Cadfil Finite Element Analysis Interface Module

Refactored thickness angle table, T1

This creates the output file 'jobname'_T1.csv. This is a comma separated value (CSV) table that can be read into excel, such a table data can be applied copy/paste into an FEA system and then referenced. ANSYS Pre-Prep has such a facility. The Table headers are "x r slope Angle1 thick1 Angle2 thick2……". X,R and slope refers to the master mandrel and then there area thickness and angle entries for each layer. Thickness can be zero and please note that the thicknesses are multiples of the PLY thickness t0. The t0 and material index number can be found at the bottom of each TH2 file.

Refactored thickness table, T2

IGES file curves for T2 Table

This creates the output file 'jobname'_T2.csv. This is a comma separated value (CSV) table that can be read into excel, such a table data can be applied copy/paste into an FEA system and then referenced. ANSYS Pre-Prep has such a facility. The Table headers are "N X0 Y0 Z0 X1 Y1 Z1 X2 Y2 Z2,.....,Thick0 Thick1 Thick2,..... N is the line number starting at 1, the (XYZ)i are the points that are the outside after layer i has been placed/wound (i=0 being the mandrel). The true layer thickness are the Ti values. The XYZ are planar so typically all the Z values will be 0.0. This option also creates the output file 'jobname'_T2.igs which contains polyline curves (composite curve of line segments) for the mandrel profile and curves for the complete outside profile after each filament wound layer (FWL). These are 2D curves (Z=0) to the Cadfil axes, origin and units and can be imported into many CAD or FEA systems. An example picture of a set of curves for a dome ended vessel with several layers of helical and hoop winding is shown below after import in the Catia CAD package.

Grid Points/Laminate Table (_PLAM)

User Points/Laminate Table (_PLAM)

Nastran BDF MAT8 angle-ply table

This creates the output file 'jobname'_MAT8.bdf. This file is a Nastran bulk date with orthotropic material properties (MAT8 data card) for a series of angle ply laminates, so for example if the Wind Angle Bin Size were specified as 1 degree than 91 property entries would be created for angle ply laminates of +/-0, +/-1, +/-2,..... +/-87,+/-88,+/-89, +/-90. These are calculated using classical laminate theory from properties specified for a unidirectional composite. A Start Material ID Number is requested, so in this example if 1000 was entered then material ID's (MID's) created would be for material 1000 through to 1090 (91 entries). The material DBF can be imported into compatible system or can be applied by Cut/Paste into another BDF file.

The Unidirectional material selection is shown below. The Data comes from and excel sheet database in the Cadfil install folder. The User can enter their own material data but some sample material is supplied. You select the material required from the dropdown combo box and it then populates the dialog, clicking the save button selects that material data and then exits.

Shell model Via Continuous Grid Mapping (CGM) Method

This is a entirely new methodology for FEA model creation based on new technology introduced in Cadfil V9.66. All previous models are based on thickness files (TH2) which have calculated (for each filament wound layer) an average thickness for each axial position along the mandrel. This thickness file method is applicable only to rotationally symmetric parts. With all FEA methods some approximations are required, for example a geometry is approximated as being represented by a collection of elements of uniform property. The averaged (uniform) thickness is for the most part a reasonable assumption but is not necessarily reality. A winding layer is in fact a series of bands that are placed on the surface of the mandrel. If we consider the band (like a tape) of having a width and a constant thickness (t0) then at any point on the mandrel the thickness will a whole number (1, 2, 3,.... N) multiple of t0. Consider the three picture shown below. The in the new technology method you can see a complex variation of thickness on the dome as the bands progressively overlap more an change direction. The new technology is based on processing path files (.pay) sequentially laying the bands as they are during the actually winding and accumulating the thickness and direction information as it goes. As such, this method can process non-axisymmetric paths and can also include the material laid down in single transition (joining paths). Because the fibre structure is much more realistically represented than with using a traditional laminate description a suitable FEA system can much more accurately represent the the fibre structure and use multi-scale approaches for more accurate prediction of failure.

Shell model Ansys/HDF5 format

Cadfil FEA Interfaces data input fields

FEA Data Output Name This box contains the jobname that is the root of any files names created by the FEA interface. The Open button is used to load previously saved data that is in a .par parameter file, and the parameter file name becomes the jobname.par. This jobname.par is it is also used by the SAVE option that saves all the date entered.

