Applying and Testing Constraints

Apply minimum constraints to allow for free thermal expansion.

When constraining a part for thermal-structural analysis, avoid applying constraints which are too restrictive and lead to unrealistic stress concentrations. In this tutorial, you apply constraints at three points on the manifold to prevent rigid body motion, while allowing free expansion of the solid structure.

Create a point segment to constrain one point on the manifold in all degrees of freedom:

Right-click the Regions > Manifold (Stress) node and select Create Segment > Point Segment.

Select the Segments > Point Segment 1 node and set the following properties:


Node	Property	Setting
Point Segment 1	Points	Vertex 1
Point Segment 1	Type	Constraint
Physics Conditions > Solid Stress Constraint	Method	Fixed (default)

Define a segment to constrain the second point along two axes:

Right-click the Segments node and select Create Segment > Point Segment.

Select the Point Segment 2 node and set the following properties:


Node	Property	Setting
Point Segment 2	Points	Vertex 2
Point Segment 2	Type	Constraint
Physics Conditions > Solid Stress Constraint	Method	Displacement
Physics Values > Displacement	Method	Composite
Composite	Constrain X	Deactivated
	Constrain Y	Activated (default setting)
	Constrain Z	Activated (default setting)

Define a segment to constrain the third vertex along y:

Create another point segment.

Select the Point Segment 3 node and set the following properties:


Node	Property	Setting
Point Segment 3	Points	Vertex 3
Point Segment 3	Type	Constraint
Physics Conditions > Solid Stress Constraint	Method	Displacement
Physics Values > Displacement	Method	Composite
Composite	Constrain X	Deactivated
	Constrain Y	Activated (default setting)
	Constrain Z	Deactivated

In thermal strain analyses, it is important to define realistic constraints. A fixed condition on a surface segment can prevent thermal expansion and lead to unrealistic stress concentrations. To test your set of constraints, increase the temperature uniformly and run the analysis. The resulting stresses must be close to zero:

Edit the Regions > Manifold (Stress) node and set the following properties:


Node	Property	Setting
Physics Conditions > Specified Temperature Option	Method	Specified
Physics Values > Specified Temperature	Method	Constant
Physics Values > Specified Temperature	Value	650 K

Freeze the flow and energy solvers and run the FE Stress solver for two iterations:

Select the Stopping Criteria > Maximum Steps node and set Maximum Steps to 352.
Expand the Solvers node.
Multi-select the Wall Distance, EB K-Epsilon Turbulence, and K-Epsilon Turbulent Viscosity nodes and activate Solver Frozen.
Select the Coupled Implicit solver and activate Freeze Flow.
Click (Run).
When the stopping criterion has been satisfied, open the von Mises Stress scene and examine the stresses.
As the stresses are approximately zero, the applied constraints are not too restrictive.
Save the simulation.