eFatigue gives you everything you need to perform state-of-the-art fatigue analysis over the web. Click here to learn more about eFatigue.

Finite Element Model Supported File Types

Three formats are currently supported:

• ABAQUS .fil
• ANSYS .rst
• Pro Mechanica ASCII .neu
• Solidworks and COSMOS/M ASCII
• eFatigue ASCII

ABAQUS FEA models are supported through the stress results in the .fil file. Both ASCII and binary formats are supported.
In addition to the plotting provided by eFatigue web site you can download the fatigue results and use your standard viewer.
The fatigue contours are exported to a newly created .fil file. The fatigue results .fil file contains one stress increment. Each tensor item contains a separate life plot. The title for the increment indicates what each tensor represents.
A sample title would be:

Supported Elements

All elements with Cartesian stress tensors are supported. This includes solids, membranes, 2-d and shell elements.

Strain Support

ABAQUS has very flexible support of strain data. The two primary strain variables are E and LE used for linear and non-linear analyses respectively. Both variables are supported.
In the case of thermal analyses strains are split into constituents caused by different phenomena. The four components are elastic strain (EE), plastic strain (PE), thermal strain (THE) and creep strain (CE). For room temperature fatigue we are only interested in the strains due to stresses, these are the elastic (EE) and plastic strains (PE).
The ABAQUS input deck controls which strain variables are written to the .fil file.
Extraction of PE and EE will take precedence over extraction of either E or LE from the .fil file.

Supported Data Locations

ABAQUS exports stress data in a number of locations. eFatigue supports the following positional data types:

• Element Nodes (Element)
• Nodal Averaged (Nodal)
• Whole Element
• Integration Points
• Element Centroidal

In reading in data the priority is as specified in the list above.
It is recommended that Element Nodes data is used as it will always include the element surface for all element types.
If a .fil file contains more than one set of positional data the list of available increments will be shown once for each set of positional data. In the example below the 4 steps are stored at 3 locations. If you wish to analyse element nodal data define the loading as 1-4. If you wish to analyse integration point data define the loading as 9-12.

Plotting Results

The ABAQUS viewer does not support contouring of .fil files. So you should load your .fil fatigue results into your standard .fil viewer in a similar manner to any structural results.
A sample Worst life plot (S_x) is shown below, The contour shows -1*LOG10(Life) - i.e. -6 is a life of 10⁶ repeats and -4 is a life of 10⁴ repeats.

ANSYS FEA data is supported via the structural results file, extension .rst. Versions 9 and above of ANSYS .rst files are supported. The .rst file must contain geometry.
In addition to the plotting provided by eFatigue web site you can download the fatigue results and use your standard viewer.
The fatigue contours are exported to a newly created .rst file. The fatigue results .rst file contains one stress increment. Each tensor item contains a separate life plot. The title for the increment indicates what each tensor represents.
A sample title would be:

Supported Elements

All SOLID, PLANE, SHELL and SOLIDSHELL elements are supported. These relate to the following ANSYS routine numbers:

Strain Support

ANSYS .rst files automatically contain the strain tensors split into elastic and plastic components. Where appropriate to the analysis the strains will be extracted and stored in the two components EE and PE.

Plotting Results

To plot the fatigue results in ANSYS perform the following steps.

• Run ANSYS
• From ANSYS Main menu pick the General Postproc menu item Results Viewer.
• This will request the .rst filename, pick the file of interest.
• On toolbar there will be a series of combo/drop-down boxes. On the left hand one select Element Solution - Stress - X Component of Stress. The component will depend upon which life contour you require.
• Press Plot Results tool. This is first tool on toolbar after drop-down boxes.

A sample Worst life (Sx) plot is shown below:

Pro Mechanica FEA models are supported through the ASCII version of the .neu file and .s01,.s02 etc stress results files.
The .neu file is used for the h-element/h-node version of the model geometry and connectivity. The .s01, .s02 etc files are used for the stress and strain data
So unlike most of the other FEA formats multiple files need to be uploaded for a Pro-Mechanica model.
When validating an FEA model the .neu file should be used.
The fatigue contours can be exported to an ASCII results file. They are also automatically exported to a eFatigue 3d plot contour that can be plotted using the eFatigue 3d viewer.

Supported Elements

All elements with Cartesian stress tensors are supported. This includes solids, membranes, 2-d and shell elements.
By default Pro-M uses tetrahedrons and octahedrons for h-element meshing. Currently octahedrons are not one of the directly supported eFatigue elements so they are stored as 2 back-to-back pyramids.

Strain Support

Pro-Mechanica strain data is supported.

Supported Data Locations

Pro-Mechanica exports all stress and strain data as Nodal Averaged (Nodal) data at h-nodes. eFatigue imports this nodal data.

