Product help with community knowledge

### Page statistics

1031 views1 edit(s)4430 characters(s) Page last modified 09:57, 21 Mar 2012 by contentconnector

# Coupling Elements

Use coupling elements to model some mechanisms easily. Specifically, these elements aid in the simulation of parts that couple at a known length. This coupling is modeled by introducing a stiffness when it reaches this length. This stiffness is calculated using a modulus of elasticity, a coupling area and the length of the element. It should be reemphasized that when the element is shorter than this coupling length, it has no stiffness. The modulus of elasticity should be high enough to ensure that there is enough stiffness when it reaches the coupling length.

## Coupling Element Parameters

When using coupling elements, first specify the length above which the element will have a stiffness in the Coupling Length field in the Element Definition dialog. Next, specify the cross-sectional area of the element in the Cross-sectional area field. Finally, specify the modulus of the element in the Coupling Modulus field.

The stiffness of the coupling element will be the product of the coupling modulus (E) and cross-sectional area (A) divided by the coupling length (L), or stiffness = A*E/L. The initial force in the element is either 0 if the length drawn in the model is shorter than the coupling length, or equal to (A*E/L)*(Ld-L) if the drawn length is longer than the coupling length, where Ld is the drawn length. The coupling element can create a tension preload.

## Basic Steps for Use of Coupling Elements

1. Be sure that a unit system is defined.
2. Be sure that the model is using a nonlinear analysis type.
3. Right-click the Element Type heading for the part that you want to be coupling elements.
4. Select the Coupling command.
5. Right-click the Element Definition heading.
6. Select the Edit Element Definition command.
7. Enter the length of the coupling element at which you want coupling to be simulated in the Coupling Length field.
8. Enter the cross-sectional area of the elements in the Cross-Sectional Area field. This is required information and the model will not run without it being entered.
9. Enter the stiffness that you want applied in the Coupling Modulus field.
10. Press the OK button.
TipWhen performing a static analysis, keep in mind that it may be necessary to considering stability without relying on the contribution from the contact. See the page Setting Up and Performing the Analysis: Performing the Analysis: Performing A Nonlinear Analysis: Performing Analyses with Contact for suggestions.