Define a Simulation Composite Analysis Material

Use the COMPAN command to define a composite material.

In an ANSYS input file, there is one command that collectively defines a Simulation Composite Analysis user-defined composite material. This command is COMPAN. Consider the following line from an ANSYS input file that completely specifies a user-defined composite material. 

COMPAN, MATID, NSTATV, UNITS, PFIB_DIR, PFA, PREFAIL, unused, PRESS, TEMP,FAIL_CRITERION,AUX_1,AUX_2,unused, MDEG, FDEG, MOISTURE

An example of a COMPAN command looks like: 

COMPAN,9007,7,1,1,1,0,,,650,0,,,,0.01,0.01,2

The COMPAN command calls the Simulation Composite Analysis macro and the arguments provided as part of the COMPAN command are passed to the macro. For any given Simulation Composite Analysis material, the number of arguments must be between 5 and 16. The first five arguments are required for all Simulation Composite Analysis materials. Arguments 7 and 13 are unused and should be left blank or set to 0. Appendix A provides a detailed description of each of the arguments, including the range of allowable values for each argument and the impact that each argument has on the multiscale constitutive relations used to represent the material. Each argument is shown in the table below and is given a brief description. For a more detailed description of any particular argument, refer to the appropriate section of Appendix A.

  1. MATID - The 1st argument allows you to specify a material reference number to be associated with a Simulation Composite Analysis material. When the product is installed for ANSYS, an ASCAMatDB.xml file is created in the %AUTODESK_DIR%\Materials directory (C:\Program Files\Autodesk\Simulation Composite Analysis 2015\Materials, for example). The purpose of this file is to link the material reference number (MATID) with the name of a material stored in the %AUTODESK_DIR%\Materials directory. The material reference numbers for the composite materials that come with the Simulation Composite Analysis install are already included in this file.

    If a new material file is created using Composite Material Manager, the ASCAMatDB.xml file is automatically updated to include the new material and is assigned a material ID number. However, if the material files are manually copied and edited, the ASCAMatDB.xml file must be updated to include the new link between the material reference number (MATID) and the name of the newly created composite material. If the ASCAMatDB.xml file is opened using a text editor or internet browser, the contents will look similar to the following:

    <?xml version="1.0"?>

    < ASCAMatDB>

    <Material id="9001" name="AS4-3501-6"/>

    <Material id="9002" name="AS4_3502"/>

    <Material id="9003" name="AS4_8552"/>

    <Material id="9004" name="AS_Epoxy1"/>

    <Material id="9005" name="Eglass21xK43Gevetex-LY556"/>

    <Material id="9006" name="HTS150_TC250"/>

    <Material id="9007" name="IM7-977-2"/>

    <Material id="9008" name="IM7_5250-4"/>

    <Material id="9009" name="IM7_8551"/>

    <Material id="9010" name="IM7_8552"/>

    <Material id="9011" name="IM7_977-3"/>

    <Material id="9012" name="S2_Glass_Epoxy2"/>

    <Material id="9013" name="SilEglass1200tex-MY750"/>

    <Material id="9014" name="T300-BSL914C"/>

    <Material id="9015" name="T300_976"/>

    <Material id="9016" name="T300_PR319"/>

    <Material id="9017" name="T800H_3900-2"/>

    </ ASCAMatDB>

    To add a link between a newly created material file and an ANSYS material reference number, copy the format of the existing file to add an additional line that links the two items. For example, if the newly created material file was saved as example_composite_material, the file would be modified as:

    <?xml version="1.0"?>

    <ASCAMatDB>

    <Material id="9001" name="AS4-3501-6"/>

    <Material id="9002" name="AS4_3502"/>

    <Material id="9003" name="AS4_8552"/>

    <Material id="9004" name="AS_Epoxy1"/>

    <Material id="9005" name="Eglass21xK43Gevetex-LY556"/>

    <Material id="9006" name="HTS150_TC250"/>

    <Material id="9007" name="IM7-977-2"/>

    <Material id="9008" name="IM7_5250-4"/>

    <Material id="9009" name="IM7_8551"/>

    <Material id="9010" name="IM7_8552"/>

    <Material id="9011" name="IM7_977-3"/>

    <Material id="9012" name="S2_Glass_Epoxy2"/>

    <Material id="9013" name="SilEglass1200tex-MY750"/>

    <Material id="9014" name="T300-BSL914C"/>

    <Material id="9015" name="T300_976"/>

    <Material id="9016" name="T300_PR319"/>

    <Material id="9017" name="T800H_3900-2"/>

    <Material id="9018" name="example_composite_material"/>

    </ASCAMatDB>

    The value 9018 would be used as the first argument in the COMPAN command and tells Simulation Composite Analysis to use the material "example_composite_material".