Plotting Results

In addition to the plotting provided by eFatigue web site you can download the fatigue results and use the eFatigue 3d viewer.

Solidworks and COSMOS/M ASCII FEA File Format

All files associated with a Solidworks FEA analysis must be stored in a single folder/directory on the eFatigue server.
Only the files for the analysis should be stored in the folder.
It is important that you do not store more than one set of analysis results in a folder as this will cause the model validation to fail.
The files required to define an analysis are:

• the geometry file
• one component stress file for each step containing the stress tensors
• one component strain file for each step if the analysis is elastic-plastic

Geometry File

Stress Tensor Files

Strain Tensor Files

How to Export ASCII data from Solidworks

• In the simulation tree, right mouse click on the study name of interest.
• This will display a menu. Select the item 'Export...'.
• The 'Save As' dialogue box opens.
• Define a suitable filename.
• From the 'Save as type' drop down select 'Simulation Files (*.geo)'. (Note that the .geo file is an ASCII file and can be renamed to .txt after exporting).
• Click the 'Options' button, this will display the 'Export Options - COSMOSM' dialogue.
• Select the 'FEM only' radio button to export the model.
• Press 'OK' to close the 'Export Options COSMOSM' dialogue.
• Press 'Save' on the 'Save As' dialogue.

• In the simulation tree right click on the 'Results' item associated with the study name of interest. On the resulting menu select the item 'List Stress, Displacement, Strain'.
• This will display the 'List Results' dialogue.
• In the 'Advanced Options' section, select the 'Nodes' radio button. Then click on 'Range'. This allows the export of the stress results for all nodes in the model.
• In the 'Quantity' section select the 'Stress' radio button.
• In the 'List Set' select 'List normal and shear stresses'.
• In the resulatnt 'List Results' window press the 'Save' button to save to a text file.

Supported Elements

All elements with Cartesian stress tensors are supported. This includes solids, membranes, 2-d and shell elements.

Strain Support

Strain data is supported.

Supported Data Locations

Only Nodal Averaged (Nodal) data is supported for Solidworks.

Plotting Results

In addition to the plotting provided by eFatigue web site you can download the fatigue results and use the eFatigue 3d viewer.

eFatigue ASCII FEA file format

Format

The eFatigue ASCII FEA file format is a multi line ASCII file. Each line can define:

• A Nodal Location
• Element type and a list of nodes on the element
• List of Shell Layers
• An Increment - used as a wrapper for analysis data such as stresses
• Stress data for an individual node

Nodal Positions

Nodal positions are defined using the token NODAL POSITIONS. All lines that follow this line are assumed to be nodal position related until an increment or element node list definition is encountered.
Each line has 4 required items, the node and the co-ordinates of the node in XYZ order. An optional 5th parameter can be added if this node belongs to a shell, in this case the fifth value is the shell thickness at the node.
Part definitions within the positions list indicate that all the following positions apply to that part.
An example definition is:

Element Definition and Node Lists

Element definitions and node lists are defined using the token ELEMENTS. All lines that follow this line are assumed to be element definitions until an increment or position definition.
Each line has an element number, an element type and a list of nodes.
The order of the nodes is important as they are used to derive the faces on the element, a full definition of the expected element order is outlined in the Discussion of Elements section.
The valid element type descriptors are:

Pyramids are supported as collapsed ANSYS bricks, this is outlined in the Discussion of Elements section. To import models from other formats you should match the element order and faces to one of the supported element types. You can also split unsupported elements into a number of supported elements, an example would be:Octohedrons can be split into 2 pyramids or 4 tetrahedrons.

Part definitions within the element list indicate that all the following elements apply to that part.
An example definition is:

Defining Shell Layers

All of the shell layers requiring increment data should be defined in the shells list. Shell layers are defined using the token SHELL. An example definition is:

This statement would occur above the increment statement in the ASCII file.

Defining Parts

Parts are defined using the token PART. An example definition is:

Defining Increments

An increment is a snapshot of data for the model, usually stresses and strains. FEA codes have different names for this snapshot, the use of the term increment is not intended to only apply to multi-increment analyses. An ASCII FEA model should have at least one snapshot of data.
Increments are defined using the token INCREMENT. An example definition is (this should all be on one line):

Defining Element Types

Element types are used within an increment data list to indicate that the following data applies to 2-d elements, shells or 3-d (solid) elements.
If all elements are 3-d this statement is not required.
Element Types are defined using the token ELEMENT TYPE. An example definition is:

• SHELL
• 2D
• 3D

All data lines after an ELEMENT TYPE statement contain data for elements of that type. The default type is 3D. If the data type is a shell then all subsequent data lines must contain a shell number too.

