Edge Load
Add an Edge Load as a force or moment distributed along an edge (for the Plate interface add it to boundaries). The load is defined in the given coordinate system.
Coordinate System Selection
Select the coordinate system to use for specifying the load. From the Coordinate system list select from:
Global coordinate system (the standard global coordinate system).
Local edge system
Face Defining the Orientations
This setting is used in conjunction with Local edge system and Shell Local System. When the load is applied to an edge which is shared between boundaries, the coordinate system can be ambiguous. Select the boundary which should define the edge system. The default is Use face with lowest number.
Through-Thickness Location
Select a surface — Top Surface, Midsurface, or Bottom Surface. The default is that the load is applied at the midsurface. The effect of using another surface than the midsurface is twofold:
To place the load at another distance from the midsurface, select the Offset checkbox, and enter a value for the offset, zoffset.
If the material model is Section Stiffness, there may physically not be a well-defined top and bottom surface. If the load is applied at such a surface, the thickness value used to compute the load is taken from the settings in the Thickness and Offset node.
If a selected edge is connected to boundaries having different thicknesses, then the result of specifying Top Surface or Bottom Surface is not well defined.
Force
Select a Load typeForce per reference area, Force per deformed area, Force per reference length, Force per deformed length, Total force, or Resultant.
For Force per reference length and Force per deformed length, the traction components are given explicitly.
For Force per reference area and Force per deformed area, the given traction components are multiplied by the thickness of the shell in order to give the edge load.
For Total force, COMSOL Multiphysics divides the total force by the length of the edges where the load is active. Then the force is applied in the same way as for a Force per reference length. When working with curved boundaries or local coordinate systems, use this option carefully, as the result is not always intuitive.
For Resultant, enter the Force and Moment with respect to a point. Select the Application point defined usingCentroid, Point, or Coordinates. For Centroid, the coordinates of the application point is the centroid of the selected boundaries. For Point, select a geometrical point in the section Application Point. For Coordinates, enter the global coordinates of the Application point, xa.
The load list normally only contains User defined. When combining with another physics interface that can provide this type of load, it is also possible to choose a predefined load from this list.
fL
N/m
fl
N/m
fA
fa
Ftot
F, M
Moment
Select a Moment type to define the moment load — Moment per reference area, Moment per deformed area, Moment per reference length, Moment per deformed length, or Total Moment. Enter values or expressions for mA, ma, mL, ml, or Mtot.
This section is available only in the Shell and Plate interfaces. It is not present when Resultant is selected as the Load type.
mA
ma
mL
ml
Nm/m2
Mtot
Nm
Traction Field
This section is only shown when Resultant has been selected as Load type. The distribution of the forces over the selected points is controlled by the settings here.
Select a Traction distributionBeam or User defined.
When Beam is selected, the force distribution approximately matches the stress distribution over a beam cross section.
For User Defined, you can write expressions for the force distribution. For 3D components enter expressions for the six dimensionless vector-valued distribution functions, q1, q2, q3, q4, q5, and q6. For 2D components enter expressions for q1, q2, and q4. Usually, the local coordinates of the loaded region would be used for this purpose, but there is no limitation on the form of the functions. The built-in variables for the local coordinates are named <physics_tag>.<load_tag>.x2 and <phys_tag>.<load_tag>.x3, for example solid.bndl1.x2. The default value is the distribution that is used when Beam is selected as Traction distribution.
The local coordinates, x2 and x3, are defined in the following way:
x2 is the axis around which the virtual principal area moment of inertia is larger.
When User Defined is selected, you can also select a Weight functionNone, Circular, or User Defined. This function acts as a multiplier to the force distribution functions. When None is selected, the weight function w = 1. For Circular, enter a radius rw of a circle, outside of which no load is applied (w = 0). Inside the circle, w = 1. For User Defined, enter a weighting expression. Usually, the built-in local coordinates of the loaded region would be used for this purpose, but there is no limitation on the form of the function. A time- or parameter-dependent function can, for example, be used to model a moving load.
The traction distribution functions have the property that the forces are distributed as
where the coefficients ci are chosen so that the given force and moment resultants are obtained.
Symmetry
This section is only shown when Resultant has been selected as Load type. If the resultant force is applied in a symmetry or antisymmetry plane, this fact needs to be taken into account when creating the corresponding force distribution.
Select a symmetry type — None, Symmetry, or Antisymmetry. When one of the types of symmetry is chosen, specify the symmetry plane by entering a Normal Vector, nsym, and a Point, xsym, located in the plane.
When specifying a resultant load in a symmetry plane, you still provide the full value of force and moment, as if there were no symmetry in the model. Any components of the given load that do not fulfill the selected type of symmetry will be discarded.
When using the Resultant option, the following should be observed
Linear Buckling
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog.
If you are performing a linear buckling analysis with a combination of live and dead loads, select the Treat as dead load checkbox to indicate that the load contributions from this node are constant. The default is that a load is proportional to the load factor.
 
You can add the Phase subnode to specify the phase of this load in a frequency domain analysis.
Location in User Interface
Context Menus
Ribbon
Physics tab with Shell or Membrane selected:
Physics tab with Plate selected: