Cadfil Help Contents Page

Cadfil - Advanced filament Winding software for program generation for all type of filament winding machine.

Return to top of page

Cadfil Finite Element Analysis Interface Module

Cadfil Help Contents Link

Cadfil FEA Interface Overview

Cadfil can be used to create finite element geometry and data for import into your Analysis package. With multi-layer windings it is both is difficult and time consuming to create fibre architecture in analysis packages, On a doubly curved surface such as a dome, the angle and thickness are continuously variable. Cadfil offers a number of solutions, which currently include Nastran Bulk Data file (BDF), ESACOMP format and numerous tabular data formats. Customers successfully produce Cadfil data for use in Nastran/Patran, ABAQUS and ANSYS and other system. Cadfil deals with winding geometry and fibre architecture only, other attributes such as loads, constraints, and analysis control options need to be created by the user in the chosen analysis system. It is possible to specify material data from within Cadfil and to calculate equivalent stiffness properties for angle-ply laminates based on user specified or selected Unidirectional material properties from our material database.

The FEA interfaces can be found in the Analysis (FEA) Output option on the Utilities menu. This creates the dialog shown below. Note that where 'jobname' is used in this topic it refers to the name taken from the "FEA Data Output Name" text box. In the picture below 'JobName' is 'testBDF'.

Cadfil FEA Interfaces Dialog

On the left of the dialog a set of tick boxes for the different types of output that can be created. There are some data input field in the middle section of the dialog and some action Buttons to the right side. The Process is to pick the type(s) of output needed using the tick boxes, populate the data boxes, save the data and then click 'Calculate to create the output files'.

On the right side there are some action buttons, Help to show this topic, Open to read a parameter file that has the data and tick box status for all the entries on this dialog that has previously been saved using the Save button. Exit quits without doing anything and Calculate validates the data entered and then creates the output files requested via the tick boxes. The output options are Briefly Described Below and there is further detail in other associated help pages. An overview of the elements types and default topologies that can be output can be found here.

The input value boxes list has kept growing in number as more options have been added which has become unwieldy. The More Options button pops the list box shown below where all the input values can be found as well as additional ones. To modify a value click on the line in the data table to get an edit box.

Cadfil FEA Interfaces Dialog

Setting Material data

Each thickness th2 file refer to a material number e.g 1 or 2 etc. These material index numbers can be connected to a set of material properties for stiffness and strength in the Cadfil material database . This is described in a separate sub-topic here.

Links Sub-topic on this Page

Nastran BDF Full Shell/laminates

This creates the data output file 'jobname'_SH.BDF. This option creates a full surface shell of elements with a laminate stack created for each element. The Element resolution in the axis direction is taken from the mandrel file specified in the "master mandrel" edit box and the element resolution around the circumference is taken from the "Elements per 360" edit box. The Nastran data cards produced are MAT8, GRID, CQUAD4, CTRIA3, COORD2R and PCOMP. For normal winding programs the laminate is created for each layer with an angle ply laminate with 50% of the thickness at the + and 50% at the - wind angle. A detailed descriptions of these can be found in the MSC Nastran documentation "MSC Nastran 2012, Quick Reference Guide".

For axisymmetric bodies the laminate stack is a constant for a band around the mandrel at any particular point. Starting at the Minus X end of the mandrel the first band of element will be assign to PCOMP No 100, the next band 101 etc. Any shell elements that have no winding coverage (e.g. sometimes at the ends) get assigned PCOMP no 99 with zero thickness. An example showing the material bands is shown below

Laminate (PCOMP) Zones / Bands

An axis system (using CORD2R) is defined for every shell element (e.g. CQUAD) as a reference for the winding angles. Element number n will have axis system number n assigned for example element number 1000 will have axis number 1000, typical axis information is shown below.

Filament direction Vectors

A sample orthotropic material is added to the BDF file using a single MAT8 card or each orthotropic material index number found in the th2 files. The user should edit the BDF to add their own material data or should apply the material data property in the FE pre-processor being used. Cadfil creates geometry material data only the user will need to finish the FEM by adding load, restraint and other types of data as appropriate.

ESACOMP Full Shell/laminates

This option produces output that can be used with the Altair ESAComp(TM) software, a system for the analysis and design of composites. The output model is similar to the Nastran BDF Full Shell/laminates option. Three output files are created, '', 'mesh.nodes' and 'mesh.elements'. Because ESACOMP is expecting fixed file names Cadfil creates a folder 'Jobname'_ESCOMP_SH for these files so the are unique to the job. The first file contains 'sections' that detail the laminate stacks (angle and thickness for each laminate section referenced in the elements file), the second file is point (grid/node) data and the third contains element topologies. The user can edit the '' file to change the ESACOMP material index/indices to the materials they have setup in ESCOMP, it is also possible in ESACOMP to map a material to the material number used in the Cadfil output. The design for design is taken from the input box on the Cadfil FEA dialog, The burst may need to be changed from the sample values supplied in the file. The ERACOMP output also creates restraints on the two open ends of the winding. One end is fixed and the other contrained to be planer but to allow axial motion. A distributed axial load is also place on the end opening that is equivalent to the pressure load on the material that would close the opening. The design pressure load is also applied to the inside of the vessel. Thus the data deck from Cadfil can be run in ESACOMP with no modification needed if required.

