Fasteners
The Fasteners node is intended for a simplified modeling of fasteners like rivets or bolts. It is based on the assumption that the holes for the fasteners are present in the shell geometry. The two plates are joined using an elastic connection. There are two possible types of connections:
•
The edges of matching holes are connected.
•
Boundaries surrounding the matching holes are connected. Such boundaries should typically match the size of rivet heads or washers.
The latter type of connection is somewhat more accurate, and can reduce local stress concentrations. This is in particular true when bolts are modeled. Making such connections requires a more sophisticated representation of the geometry, where the fastener holes are surrounded by suitable, usually annular, boundaries.
The actual selection of the pairs of holes to be connected is done in a Hole Selection subnode.
When one or more Fasteners nodes are active in the model, five entries are added to the list of result templates:
•
A Fasteners Forces plot group that shows the normal and shear forces and a label showing the identity number of each fastener. Evaluate the Fasteners Normal Forces and Fasteners Shear Forces evaluation group to display the fasteners forces. The coloring can be affected by the addition of a Safety subnode.
•
A Fasteners Normal Forces evaluation group that contains a table of the location, normal forces, and damage index of all fasteners. Evaluate this table to display the forces in the Fasteners Forces plot group.
•
A Fasteners Shear Forces evaluation group that contains a table of the location, shear forces, and damage index of all fasteners. Evaluate this table to display the forces in the Fasteners Forces plot group.
•
A Fasteners Forces Magnitude evaluation group that contains a table of the normal and shear forces magnitude for all fasteners.
•
A Connected Region Indicator plot group that contains a line plot or a surface plot showing the hole edges or hole surrounding boundaries, respectively, on the destination surface where the fasteners are active. If there are other connection features in the Shell interface, all connection indicators appear in the same plots.
You must evaluate the Fasteners Normal Forces and Fasteners Shear Forces evaluation groups to update the Fasteners Forces plot group if you change the number of fasteners in your model or compute new results. Also, remove the Connected Region Indicator plot group and replace it by a new one if you change the hole selection type between edge or boundary.
Location
The sides of the shells (top or bottom) that are to be connected must be known. The information is used for two purposes: to connect to the correct set of displacements, and to compute the distance, including the shell thickness and offset. Select Connected location — Automatic or Manual. In the automatic mode, the two sides of the shells that are found to be closest to each other are connected. If you want to make another choice, or the if the automatic search for some reason does not give the intended result, select Manual.
In manual mode, the Source and Destination lists are shown. Select Top surface or Bottom surface from both lists.
There are some uncommon cases for which the automatic mode will fail. If this happen, you will get an error message. You can then either move to manual mode or, for some cases, use several Fasteners nodes having smaller selections.
Fastener Properties
Enter Diameter, df for the fasteners diameter.
The stiffness of the fasteners can be computed in two ways, either using analytical expressions based on that the fastener is approximated as a beam, or by direct entry of stiffness values. From the Fastener model list, select Beam or Spring.
Beam
The normal stiffness, kn, and shear stiffness, ks, of the fastener are computed using the following expressions:
The four compliance contributions are defined as
In these expressions
•
df is the diameter of the fastener.
•
Ef, Esrc, and Edst are the elastic moduli of the fastener, the shell on the source side, and the shell on the destination side respectively.
•
νf is the Poisson’s ratio of the fastener.
•
tsrc and tdst are the thicknesses of the shell on the source and destination sides respectively.
•
The multipliers αm are multipliers that make it possible to adjust the default analytical values.
Enter the following data for the fasteners:
•
Young’s modulus, Ef.
•
Poisson’s ratio, νf.
•
Bending flexibility multiplier, αb.
•
Shear flexibility multiplier, αs.
•
Fastener bearing flexibility multiplier, αbr.
•
Plate bearing flexibility multiplier, αpbr.
Spring
Enter the Normal stiffness, kn, and Tangential stiffness, ks.
Advanced
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog.
Select the Search method — Closest point or Manual to specify what should happen if an evaluation point in the destination boundary is mapped outside the source boundary.
The Closest point method is the default and most robust search method. The closest point in the source selection is used by the mapping operator, even if that point is far away from the destination point. This method is not as efficient as the Manual method.
The Manual method is an alternative search method that is computationally efficient, but its robustness is determined by the curvature of the boundaries, the Search distance, and the Extrapolation tolerance. Specify the maximum search distance between the source and destination boundaries and the extrapolation tolerance.
See Advanced Settings for Nonlocal Couplings in the COMSOL Multiphysics Reference Manual for more information.
•
Simplified Modeling of Fasteners
•
Theory for Fasteners
Location in User Interface
Context Menus
Shell > Fasteners
Ribbon
Physics tab with Shell selected:
Global > Shell > Fasteners