haigh curves are used, the Target Life is used to interpolate a single curve for the required life. If a single Haigh curve is selected and the life does not match the Target Life, this will cause an error.
Max Safety Factor. This property is specific to the analysis type. This is an adjustment to improve the plot.
Short Fiber Composite Analysis:
Orientation Tensor File: Specifies an ASCII/XML file containing material orientation tensors.
Composites, in general, have anisotropic structures and properties. The material orientation tensor describes the microstructure in terms of the distribution of fiber orientations at each calculation point (element, layer, section point) in the structure, and this information is required if nCodeDT is to take into account the anisotropy of fatigue properties in the analysis. The material orientation tensor will normally be derived from a simulation of the manufacturing process. The nCode MaterialOrientationTensor property is set to and the file specified by Orientation Tensor File must be in this Glyphworks-compatible CSV format:
#HEADER #CHANTITLE Orientation Tensors #TITLES Element,Layer Number,Section Point,a11,a22,a33,a12,a23,a13 #KEYWORDS ElementID,LayerNumber,Section Point,a11,a22,a33,a12,a23,a13 #DATATYPES LONG,LONG,LONG,FLOAT,FLOAT,FLOAT,FLOAT,FLOAT,FLOAT #DATA 1,1,1,0.9483,0.04747,0.004257,-0.003031,2.619E-5,-0.005304 1,2,1,0.7847,0.209,0.006283,-0.002284,-3.154E-5,-0.003902 1,3,1,0.5095,0.4853,0.005148,-7.342E-4,-2.02E-5,-0.003999 1,4,1,0.2087,0.7901,0.001193,0.007548,2.444E-5,-0.002749
Columns with these keywords and types must be present:
ElementID (Element ID) - long or huge
LayerNumber (Layer Number≥1) - long or huge
Section Point (Section Point≥1) - long or huge
a11 - (orientation tensor component) float or double
a22 - (orientation tensor component) float or double
a33 - (orientation tensor component) float or double
a12 - (orientation tensor component) float or double
a23 - (orientation tensor component) float or double
a13 - (orientation tensor component) float or double
Metadata can optionally be used to set a default orientation tensor. This is used for any locations not present in the data section of the file. If required, it must be placed in the header with this format:
#TESTMETADATA "OrientationTensor.Default,1,0,0,0,0,0"
This specifies a property set named OrientationTensor with a string property named . The tensor must be specified as a comma-separated list of six numeric values.
Solve Process Settings:
Number of Analysis Threads (default = 4): More than four threads requires an Ansys nCode DesignLife Parallel Add-on license.
The Number of Analysis Threads property can be used to set the number of threads for a job or an individual run. For a distributed job, this count will apply to each process that comprises the job. This property corresponds to the NumAnalysisThreads parameter in the input.dcl file consumed by the nCode solver.
Number of Translational Processes (default = 2): This property controls the number of processes used simultaneously during the translation process. It corresponds to the NumTranslationProcesses parameter in the input.dcl file consumed by the nCode solver.
Use MPI (default = No): When set to , this enables distributed solution through MPI. See Distributed Solve with MPI for more information.
MPI nodes. The total number of nodes to use for MPI (see above).
Host 2. The name of the second host for the MPI distributed solution (see above).