  2. NSTATV - The 2nd argument is used to identify the number of solution-dependent MCT state variables (SVARS) that must be tracked at each integration point in the finite element model. The number of solution-dependent MCT state variables is dependent upon whether or not you desire access to constituent average stresses and strains and the microstructure of the composite (unidirectional or woven). Allowable values for this argument are 7 or 35 for unidirectional materials and 7 or 90 for woven materials. 7 state variables should be requested unless you desire access to the constituent average stresses and strains. In this case, 35 state variables should be requested for unidirectional materials and 90 state variables should be requested for woven materials.
  3. UNITS - The 3rd argument specifies the system of units that should be used in computing the constitutive relations and stresses. In the example provided above, the third argument has a value of 1, indicating that the constitutive relations and stresses should be computed in the default system of units (N/m/K). There are three other systems of units (2 → N/mm/K, 3 → lb/in/°R, and 4 → lb/ft/°R) that can be requested via specific values of the 1st argument. There is also a custom (or user-defined) system of units which would be specified using the value of 5. For instructions on the creation of a custom set of units, refer to The HIN File section.
  4. PFIB_DIR - Simulation Composite Analysis expresses constitutive relations and computes stress in the principal material coordinate system of the composite material. The 4th argument specifies the specific orientation of the principal material coordinate system that will be used by the software.
    • Unidirectional Microstructures: The default principal material coordinate system is oriented with the '1' direction aligned with the fiber direction, while the '2' and '3' directions lie in the material's plane of transverse isotropy. However, in situations where it adds convenience or simplicity to the model creation process, you may change the orientation of the principal material coordinate system so that the '2' direction is aligned with the fiber direction, while the '1' and '3' directions lie in the composite material's plane of transverse isotropy. The numerical value (1 or 2) of the 4th argument specifies which of the principal material coordinate axes will be aligned with the fiber direction.
    • Woven Microstructures: The default principal material coordinate system is oriented with the '1' direction aligned with the fill tow direction, while the '2' direction corresponds to the warp tow direction and the '3' direction corresponds with the out-of-plane direction. However, in situations where it adds convenience or simplicity to the model creation process, you may change the orientation of the principal material coordinate system so that the '2' direction is aligned with the fill tow direction, while the '1' direction corresponds to the warp tow direction. Additionally, you may change the orientation of the principal material coordinate system so that the '3' direction is aligned with the fill tow direction while the '2' direction corresponds to the warp tow direction.
  5. PFA - The 5th argument activates or deactivates the progressive failure analysis feature. If the progressive failure feature is activated, Simulation Composite Analysis will routinely evaluate both the matrix and fiber failure criterion to determine if either constituent material has failed. Each constituent failure criterion is based on the corresponding constituent average stress state. In the event that one or both of the constituents fail, the stiffnesses of the failed constituent(s) and the stiffnesses of the composite are appropriately reduced to the respective post-failure stiffnesses.
    • Unidirectional Microstructures: A value of 1 activates the progressive failure analysis feature, while a value of 0 deactivates the progressive failure analysis feature.
    • Woven Microstructures: A value of 0 deactivates the progressive failure feature. A value of 1 activates the progressive failure feature and uses the matrix and fiber degradation levels from the material data file to calculate the failed material properties. A value of 2 activates the progressive failure feature and uses the matrix and fiber degradations levels specified by the 14th and 15th arguments to calculate the failed material properties. Selecting a value of 2 for plain weaves will add approximately 45-60 seconds to the pre-processing time per woven material. A value of 1 will not add run-time during pre-processing because the failed material properties (at the matrix and fiber degradation levels specified during material creation in Composite Material Manager) are already stored in the material file.
  6. PREFAIL (optional, for unidirectional composites only) - The 6th argument activates or deactivates the pre-failure nonlinearity feature. A value of 1 activates the pre-failure nonlinearity feature, while the default value of 0 deactivates the pre-failure nonlinearity feature. When the pre-failure nonlinearity feature is activated, Simulation Composite Analysis explicitly accounts for the nonlinear longitudinal shear stress/strain response typically observed in unidirectional fiber-reinforced composite materials. The pre-failure nonlinearity feature imposes a series of discrete reductions in the longitudinal shear stiffness of the matrix constituent material, causing the composite material's nonlinear longitudinal shear response to closely match experimentally measured data. It should be emphasized that the pre-failure nonlinearity feature only affects the longitudinal shear moduli of the composite (i.e., vs. , and vs. ), while the responses of the other four composite stress and strain components remain unaffected by this feature. Also, the pre-failure nonlinearity feature will not alter the shear stress level at which the composite fails; however, it will result in an overall increase in longitudinal shear deformation of the composite prior to failure.
    Note: The pre-failure nonlinearity feature is only available for unidirectional composite materials. This feature is ignored by woven composites.
    Note: The pre-failure nonlinearity feature is only available for unidirectional composites where a longitudinal shear stress/strain curve was supplied during the MCT material characterization process. If this feature is requested for a composite material characterized without a longitudinal shear stress/strain curve, an error message is issued at runtime and execution halts. For more information on using measured longitudinal shear data during the material characterization process, please refer to the Material Manager User's Guide.
  7. Argument 7 is unused.
  8. PRESS (optional, for unidirectional composites only) - The 8th argument activates or deactivates the hydrostatic strengthening feature. A value of 1 activates the hydrostatic strengthening feature, while a value of 0 deactivates the hydrostatic strengthening feature. If the hydrostatic strengthening feature is activated, Simulation Composite Analysis explicitly accounts for the experimentally observed strengthening of the composite in the presence of a hydrostatic compressive stress. If the hydrostatic compressive stress in the matrix constituent exceeds a threshold value, the strength of both the matrix and fiber constituents are scaled upwards commensurate with the level of hydrostatic compressive stress level in the matrix constituent.
    Note: The Hydrostatic Strengthening feature is only available for unidirectional composite materials. This feature is ignored by woven composites.
  9. TEMP - The 9th argument is used to specify the temperature value corresponding to the environment in the material data file (mdata file) to be used in the analysis. For example, if the mdata file contains environments characterized at 600, 650, and 700 R, and the value of the 9th argument is 650, the properties stored at 650 R are used in the analysis. The temperature value, along with the moisture flag (argument 16) are used to fully specify the environment to be used in the analysis. If the mdata file contains a single set of properties, the 9th argument can be left blank.

