Elemental and Nodal Constraints
For most constraints, you can select between using elemental and nodal constraints. To do this, select Advanced Physics Options, so that the Constraint Settings section is displayed.
When using nodal constraints, one constraint is generated for each node within the selection a certain constraint feature. With elemental constraints, the number of constraints added at a node equals the number of elements connected to that node. This means that if some values used in the constraints differ between the elements, then different constraints will be generated by the elemental method, whereas with the nodal method an average is computed at the node before adding the constraint.
When several constraints are present at a node, the internal constraint elimination algorithm is responsible for reducing them to a minimum unique set. Using elemental constraints will clearly put an extra burden on this algorithm, so whenever possible you should use nodal constraints.
The two different options exist, since under some circumstances the actual constraints can differ between the two methods. Consider for example a symmetry constraint, where the displacement in the direction normal to the boundary is constrained by the equation
where n is the unit normal vector.
If there are several intersecting symmetry planes, like in Figure 2-6, using nodal constraints could cause a problem:
•
If both boundaries are selected in the same Symmetry node, then only a single constraint is applied for each node along the common edge, while you actually want constraints along the normals of both planes. The normal used would be pointing somewhere between the two planes, since a nodal constraint uses averaging of the values from the adjacent elements.
•
If two Symmetry nodes are used, so that the selection in any one of them only contains boundaries without a normal direction discontinuity, the intended constraints are added. On the common edge, there will be two contributions, one from each Symmetry node, and each using the normal direction of its boundary. If you want to use nodal constraints, you must set up your model in this way if the constraints are orientation dependent.
Elemental constraints, on the other hand, can cause problems if the constraints added by adjacent elements are not exactly the same. This could for example happen if the normal orientation differs between neighboring elements. In such a case, a boundary could behave as if it were fixed when a Symmetry, Antisymmetry, or Roller constraint is applied. Such a situation could occur when the component consists of an imported mesh, so that no underlying geometry exists.
The default type of the constraint, nodal or elemental, differs between different constraint features. A nodal formulation is the default whenever it is considered safe, like for a Fixed Constraint. Whenever the constraint can have a dependency on the surface orientation, the default value is elemental.
See also Constraint Settings in the COMSOL Multiphysics Reference Manual.