Applying Constraints

Applying a constraint on a surface, curve, or point, means prescribing one or more components of the displacement vector at that part entity. In stress analysis, you constrain the solid structure to mimic a real life scenario and to prevent the free displacement and rotation of the entire solid. Constraints are an effective way of reducing the number of modeled parts, and hence the simulation cost.

In Simcenter STAR-CCM+, you constrain the displacement of part entities (that is, surfaces, curves, and points) using segments (see Segments Reference). Additionally, for part surfaces that are assigned to symmetry plane boundaries, Simcenter STAR-CCM+ automatically prevents displacement in the normal direction.

To constrain a part entity using a segment:

  1. Right-click the relevant Regions > [Region] > Segments node, select Create Segment and choose either:
    • Surface Segment, to apply a constraint on one or more part surfaces.
    • Curve Segment, to apply a constraint 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 constraint 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 constraint is applied:
    • For surface segments, specify the constrained part surfaces using the Surfaces property.
    • For curve segments, specify the constrained part curves using the Curves property.
    • For point segments, specify the constrained part points using the Points property.
  3. Select the relevant Segments > [Segment] node and set Type to Constraint.
To specify the type of constraint:
  1. Select the [Segment] > Physics Conditions > Solid Stress Constraints node and set the constraint Method.
    For more information, see Segments Reference.
  2. Specify the constraint under the [Segment] > Physics Values > [Fixed/Normal Displacement/Displacement] node.
    • If you define initial conditions for the displacement field, do not specify a nonzero initial displacement for the unconstrained degrees of freedom, as this can lead to instabilities.
    • To prevent conflict, do not apply a nonzero normal displacement on part surfaces that are associated with symmetry boundaries. See Symmetry Plane.
    • When defining Displacement constraints in a non-Cartesian coordinate system, or when defining Normal Displacement constraints, the respective directions are taken with respect to the undeformed configuration.


    You can create other segments to specify additional constraints. In general, it is good practice to constrain the structure in three orthogonal directions, by either:
    • Applying a fixed constraint to at least one surface.
    • Applying symmetry plane conditions, or equivalent zero normal displacement constraints, to three mutually orthogonal surfaces.
    • Define three non-collinear point constraints.
    In thermal strain analyses, it is important to define realistic constraints. A fixed condition on a surface segment does not allow thermal expansion and leads to local stress concentrations. To model a free expansion of a structure, define three non-collinear point constraints, with:
    • the first point constrained in the x, y, and z directions
    • the second point constrained in the x, and y directions
    • the third point constrained in the z direction

    In general, when analyzing the computed stress distribution, restrictive constraints can lead to over-estimated stresses near the constrained areas.