Header Include file This is used for options where Cadfil creates and an output model based on bulk data such as for Nastran, Patran, Femap, Hypermesh, Optistruct,.... In these cases there are job control instructions for the solver that become before the first bulk data entry. This option value is the name of a text file whose contents will be added to the top of the bulk data. A user can make their own file or copy and edit edit some of the examples found \Cadfil\cafil9xx\Data folder. The header txt file should be in the same folder as all the other input files being used. This entry can be left empty if no header file is required. An example header is shown below for the Altair Optistruct solver. For the standard bulk data output from Cadfil that has materials restraints and pressure loads with this header the output deck can been sent straight to the Altair Optistruct solver which will then do a linear static analysis creating the defined results sets.

$$------------------------------------------------------------------------------$
$$                  OPTISTRUCT HEADER INCLUDE FILE START                        $
$$                 Optistruct Input Deck Generated by Cadfil                    $
$$                             www.Cadfil.com                                   $
$$------------------------------------------------------------------------------$
OUTPUT,OP2,FL
CSTRAIN(H3D,NDIV=3) = YES
CSTRESS(H3D,NDIV=3) = ALL
CFAILURE(H3D,NDIV=3) = ALL
ELFORCE = ALL
$
$$------------------------------------------------------------------------------$
$$                      Case Control Cards                                      $
$$------------------------------------------------------------------------------$
$
$HMNAME LOADSTEP               1"DesignPressure" 1
$
SUBCASE        1
  SPC =        100
  LOAD =       200
$
$$------------------------------------------------------------------------------$
$$                  OPTISTRUCT HEADER INCLUDE FILE END                          $
$$------------------------------------------------------------------------------$

The Materials Include File is the name of a text file that contains the users own material Cards that correspond to the material ID numbers that are defined in the TH2 files. This entry can be left blank and the materials properties specified by interactive selection for each ID from the Cadfil material database. If you are doing a series of design loops it is better and quicker to make your own material file the first time to save having to pick materials each subsequent time and maybe risk making a mistake. There is an examples text (.txt) file in the \Cadfil\cafil9xx\Data folder.

Output Axis P1/P2/P3 These three data boxes define the axis system of the FEA model output. These are specified using the Cadfil axes that are used to define the mandrel where the X axis is always the mandrel rotation axis. A discussion of Cadfil axes and origin can be found elsewhere in the help system. P1 defines the x,y,z position that will become the 0,0,0 (origin) in the output model. P2 defines the X axis direction vector in the output model so if this were 0.0 1.0 0.0 the X axis in the output would be the Cadfil Y axis. This does not need to be a unit vector. Another way to think of this is that the vector P1-P2 (unit vector P1 to P2) will become the X axis of the output model. P3 defines the output Z direction or to be more specific P1-P2-P3 define the XZ plane as P1-P3 does not have to be at 90 degrees to P1-P2. If P1-P2-P3 are in a line (co-linear) an error will result. For the mathematically minded P1 is the new origin P1-P2 is the new X direction, (P1-P2 ^ P1-P3) is the new Y direction and the new Z direction forms a right handed set.

Output System Scale The input box is a scale to change the units of the output model, so for example if the Cadfil mandrel is defined in mm but you want the output in m then use 0.001. The default value is 1.0. All coordinate positions and linear dimensions (such as thickness) will be scaled in the output.

Elements Per 360 for full shell output models this is the number of elements that will be created around a section of the mandrel in a circumferential direction.

QUAD/TRIA Node Order(topology) for full shell output models some systems expect the node order in an element in a certain way. In a Cadfil axisymmetric model when you are looking onto the outside of the mandrel the nodes on an element go in anti-clockwise order with the first two nodes being around circumferential direction (around a cross section) so the order is [1 2 3 4], this is the default topology (order). The last two nodes will be on the next mandrel section which will be in increasing X (axial) direction. We note for example that in ESCACOMP the order is also anti-clockwise but for a quad the system expects the first two notes to be in the positive axial direction as it uses these in its element axis definition. Thus you should set the output topology as [2 3 4 1]. If you wanted an clockwise output order you might use [1 4 3 2]. Cadfil may use triangular elements to close the last sections of a dome at the poles (a fan of elements) again the order is ant-clockwise looking on the outside, with the first node on the pole (x axis) and the other two nodes an the next/previous section, the default order is [ 1 2 3].

Wind Angle Bin Size For axisymmetric models the wind angle for an element is approximated to the nearest 'bin' value. So for example if then Wind Angle Bin Size were specified as 1 degree then there will be 91 bins for angle ply laminates of +/-0, +/-1, +/-2,..... +/-87,+/-88,+/-89, +/-90. If the bin size was 5 degrees then there are 19 bins 0,5,10,....80,85,90. This value is also used for the Nastran BDF MAT8 angle-ply table. The bin size is constrained to be in the 0.2 to 5.0 degree range, values outside this will give an error. If a bin size is specified that does not divide exactly into 90 degrees then it will be rounded to the nearest value that does.

