The Material Assignment feature provides a convenient way to assign a material to multiple bodies and control its behavior, such as nonlinear effects, thermal strain calculation, or reference temperature. It also provides a convenient way for you to edit material properties through a Commands (APDL) object.
Important:
If you scope a Material Assignment object to elements, the application does not validate that the assigned material includes all required material properties to assure a successful solution. As a result, the following results and result tools that use these material properties, do not produce correct result values. These result types only support body scoping.
Error (Structural, Thermal, and Magnetic)
Strain results
Stress Tool results
Fatigue Tool results
The Material Assignment feature is not supported by LS-DYNA.
To insert and apply a Material Assignment object:
Select either the Materials object or one of its material child objects.
Select the option from the Materials Context tab or, right-click the object and select > . A object is placed in the Outline.
Select your Scoping Method: either Geometry Selection or Named Selection.
Select the desired Bodies or Elements or select an appropriate user-defined Named Selection.
Specify the desired material using the Material Name property. This property behaves just like the Material Assignment property of a body or part. And, it can be designated as a parameter.
Specify the following as needed:
As needed, modify the Field Coordinate System setting. Using the setting, all of the specified bodies will have the same coordinate system.
The use of material assignment also affects how materials are sent to the solver. By default, when Mechanical creates an input file, the application assigns a unique
material identifier (matid, #) to each body of the model regardless of the material assigned to the body/part. Here is an example input file. Each part
is assigned the material Structural Steel and has its own material identifier.
!*********** Model Summary ******************** !Part 12, Structural Steel, matid, 1 !Part 13, Structural Steel, matid, 2 !Part 14, Structural Steel, matid, 3 !Part 133, Structural Steel, matid, 4 !Part 134, Structural Steel, matid, 5 !Part 135, Structural Steel, matid, 6 !*********************** End Model Summary *****************
When material assignment object is used, all the scoped bodies are assigned the same material identifier, as illustrated below (mat id, 43). For
this example, you can see the default behavior of material assignment as well as the Material Assignment feature.
!*********** Model Summary ********************
!Part 12, Structural Steel, matid, 1
!Part 13, Structural Steel, matid, 2
!Part 14, Structural Steel, matid, 3
!Part 133, Titanium Alloy, matid, 43
!Part 134, Titanium Alloy, matid, 43
!Part 135, Structural Steel, matid, 6
!*********************** End Model Summary *****************Note:
When specifying the same material to multiple bodies using Material Assignment object, the application can no longer identify the bodies using the material identifier (
matid) in the solver input file. In this case, you can use thetypeidslist to identify a body. The identifiertypeidsis a one-dimension array parameter that you can use to access the type numbers for a body. You can access type numbers using a subscript (enclosed in parentheses) to identify the required item of the array. For example, to access the first type number for the body usetypeids(1).The Material Assignment feature cannot be used with either Layered Section or Imported Trace.