COMSOL 6.2 - Using the Beam Cross Section Interface

Using the Beam Cross Section Interface


	When the document refers to ‘beams’ in the following, the information is applicable to both the Beam and Pipe Mechanics interfaces.

The Beam Cross Section interface can be used in three different ways:

•

In a separate model, to compute beam cross section data that is manually transferred as input to another model where a beam analysis is performed. Possibly, the cross section data is also used outside COMSOL Multiphysics.

•

In the same model as beam interface, but with the Beam Cross Section interface placed in a separate component. Data can then be transferred between the two interfaces by entering variable names in input fields.

•

In the same component as the beam interface. In this case, multiphysics couplings can be used to transfer data between the interfaces.

When using the Beam Cross Section interface and the beam interface in the same model, there are a number of things to pay attention to:

•

Usually the determination of the cross-section data is computationally more expensive than the actual analysis of the beam structure. Thus, it is best to use either separate studies or separate study steps for the two tasks.

•

If two separate studies or study steps are used, then the must be set in the second study step, where only the beam problem is solved. Under , you can also uncheck the check box for the beam cross section degrees of freedom in order to save space.

•

You can transfer data between the two physics interfaces using the Beam Cross Section–Beam Coupling and Beam–Beam Cross Section Coupling multiphysics couplings if the interfaces belong to the same component.

•

If you are using two different components, you must use a fully scoped variable name (like comp2.bcs3.A for the area) when referencing the beam cross-section properties in the input fields of the beam interface.

•

If a beam interface is added either after or at the same time as a Beam Cross Section interface, the only study type shown when adding a physics interface is . In this case, under , select to find the other study types available for the beam analysis.


	Values of Dependent Variables and Physics and Variables Selection in the COMSOL Multiphysics Reference Manual

For the Beam Cross Section interface in 2D, the cross sections are analyzed in the xy-plane. However, the beam interface uses a notation where the local x-axis is along the beam, and the cross section is described in a local yz-plane.

For the Beam Cross Section interface in 3D, the boundaries that represent cross sections can have arbitrary orientation. It is not related to the orientation of an actual beam.

In order to avoid confusion, the cross-section properties are described in the local x1- and x2-coordinates (see Figure 9-1). When data is transferred to a beam interface, you must keep track of the coordinates that correspond to the local y and z directions.


	Channel Beam: Application Library path Structural_Mechanics_Module/Verification_Examples/channel_beam

The 3D version of the interface is based on the layered material technology. The reason is that the extra dimension inherent in layered materials is used to extrude the cross section when the interface is used to create a fully 3D representation of the stress state. Thus, there are significant conceptual differences between the 2D and 3D versions of this physics interface.

Computing the Cross-Section Data

You can compute the properties for several different cross sections in the same Beam Cross Section interface.

In a 2D component, the geometry of the cross sections is drawn in the xy-plane. In a 3D component, you can create one or more arbitrary work planes, in which the cross sections are drawn.

You need to attach material data to the cross section. The procedure is different in 2D and 3D.


	The material properties can be assigned to the domain in a Material node, and then the option From material is used in the Homogeneous Cross Section node. Alternatively, you can also select User defined, and enter expressions for the material data manually.


	Material data cannot be set locally in the Homogeneous Cross Section node. Usually, you would add a Single Layer Material node under Materials in the component to provide the material data. You can, however, also use a global Layered Material, which is then referenced from a Layered Material Link in the component. A boundary is not eligible for selection in the physics interface until a layered material has been assigned. A layered material has, in addition the material data, three more inputs. The only one that may need to be changed is the Thickness, lth. It is not used as long as you are only computing cross-section properties, but if you are mapping results back from a beam interface, it should match the length of the beam.

If the section is not simply connected, add one Hole node for each internal hole. In that node, select all boundaries around the hole.

The default mesh density is tuned for thin-walled sections. For solid sections, an unnecessarily large model is obtained when using the default mesh.