4 Plys per layer. Set to YES or NO. When Cadfil creates laminates entries for a winding, the layer thickness is assumed to be 50% at the plus angle and 50% at the minus angle, ie 2 plies. If this is set to YES then we get 4 plies each 25% of the total layer thickness with the angles +/-/-/+. This gives a symmetric laminate for that wind and my give better stress results.

Design Pressure This value is used currently in ESACOMP or Optistruct data decks. In those systems the value is expected in MPa. In these systems the pressure is used to create a pressure load-case on the shell surface and a distributed load around the rim of the axially free end opening.

SB Allowable inter-laminar shear This value is output in BDF files in the PCOMP or PCOMPG data entries. It is the allowable inter-laminar shear stress that the system will use in conjunction with a failure theory. If left blank or zero Cadfil will output and empty field for this in PCOMP/PCOMPG data records. The value is in whatever units the receiving system expects, Cadfil does nothing with this value other than output it.

FT Failure Theory This box can be left blank but can be used to specify a failure theory as described in the Nastran Manual for PCOMP and PCOMPG. Valid inputs for MSC Nastran are "HILL", "HOFF', "TSAI", "STRN". These may or may not be supported by receiving FEA system or other options my be available. Cadfil does not validate this input, validation is a function for the target FEA program. Note that for solid HEXA elements in NX-Nastran using solid PCOMPS laminates the options are HILL, HOFF, TSAI, STRESS, STRAIN and MCT. If FT is set it is normal that SB also needs to be set but again you are advised to read your FEA system manual.

Material Card FT Failure Theory This box can be left blank but can be used to specify a failure theory as described in the Nastran Manual for MAT* CARDS in the NX Nastran manual (e.g. "STRN"). With MSC Nastran or Optistruct specifying a value will create a error so leave this blank.

Create element axes This takes the Value YES or NO. The default is NO. For BDF shell and Solid output if yes is set an axis is created for each element and this is then used to reference the angle for the materials in the PCOMP/PCOMP/PCOMPLS data. If NO a single axis is created and it is assumed the FEA system projects the X axis of this into the plane of the element and uses that as the reference direction for materials. This is documented as the default Nastran behavior.

Use PCOMPLS. Set to YES or NO. The default is YES. For solid elements there is a choice of PCOMPLS (MSC Nastran/Optistruct) or PCOMPS (NX Nastran) which have slightly different formulations.

'Material property output Units'. This is set to SI or SI(mm), the default is SI. This option can be used if you are using material property data for strength and stiffness from the Cadfil material (Excel) database. Data in the Cadfil database is set in strict SI units (Pa (N/m2) and Kg/m3 ). If you are outputting a model that in mm with no scaling then you can use the SI(mm) option which outputs the MAT8 cards in (N/mm2 (MPa) and Kg/mm3) rather than strict SI. At present this option does not support Imperial (Inch) based unit systems.

Minimum Solid thickness' When creating a Solid HEXA mesh the thickness of an element can vary at each corner of the inner shell face. When we are at the end of the winding, that is the element edge is in no man's land between a place where we have material and no material the system interpolates a thickness. This can lead to an anomaly where we have a element edge that has near zero thickness which can create an invalid element with respect to geometric checks etc. This option allow the user to specify the minimum thickness to uses when the real thickness is tapering away to zero in such a case. The default value is 0.0

'YES to use PCOMPG otherwise use PCOMP' This takes the value YES or NO, the default is YES. Where a bulk data shell model is being created the laminate data is output in PCOMP or PCOMPG cards. They are basically the same except PCOMPG is better if the target system supports that. With PCOMPG a unique global ply ID is given for each layer. This ID gives the systems that uses the data the knowledge of which plys are continuous across an element boundary. For example the 5th ply on one element might be the 1st ply on the next because 4 plies have stopped. In Some system it is also useful when post-processing as one can analyse the performance of a specific winding layers as each has it's own global ply ID.