Defining Data Types

Data types are defined using the token DATA TYPE. An example definition is:

Any data lines following this statement are assumed to be of this data type.
The following data types are used in the fatigue analysis process:

Data Lines

Data lines contain the data for the current increment, data type and part.
Each line contains the data for one node.
The format is (all on one line):

Example file

The following element types are supported in the ASCII FEA format:

• Shells
• 2-d/Plane
• Solid Tetrahedrons
• Solid Bricks
• Solid Weges
• Solid Pyramids

Shells

For 3 and 4 node shells elements ANSYS and ABAQUS have an identical node order. ABAQUS supports 6 and 8 node shell elements, the mid-side nodes have stresses.
ANSYS also supports 6 and 8 node shell elements however only the corner nodes (3 or 4) have stresses so using this technique for importing stress data into eFatigue is of little use.
Shells have data values (stresses) at multiple layers through the thickness of the element.
The node order of the shell element is important and should be as shown in the figure, table and example below:

Within the ASCII FEA file the ELEMENTS section of the file should contain:

• 3 node shell element with Elemental Stresses
• 6 node shell element with Nodal Stresses

2-d/Plane

For 3 and 4 node 2-d elements ANSYS and ABAQUS have an identical node order. ABAQUS also has 6 and 8 node 2-d elements, they have mid-side nodes with stresses.
ANSYS also supports 6 and 8 node 2-d elements however only the corner nodes (3 or 4) have stresses so using this technique for importing stress data into eFatigue is of little use.
The node order of the 2-d element is identical to that described for SHELL elements.

Within the ASCII FEA file the ELEMENTS section of the file should contain:

• 3 node 2-d element with Elemental Stresses
• 6 node 2-d element with Nodal Stresses

Solid Tetrahedrons

Solid tetrahedron elements are supported using both the ANSYS and ABAQUS techniques of storing these elements.
For 4 node tets ANSYS and ABAQUS have an identical node order. ABAQUS also supports 10 node tets, they have mid-side nodes with stresses.
ANSYS also supports 10 node tets however only the corner nodes (4) have stresses so using this technique for importing stress data into eFatigue is of little use.
The node order of the tetrahedron is important and should be as shown in the figure, table and example below:

Within the ASCII FEA file the ELEMENTS section of the file should either contain:

• As an ANSYS 4 node tet. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ANSYS_TET4 1 2 3 4

  
  
• As an ABAQUS 4 node tet. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ABAQUS_TET4 1 2 3 4

  
  
• As an ABAQUS 10 node tet. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ABAQUS_TET10 1 2 3 4 5 6 7 8 9 10

• ANSYS 4 node style tet with Elemental Stresses
• ABAQUS 10 node style tet with Nodal Stresses

Solid Bricks

Solid brick elements are supported using both the ANSYS and ABAQUS techniques of storing these elements.
For 8 node bricks ANSYS and ABAQUS have an identical node order. ABAQUS also supports 20 node bricks, they have mid-side nodes with stresses.
ANSYS also supports 20 node bricks however only the corner nodes (8) have stresses so using this technique for importing stress data into eFatigue is of little use.
The node order of the brick is important and should be as shown in the figure, table and example below:

Within the ASCII FEA file the ELEMENTS section of the file should either contain:

• As an ANSYS 8 node brick. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ANSYS_BRICK8 1 2 3 4 5 6 7 8

  
  
• As an ABAQUS 8 node brick. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ABAQUS_BRICK8 1 2 3 4 5 6 7 8

  
  
• As an ABAQUS 20 node brick. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ABAQUS_BRICK20 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20

• ANSYS 8 node style brick with Elemental Stresses
• ABAQUS 20 node style brick with Nodal Stresses

Solid Wedges

Solid wedge elements are supported using both the ANSYS and ABAQUS techniques of storing these elements.
The ANSYS technique is in the form of a collapsed brick, there are 6 nodes with stresses. ANSYS also supports 15 node wedges (collapsed 20 node bricks) however only the corner nodes (6) have stresses so using this technique for importing stress data into eFatigue is of little use.
ABAQUS wedges can either have 6 nodes or 15 nodes, the latter have mid-side nodes with stresses.
The node order of the wedge is important and should be as shown in the figure, table and example below:

Within the ASCII FEA file the ELEMENTS section of the file should either contain:

• Wedge elements defined as ANSYS BRICKS. Each element is defined with 3rd and 4th nodes identical and the 7th and 8th nodes identical. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ANSYS_BRICK8 1 2 3 3 4 5 6 6

  
  
• As an ABAQUS 8 node wedge. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ABAQUS_WEDGE6 1 2 3 4 5 6

  
  
• As an ABAQUS 15 node wedge. For the above figure and node numbers the definition for element 17 would be:
  
  

  ELEMENTS 17 ABAQUS_WEDGE15 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15

