About Material Parameters
A part created in Creo Parametric 7.0 and later can contain multiple solid bodies where each body can have its own material assignment. A part created in an earlier release of Creo Parametric contains one body and one material is assigned to the part.
All parts opened or created in Creo Parametric 7.0 and later have the system parameter PTC_MASTER_MATERIAL. The default value of this parameter is PTC_SYSTEM_MTRL_PROPS. In legacy parts, the value of PTC_MASTER_MATERIAL is the material assigned to the part.
The density parameter for any material is PTC_MASS_DENSITY.
All bodies have the system parameter PTC_ASSIGNED_MATERIAL. The default value of this parameter is PTC_MASTER_MATERIAL. You can also explicitly assign a material to a body.
Set the configuration option enable_multi_material_model to the default value, yes, to explicitly assign materials to bodies.
Creating Material Data
You can create and modify material data using the Materials and the Material Definition dialog boxes. The material data can be saved to the model or saved to material data files that have a .mtl extension. The .mtl files are stored in the material library directory. Each file contains the name of the material and a set of material parameters identified by an ID and containing information on parameter value units.
User-defined material definitions are parameters that you define on the User Defined tab in the Material Definition dialog box. All other parameter values that you define through the Material Definition dialog box are stored as reserved parameter values. If you define a user-defined parameter that has the same name as a reserved parameter, Creo Parametric issues a warning.
Note the following points about material parameters:
You can use values of material parameter in relations.
You can assign materials to family table instances by adding the PTC_MASTER_MATERIAL parameter to the family table.
When you save a material, parameters with default values are saved only when you have changed the default value. Additionally, only parameters that are valid for a specified material type are saved, for example, the Orthotropic Young's Modulus is not saved for an isotropic material definition.
Reporting Material Data
The system parameter PTC_REPORTED_MATERIAL is used to report materials in the BOM table and to view all materials assigned to the part. You cannot edit this parameter. You also cannot use it in relations. At part level, the parameter PTC_REPORTED_MATERIAL reports all the materials assigned to all bodies in that part. At body level, this parameter reports the actual material assigned to the body.
At body level, if no explicit material is assigned to the body, the parameter PTC_REPORTED_MATERIAL reports the master material of the part. If no master material is set for the part, it reports an empty cell.
Legacy Parameters
In Creo Parametric 7.0 and later, we recommend that you use the parameters PTC_MASTER_MATERIAL and PTC_MASS_DENSITY.
You can still use the legacy parameters PTC_MATERIAL_NAME and MP_DENSITY. However, the legacy parameters do not appear correctly in calculations and reports when you are working with a part that uses multiple materials.
You can modify values of legacy parameters as follows:
Click Tools > Parameters and select Legacy from the list at the bottom of the Parameters dialog box. Type the parameter values in the appropriate boxes.