CSV Separator This Option takes a single character that will be used as the separator. When Outputting CSV (comma separated values) files such as for the T2 T2 or PLAM files, the data entries are normally separated by a comma ",". When this file type is read into Excel it separates the values into different cells to make a table using the commas. This works well in my world (the UK) but on some PC's Excel will read all the data into column number one because comma is not the default separator on that PC. This often occurs on machines set for countries that use comma as a decimal separator (e.g between the Euros and the Cents). Often in such cases the semicolon ";" is used the separator. The issue can be confusing as often the relevant setting in windows is not in Excel it is hidden away in the Language County and Region settings in the Windows control panel (settings). Look in system regional setting for a setting called called List separator to determine which default delimiter to use. We have found the behaviour from different combinations of Windows and Excel version very confusing. If you change the setting you may also need to restart the PC. If this is causing you a problem one way that sometimes works for Excel. add a new line at the top of the file with the text "sep=," (including quotes) in order for Excel to open the file with "," as the list separator.

(_AX) Model axial mesh Xstep value FEA-AX-STEP is used for the _AX , _CYSYM models or for the _T1 table. The table positions / element axial divisions are set to this value. If 2.5mm is set for example the mesh spacing along the mandrel profile will be 2.5mm. For some types of model this parameter will need to be selected very carefully considering items such as layer thickness, model size and accuracy of the thickness distribution changes particularity in turnaround areas. If in doubt try some different values and look at the mesh created, it will only take a few minutes.

AX Steps From Master Mandrel FEA-AX-MASTR is used for the _AX and _CYSYM models. Read the topic above. If this is set to YES (the default is NO) the axial discretisation (size) of the elements in each filament wound layer is taken directly from the mandrel points in the master mandrel specified and FEA-AX-STEP value is not used. Care must be taken in setting up a suitable spacing that will represent changes in thickness and angle in areas where that changes rapidly. Using this method allows more user control and can be useful when the liner assembly is being meshed separately and a marriage of two meshes (liner and composite) needs to be made in the FEA Pre-process software being used.

Add Hypermesh Comments This takes the value YES or NO. If you are using Altair Hypermesh/Hyperworks these are very useful as they label (give meaningful names) and organise the model features for easier use. For example the elements get grouped (COMPONENTS) and Tagged by FWL (filament winding layer number), and COMPONENTS maybe get put into an assembly. As these lines in the bulk data all start with the $HM they will be just treated as comment lines and otherwise ignored by systems that do no use them. If you don't want them set this variable to NO.

3D Material Card type This specified the data card Cadfil will output if Solid elements are used in bulk data. It takes the values MATORT, MAT9OR or MAT11, the default is MATORT. This option is because MSC Nastran (MATORT), NX Nastran (MAT11) and Optistruct (MAT9OR) all use different data formats for specifying an orthotropic material based on Engineering constants. You should refer to the manual for the FEA system that you use. Cadfil only uses this option if solid elements are being output and also only of materials from the Cadfil database are being used. More generally you can specify your own data-cards and data using a material include file. Please note that the Cadfil database only has 4 engineering constants for a UD material (E1 E2,Nu G) but a 3D material can have more constants so some assumptions are made for example E3 = E2. It is down to use user to check and validate any material data used and indeed specific test data for your own materials are the safest choice.

Output Pressure Loads Y/N The FEA-PLOADS option takes the values YES or NO, the default is YES. If NO is selected any relevant FEA output option that would normally includes loading data will have that data removed if that is possible. This option is primarily for bulk data type output and may be helpful if the Cadfil model is being combined with external FEA models such as a liner model for example.

Output Boundary Conditions Y/N The FEA-BCONDNS option takes the values YES or NO, the default is YES. If NO is selected any relevant FEA output option that would normally includes boundary conditions such as SPC data (restraints) will have that data removed if that is possible. This option is primarily for bulk data type output and may be helpful if the Cadfil model is being combined with external FEA models such as a liner model for example.

Output Laminates Data to BDF Y/N The FEA-LAMINATS option takes the values YES or NO, the default is YES. If NO is selected any relevant FEA output option that would normally includes laminates /section data is not output. this is primarily for SHELL models where a clean geometry model is needed for some reason.

Output Flavour Setting The FEA-FLAVOUR option is discussed in an earlier section, it can also be set in the pull down list box option. If you set the flavour in either location it will be also in both locations to match.

Set/Group Lists in full(expand range) Y/N The FEA-EXPD-RNG option takes the values YES or NO, the default is NO. This option is used selectively in some (annoying) cases (yes you ABAQUS...) where specifying node or element sets quite validly in a range for example 10 to 20 inclusive works OK for the solver however the CAE rejects it as a data error because they were too lazy to support there own data forms in full. Anyway if this is set to YES set and if there is a problem known to us at Cadfil, Cadfil will expand the ranges as a list and bloat out your datadeck with what is in some cases thousands of extra lines of data.