• Element stresses in which case there should be 8 sets of stress data for element 17, 3rd and 4th being identical, and the 7th and 8th being identical. For example:
  
  

  17 1 +2.368E-1 -2.626E-3 +6.248E-4 +8.046E-3 +6.625E-3 -9.807E-3 17 2 +1.227E-2 +1.883E-2 -2.482E-3 -3.148E-3 -8.498E-3 +1.033E-2 17 3 -4.283E-3 +2.862E-2 +8.782E-3 -9.373E-3 -1.461E-2 +1.898E-2 17 4 -4.283E-3 +2.862E-2 +8.782E-3 -9.373E-3 -1.461E-2 +1.898E-2 17 5 +1.755E-1 +2.574E-3 -9.934E-3 +1.915E-2 +7.712E-3 -1.852E-2 17 6 +4.106E-6 +9.823E-6 +1.289E-6 +7.902E-6 -4.106E-6 -1.167E-1 17 7 +4.906E-6 +7.823E-6 +6.259E-6 +3.602E-6 -5.016E-6 -1.367E-1 17 8 +4.906E-6 +7.823E-6 +6.259E-6 +3.602E-6 -5.016E-6 -1.367E-1

  
  
• Nodal stresses. In this case the stresses are associated with node numbers so there will only be 6 sets of stresses. For example:
  
  

  1 1 +2.368E-1 -2.626E-3 +6.248E-4 +8.046E-3 +6.625E-3 -9.807E-3 2 1 +1.227E-2 +1.883E-2 -2.482E-3 -3.148E-3 -8.498E-3 +1.033E-2 3 1 -4.283E-3 +2.862E-2 +8.782E-3 -9.373E-3 -1.461E-2 +1.898E-2 4 1 +1.755E-1 +2.574E-3 -9.934E-3 +1.915E-2 +7.712E-3 -1.852E-2 5 1 +4.106E-6 +9.823E-6 +1.289E-6 +7.902E-6 -4.106E-6 -1.167E-1 6 1 +4.906E-6 +7.823E-6 +6.259E-6 +3.602E-6 -5.016E-6 -1.367E-1

• ANSYS style with Elemental Stresses
• ANSYS style with Nodal Stresses
• ABAQUS style with Elemental Stresses
• ABAQUS style with Nodal Stresses

Solid Pyramids

Pyramid Elements are supported in the eFatigue ASCII FEA file in the form of collapsed bricks. The node order of the pyramid is important and should be as shown in the figure, table and example below:

Within the ASCII FEA file the ELEMENTS section of the file should contain all pyramids elements defined as ANSYS BRICKS. Each element is defined with the first 4 nodes being the base in a clockwise manner when viewed from beneath the element, and the last 4 nodes being the vertex node (all identical). For the above figure and node numbers the definition for element 17 would be:

• Element stresses in which case there should be 8 sets of stress data for element 17, the last 4 being identical. For example:
  
  

  17 1 +2.368E-1 -2.626E-3 +6.248E-4 +8.046E-3 +6.625E-3 -9.807E-3 17 2 +1.227E-2 +1.883E-2 -2.482E-3 -3.148E-3 -8.498E-3 +1.033E-2 17 3 -4.283E-3 +2.862E-2 +8.782E-3 -9.373E-3 -1.461E-2 +1.898E-2 17 4 +1.755E-1 +2.574E-3 -9.934E-3 +1.915E-2 +7.712E-3 -1.852E-2 17 5 +4.106E-6 +9.823E-6 +1.289E-6 +7.902E-6 -4.106E-6 -1.167E-1 17 6 +4.106E-6 +9.823E-6 +1.289E-6 +7.902E-6 -4.106E-6 -1.167E-1 17 7 +4.106E-6 +9.823E-6 +1.289E-6 +7.902E-6 -4.106E-6 -1.167E-1 17 8 +4.106E-6 +9.823E-6 +1.289E-6 +7.902E-6 -4.106E-6 -1.167E-1

  
  
• Nodal stresses. In this case the stresses are associated with node numbers so there will only be 5 sets of stresses. For example:
  
  

  1 1 +2.368E-1 -2.626E-3 +6.248E-4 +8.046E-3 +6.625E-3 -9.807E-3 2 1 +1.227E-2 +1.883E-2 -2.482E-3 -3.148E-3 -8.498E-3 +1.033E-2 3 1 -4.283E-3 +2.862E-2 +8.782E-3 -9.373E-3 -1.461E-2 +1.898E-2 4 1 +1.755E-1 +2.574E-3 -9.934E-3 +1.915E-2 +7.712E-3 -1.852E-2 5 1 +4.106E-6 +9.823E-6 +1.289E-6 +7.902E-6 -4.106E-6 -1.167E-1

• with Elemental Stresses
• with Nodal Stresses