#### 2.1.2.1. Materials

The Materials database is only editable within ACP in Stand Alone mode. Otherwise it draws all material properties from Engineering Data within Workbench. In this case, the material properties can only be viewed but not altered in ACP.

##### 2.1.2.1.1. Materials Context Menu

The context menu of the Materials class has the following options:

- Create Material (Stand Alone only): Open a Material Properties dialog for creating a new material.

- Paste (Stand Alone only): Paste a copied material into the material database.

- Sort: Sort the list of materials alphabetically.

- Export: Export the material database into a .CSV file, ESAComp XML file, or an ANSYS Workbench XML file.

- Import (Stand Alone only): Import materials from a .CSV file or ESAComp XML file.

More information on the import and export of ESAComp XML file can be found in ESAComp. Stackups and Sublaminates can also be exported to an ESAComp XML file format but are converted to laminates in the process.

Figure : Materials Class Context Menu in Stand Alone Mode

##### 2.1.2.1.2. Temperature Dependent and General Variable Material Properties

Engineering constants, as well as stress and strain limits, can be set to depend on scalar field variables, including Temperature, Shear Angle, and Degradation Factor. Other properties can only depend on temperature. The material properties are always show at the reference point in the Materials object. Variable material data can be edited in Workbench Engineering Data.

In ACP, variable material data are considered in ACP-Post when evaluating failure criteria. Temperature-dependence comes into effect if the solution contains a temperature data block. Shearing of plies is considered if the material is dependent on the Shear Angle variable and at least one ply is draped. All other dependencies require the respective field variable to be defined by means of look-up tables. For more information, see Material Fields and Analysis Using Variable Material Data.

Within the Workbench workflow, variable data are passed to and from ACP. In Stand-Alone mode, temperature-dependent data are passed to and from ACP if the import and export is in an ANSYS file format, such as .CDB.

General variable material properties are read only from the Workbench Engineering Data (.ENGD) file. Export and import of material data within the Materials object via .CSV or .XML file formats does not support general variable material data.

##### 2.1.2.1.3. Material Properties Dialog

In the Material Properties dialog, the following preprocessing data is required:

- Name: Name of the material.

- ρ: Density of the material.

- Ply Type: Defines the type of material (necessary for postprocessing).

  - Regular: Uni-directional reinforced material

  - Woven: Weave material

  - Homogeneous Core: Sandwich core material (for example, balsa or foam)

  - Honeycomb Core: Sandwich core material with a honeycomb pattern

  - Isotropic Material: Isotropic material and post-processed with the von Mises criterion

- Orthotropic Young's Modulus:

  - E1: In-plane, in fiber direction (fiber direction is corresponding to angle 0 for the ply's definition)

  - E2: In-plane, orthogonal to fiber direction

  - E3: Out of plane direction

- Orthotropic Poisson's Ratio:

  - ν12: In-plane

  - ν13: Out of plane, in fiber direction

  - ν23: Out of plane, normal to fiber direction

- Orthotropic Shear Modulus:

  - G12: In-plane

  - G13: Out of plane, in fiber direction

  - G23: Out of plane, normal to fiber direction

Further failure properties can be activated. Depending on the Ply Type some properties are deactivated automatically.

Note: Engineering Data can only be modified in preprocessing. Once postprocessing has been initiated the data is frozen.

##### 2.1.2.1.4. Thermal Expansion Coefficients

For thermal stress analyses, the thermal expansion coefficients of the material and the reference temperature must be given:

- Reference Temperature: Temperature at which strain in the design does not result from thermal expansion or contraction

- alpha X: In-plane, in fiber direction (fiber direction is corresponding to angle 0 for the ply's definition)

- alpha Y: In-plane, orthogonal to fiber direction

- alpha Z: Out of plane direction

##### 2.1.2.1.5. Strain Limits

The Strain Limits are used to calculate the IRF if the Max Strain criteria is selected in the failure criteria definition. Compressive strain limits must be negative.

