Applying Mechanical Loads

The FE solid mechanics framework offers different types of mechanical loads: point loads, curve loads, surface loads, and body loads. You define point, curve, and surface loads on part entities using segments, whereas body loads are specified on the solid region.

Segments are Simcenter STAR-CCM+ objects that apply loads or constraints on collections of part surfaces, curves, or points. For more information on segments, see Segments Reference.

To create a point, curve, or surface load:

  1. Right-click the Regions > [Region] > Segments node, select Create Segment and choose either:
    • Surface Segment, to apply a load on one or more part surfaces.
    • Curve Segment, to apply a load on one or more part curves. This option is not available when you generate the mesh using the Thin Mesher.
    • Point Segment, to apply a load on one or more part points.
    Depending on the selection, Simcenter STAR-CCM+ adds a surface, curve, or point segment under the [Region] > Segments node.
  2. Specify the part entities where the load is applied:
    • For surface segments, specify the loaded part surfaces using the Surfaces property.
    • For curve segments, specify the loaded part curves using the Curves property.
    • For point segments, specify the loaded part points using the Points property.
    Alternatively, you can create new segments, or assign part entities to existing segments, by using the Set Segment option. To access this option:
    1. Expand the Geometry > Parts > [Part] node.
    2. Select the relevant Surfaces > [Part Surface], Curves > [Part Curve], or Points > [Part Point] node. If you wish to assign multiple part entities to the same segment, multi-select the corresponding nodes.
    3. Right-click one of the selected part entities, select Set Segment and choose to either create a new segment or assign the selected part entities to an existing segment. When no suitable segments are available, the Set Segment option is replaced with Set New Segment.
  3. Select the Segments > [Segment] node and set Type to Load.
To specify the type of load:
  1. Select the [Segment] > Physics Conditions > Solid Stress Loads node and set the loading Method.
    For more information, see Segments Reference.
  2. Specify the load by setting the relevant profile under [Segment] > Physics Values.
    In the following example, a surface load is specified using a traction profile.

    You can specify additional loads by creating corresponding segments. If you select the same part entity (either a part surface, curve, or point) in multiple segments, Simcenter STAR-CCM+ automatically computes the total load on the part entity.
In addition to the surface, curve, and point loads applied using segments, you can apply body loads on the solid region:
  1. Select the [Region] > Physics Conditions > Body Load Option node and set Method to Specified.
  2. Use the [Region] > Physics Values > Body Load node to define the load profile.
    You can define the body load in various ways. Common choices are constant body loads or body loads defined by field functions.

    When using the Solid Stress model in combination with the Finite Element Magnetic Vector Potential model, you can provide user-defined field functions based on electromagnetic fields.

    Physics and motion models can introduce additional body loads. For example, the Gravity model introduces a body load of f = ρ g . Prescribed rotations and translations introduce body loads due to the inertia forces that arise from the acceleration of the structure (see Prescribing Rigid Rotations and Translations).

If the body load you have defined depends on the displacement, velocity, or acceleration, you can specify this relationship by providing the derivatives of the load with respect to these quantities, in the form of second-order tensors. The solver uses the body load derivatives to linearize the stiffness matrix (see Eqn. (4571)).
  1. Select the Physics Conditions > Body Load Derivative node and activate the derivative options you require.
  2. To define the derivatives:
    1. Select the corresponding Physics Values > [Derivative] nodes and set the Method that you want to use to define the tensor components.
    2. Expand the [Derivative] > [Tensor] node and specify the tensor components.
      Non-symmetric tensors can have a negative impact on the simulation performance.
    3. If you want to define the tensor in a specific local coordinate system, select the [Tensor] node and set the Coordinate System.