    If the value of the 9th argument is set to -1.0, the temperature dependence feature will be activated. When temperature dependence is active, Simulation Composite Analysis linearly interpolates the composite and constituent properties for any given temperature that lies within the bounds of the lowest and highest temperature points stored in the material file. Material properties stored at the lowest temperature datum are used for temperatures below the lowest stored temperature datum (the software will not extrapolate properties beyond the bounding stored temperature data points). The same is true for temperatures above the highest stored temperature datum. For further information on the use of temperature dependent material properties, refer to the Theory Manual.

  10. FAIL_CRITERION - The 10th argument specifies the criterion to use to evaluate failure initiation in the composite material. For unidirectional composites valid values are:

    -1. User

    0. MCT

    1. Max Stress

    2. Max Strain

    3. Tsai-Hill

    4. Tsai-Wu

    5. Christensen

    6. Hashin

    7. Puck

    8. LaRC02

    Woven composite materials can use the following values for the criterion flag:

    -1. User

    0. MCT

    1. Max Stress

    2. Max Strain

  11. AUX1 - The 11th argument specifies parameters for some of the auxiliary failure criteria. If Tsai-Wu is selected this constant represents the cross product term, f*. If Hashin is selected this constant represents the contribution of longitudinal shear stress to the fiber failure criterion, α.
  12. AUX2 - The 12th argument specifies parameters for some of the auxiliary failure criteria. If Tsai-Wu is selected this constant represents the optional equibiaxial stress at failure (σ11 and σ22 combined). This value can be left as zero if it is unknown.
  13. Argument 13 is unused.
  14. MDEG - The 14th argument is a fraction used to define the damaged elastic moduli of the matrix constituent after matrix constituent failure occurs. Specifically, the value is the ratio of the failed matrix constituent moduli to the unfailed matrix constituent moduli. A value of 0.1 would specify that after a matrix failure occurs at an integration point, all six of the matrix constituent moduli ( , , , , , ) are reduced to 10% of the original undamaged matrix constituent moduli. The matrix post-failure stiffness value must be greater than 0, and less than or equal to 1. If the fourteenth argument is not specified, the default value of 0.1 is assumed.
  15. FDEG - The 15th argument is a fraction used to define the damaged elastic moduli of the fiber constituent after fiber constituent failure occurs. Specifically, the value is the ratio of the failed fiber constituent moduli to the unfailed fiber constituent moduli. A value of 0.01 would specify that after a fiber failure occurs at an integration point, all six of the fiber constituent moduli ( , , , , , ) are reduced to 1% of the original undamaged fiber constituent moduli. The fiber post-failure stiffness value must be greater than 0, and less than or equal to 1. If the fifteenth argument is not specified, the default value of 1E-06 is assumed.
  16. MOISTURE - The 16th argument is specifies the moisture flag corresponding to the environment in the material data file (mdata file) to be used in the analysis. Set this argument to 0 for ambient, 1 for dry, and 2 for wet moisture conditions. For example, if the mdata file contains environments characterized at ambient, wet, and dry moisture conditions, and the value of the 16th argument is set to 1, the properties for the dry moisture content(s) are used in the analysis. The moisture flag and the temperature value (argument 9) are used to fully specify the environment to be used in the analysis. If the mdata file contains a single set of properties, the 16th argument can be left blank.
Parent topic: Use a Text Editor to Convert Pre-Existing ANSYS Input Files for Use with Simulation Composite Analysis