For orthotropic materials, 9 strain limits (5 in-plane and 4 out-of-plane strains) can be entered:

- eXc: Normal strain, in-plane, in fiber direction, compression limit

- eXt: Normal strain, in-plane, in fiber direction, tension limit

- eYc: Normal strain, in-plane, orthogonal to fiber direction, compression limit

- eYt: Normal strain, in-plane, orthogonal to fiber direction, tension limit

- eZc: Normal strain, out of plane, compression limit

- eZt: Normal strain, out of plane, tension limit

- eSxy: In-plane shear strain

- eSxz: Transverse (interlaminar) shear strain, plane in fiber direction

- eSyz: Transverse (interlaminar) shear strain, plane normal to fiber direction

If the material is defined as isotropic, the von Mises Strain Limit can be entered:

##### 2.1.2.1.6. Stress Limits

All the other Failure Criteria definitions are based on values defined in the Stress Limits dialog. Compressive stress limits must be negative.

For orthotropic materials, 9 stress limits (5 in-plane and 4 out-of-plane strains) can be entered:

- Xc: Normal stress, in-plane, in fiber direction, compression limit

- Xt: Normal stress, in-plane, in fiber direction, tension limit

- Yc: Normal stress, in-plane, orthogonal to fiber direction, compression limit

- Yt: Normal stress, in-plane, orthogonal to fiber direction, tension limit

- Zc: Normal stress, out of plane, compression limit

- Zt: Normal stress, out of plane, tension limit

- Sxy: In-plane stress strain

- Sxz: Transverse (interlaminar) shear stress, plane in fiber direction

- Syz: Transverse (interlaminar) shear stress, plane normal to fiber direction

If the material is defined as isotropic the von Mises Stress Limit can be entered (equivalent to Tensile Yield Strength in Engineering Data):

##### 2.1.2.1.7. Puck Constants

The Puck failure criterion requires internal parameters, which depend on the material. The Material Classification drop-down menu offers a selection of pre-defined constants and also allows for the definition of custom constants. The menu has the following options:

- Carbon: Sets pre-defined Puck constants for carbon fiber materials.

- Glass: Sets pre-defined Puck constants for glass fiber materials.

- Material-specific: Allows you to set your own Puck constants.

- Ignore Puck Criterion: No constants are set.

- p21(+): Tensile inclination XZ

- p21(-): Compressive inclination XZ

- p22(+): Tensile inclination YZ

- p22(-): Compressive inclination YZ

- s and M: Degradation parameters

- Interface Weakening Factor: Scales the interlaminar normal strength

##### 2.1.2.1.8. Puck for Woven

The Puck for Woven functionality of ACP allows to evaluate the Puck failure criterion for woven materials. Two UD plies can be specified representing the woven ply. During the failure evaluation, ACP evaluates the stresses for theses plies and computes the Puck failures. The relative ply angles, engineering constants, stress limits and Puck constants must be defined for both plies.

Note: This specification does not affect the analysis model and is only considered in the failure analysis for the Puck criterion.

##### 2.1.2.1.9. Tsai-Wu Constants

The Tsai-Wu constants are constants used into the interaction coefficient of the quadratic failure criteria for Tsai-Wu formulation. Refer to Tsai-Wu Failure Criterion for more details.

In ACP the Tsai-Wu constants correspond to:

- 2 F12 = XY, default -1

- 2 F13 = XZ, default -1

- 2 F23 = YZ, default -1

##### 2.1.2.1.10. LaRC Constants

The LaRC failure criteria requires the following parameters to evaluate the failure in matrix and fiber:

- Fracture Angle Under Compression: The value for α0 used in the LaRC fiber and matrix failure. Default value is 53°.

- Fracture Toughness Ratio: The ratio of the mode I to mode II fracture toughness, which is used in the fiber failure criteria.

- Fracture Toughness Mode I

- Fracture Toughness Mode II

- Thin Ply Thickness Limit (set to 0.7 mm in Workbench mode)

For more information, see LaRC03/LaRC04 Constants.

Release 18.2 - © ANSYS, Inc. All rights reserved.