The computed cross-section data is stored in the variables listed in Table 9-1:

Table 9-1: Variables Containing Cross-Section Data.
Variable	Description	Input to beam interface	Link to Theory Section
bcs.A	Area	Area (A)	Area
bcs.CGx	Center of gravity, x-coordinate	Implicit, since it affects the positioning of the beam centerline.	Center of Gravity
bcs.CGx	Center of gravity, y-coordinate	As above	Center of Gravity
bcs.x1	First coordinate in principal axes system	Implicit, since it can be used for determining stress evaluation locations	Local Coordinates
bcs.x2	Second coordinate in principal axes system	As above	Local Coordinates
bcs.I1	Largest principal moment of inertia	Moment of inertia around local y/z-axis (Izz/Iyy)	Moments of Inertia
bcs.I2	Smallest principal moment of inertia	As above
bcs.Ixx	Moment of inertia around x-axis	-
bcs.Iyy	Moment of inertia around y-axis	-
bcs.Ixy	Deviatoric moment of inertia in xy-system	-
bcs.rg	Radius of gyration	-
bcs.alpha	Angle from x-axis to first principal axis	Rotation of vector around beam axis (ϕ)	Directions of Principal Axes
bcs.mu1	Max shear stress factor, x1 direction	Max shear stress factor in local y/z direction (μy/μz)	Bending Shear Stresses
bcs.mu2	Max shear stress factor, x2 direction	As above
bcs.kappa1	Shear correction factor, x1 direction	-
bcs.kappa2	Shear correction factor, x2 direction	-
bcs.ei1	Shear center location, first local coordinate	Distance to shear center in local y/z direction.
bcs.ei2	Shear center location, second local coordinate	As above
bcs.J	Torsional constant	Torsional constant (J)	Torsion
bcs.Wt	Torsional section modulus	Torsional section modulus (Wt)	Torsion
bcs.Cw	Warping constant	-	Warping
bcs.Kw	Warping section modulus	-
bcs.sw	Nonuniform torsion parameter	-

Computing Detailed Stresses

If you have a set of section forces (axial force, shear forces, bending moments, and twisting moments), it is possible to display the stresses it causes. To do this, enter the values in the section. You can also add your own acceptance criteria by adding one or more Safety nodes.

The stresses are available in the variables listed in Table 9-2.


	After changing data in this section, you do not need to compute the study for this physics interface again once is has been solved. It is sufficient to do an Update Solution to get the stress plots updated.


	Studies and Solvers in the COMSOL Multiphysics Reference Manual

Table 9-2: Variables Containing Stress Distributions.
Variable	Description and	Link to Theory Section
bcs.sN	Stress from axial force	Axial Stress
bcs.sM1	Bending stress from moment around x1 axis	Bending Axial Stresses
bcs.sM2	Bending stress from moment around x2 axis	Bending Axial Stresses
bcs.tT1x	Shear stress from force in x1 direction, x-component	Bending Shear Stresses
bcs.tT1y	Shear stress from force in x1 direction, y-component
bcs.resT1	Shear stress from force in x1 direction, resultant
bcs.tT2x	Shear stress from force in x2 direction, x-component
bcs.tT2y	Shear stress from force in x2 direction, y-component
bcs.resT2	Shear stress from force in x2 direction, resultant
bcs.tMtx	Shear stress from twisting moment, x-component	Torsional Shear Stresses
bcs.tMty	Shear stress from twisting moment, y-component
bcs.resMt	Shear stress from twisting moment, resultant
bcs.mises	von Mises equivalent stress	Equivalent Stress
bcs.spN	Principal stresses; N=1,2,3
bcs.INs	N:th invariant of stress tensor; N=1,2,3
bcs.IINs	N:th invariant of stress tensor deviator; N=2,3
bcs.thetaL	Lode angle for stress tensor

Computing Warping Displacement

You can also compute the axial warping displacement by entering the axial twist of the beam in the section. The theory is described under Warping. The axial displacement is stored in the variable bcs.u.