Nastran BDF 2D Axisymmetric

This creates the output file 'jobname'_AX.BDF . A 2D model of a longitudinal section is created with planar shell elements. In an FEA system this 2D section could be rotated about the axis to produce a full 3D solid elements mesh or could be used in an Axisymmetric analysis if the loads and constraints are also rotationally symmetric. This type of analysis is very efficient for thick wall pressure vessels. The various layers and of the winding and elements within are given PSHELL identifiers that reflect the +/- angle ply and physical material for that element. An axis for the principal material direction for the angle-ply is created for each element. The Nastran data cards created are MAT1, GRID, CQUAD4, COORD2R and PSHELL. Users have used this type of file with the ABAQUS system using the Winding Plugin.

Cadfil axisymmetric fea model

The Above image shows a 2D axisymmetric model based on three winding layers, two low angle helical layers of slightly different base wind angle and extent and a double hoop layers on the cylinder part. The colour coding is showing different PCOMP (material) entries for different groups of elements.

TH2 Files refactored

The "thickness file list file" edit box contains the name of a text file whose contents are a list of TH2 thickness files that are for the layers of the full winding sequence. An example of such a file can be seen in the picture below. These thickness files are 'refactored' to create files 'JobName'001.TH2,'JobName'002.TH2,'JobName'003.TH2,... To explain further, within Cadfil you create a mandrel surface and then create a winding pattern on that surface. One of the outputs of that process is a thickness description in the 'TH2' file. The format and layout of the TH2 file can been seen in the linked topic. The file is basically a table of X, R, Angle, t/t0, Slope, ( axial and radial position XY in effect, winding angle , thickness as a multiple of the ply thickness and the slope angle in degrees of the mandrel axial section profile). When winding a thick part such as a pressure vessel it is often necessary to redefine the mandrel surface for later windings. Unfortunately adding the thickness of one layer to a mandrel to create a new mandrel does not work well because the wound surface has some small steps, bumps and discontinuities in the turn zones. Using such a surface will not create good winding programs because there will be discontinuities in the paths that make the machine motion erratic. The solution is to change the parameters for the domes to reflect the approximate effect of the thickness. A problem with this is that when you have a series of TH2 files for a series of layers there is no longer and obvious correlation between X,R positions from file to file to allow the overall multi-layer laminate to be constructed. What this option does is take a series of points along the master mandrel surface and then looking normal to the surface of the master mandrel finds the corresponding position in the profile of each of the TH2 files. It then interpolates the thickness an wind angle at that point. The refactored TH2 files have X,R coordinates that reflect the surface profile after the previous layers have been applied. All the new TH2 files have the same number of points and there is correspondence between positions, for example line 3 in the table is the same location in all the files. Refactored thickness files can be used by external processes to apply fibre architecture, for example these can be read into the ABAQUS winding plugin.

TH2 file list prompt

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

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

Grid Points/Laminate Table (_PLAM)

User Points/Laminate Table (_PLAM)

This creates the output file 'jobname'_PLAM.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. Note that these two options are very similar, you should select one or the other but not both, if both are selected you will get the former only. The PLAM file is optional but is a table containing coordinate points and an angle, thickness list for each layer at that coordinate point. This data can be useful for an alternative way of getting data into an FEA program. If you chose the user/points option you will be asked for a file name. The file chosen should be a comma separated value file. The file contains a list of coordinates with the format ID,x,y,z. So, if the part had ben meshed to include various non-axisymmetric features such as supports, ports and bosses the user could export the coordinates of the centre of each element in the mesh for which the laminate description is needed. Cadfil then create the table with ID, coordinate and thickness angle for all the points the user specified. The ID then gives the laminate an association to the original mesh. This option is discussed in more detail in the ANSYS notes but can be used with other systems where the laminate table data can be mapped onto a mesh that has been created in other software (that is, not created in Cadfil). Such mapping facilities have been created to import data from external processes such as draping simulation.

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.

Cadfil FEA unidirectional material selection Dialog

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.

Master Mandrel Name Many of the FEA options use thickness files (.TH2), each thickness file will have been associated with a mandrel profile from a mandrel file. Where a full shell model is being created the elements sizes and resolution that are good for program generation might not be ideal for an FEA model. A mandrel can be modified to refine the mesh grading if required using the Cadfil main menu mandrel edit options.

Thickness File List File This input box contains the name of a text file that is a list of thickness files. The list file must contain the names one or more thickness files (.TH2). The TH2 file described the thickness and winding angle along the length of the mandrel. The Pick File button allows an existing list file to be selected using a standard window file open/selection dialog. The Make File button opens a standard windows file open dialog and the user can then click an existing th2 file and then click OK (or to be faster double-click the file), the file dialog remains and then another th2 file scan be picked in the same way. When the selection of TH2 files is complete click the CANCEL button on the file selection dialog. You will then be asked for a name of a (.txt) file to save the list to and after the list file is saved the file name is automatically placed in the Thickness File List File data box. There is a third button b>Edit File which opens the list file in the windows text editor (normally Notepad) for manual editing or viewing if needed .

Note that the TH2 file is created during the payout path creation (currently only for Cadfil Axsym and Vessels with end caps in Cadfil Lite, and Multi-Hoop ), this link has a description of the TH2 and THK file formats. The TH2 box shown in the dialog below must be ticked and the band width (BW) and band thickness (t0) must be set correctly. The band thickness can be estimated by using tow and resin properties if the material data button is selected from the dialog

Thickness Dialog

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 (colinear) 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 ouside 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 ouput order yoyu 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 currenrty 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 loadcase on the shell surface and a distributed load around the rim of the axially free end opening.

SB Allowable interlaminar shear This value is output in BDF files in the PCOMP or PCOMPG data entries. It is the allowable interlaminar sheat 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 avialable. 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.

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 refence direction for materials. This is documented as the defalt Nastran behaviour.

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 outputng 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.

Follow this link for Details of a test case for ABAQUS

This is a link for some additional details for ANSYS