Product help with community knowledge

### Page statistics

1157 views1 edit(s)5424 characters(s) Page last modified 09:57, 21 Mar 2012 by contentconnector

# Contact Elements

Use contact elements to easily model impact problems. Contact is modeled using a contact stiffness. This stiffness is calculated using the modulus of elasticity, a contact area and the length of the element. It should be noted that when the element is longer than this contact length, it has no stiffness. The modulus of elasticity should be representative of the materials making contact.

## Contact Element Parameters

When using contact elements, first specify the length below which the element will have a stiffness in the Contact Distance field in the Element Definition dialog. Since the contact element cannot become shorter than 0 units, a contact distance of 0 is not an acceptable distance. Use a small, finite value for the contact distance. Next, specify the cross-sectional area of the element in the Cross-sectional area field. Finally, specify the modulus of the element in the Contact Modulus field.

The stiffness of the contact element will be the product of the contact modulus (E) and cross-sectional area (A) divided by the contact distance (L), or stiffness = A*E/L. The initial force is always 0 even if the length of the element drawn in the model is shorter than the contact distance. There is no preload.

When duplicating a real spring or soft gasket-like material, you can calculate either the area or the modulus of the contact elements based on the known stiffness and contact distance. When duplicating part-to-part contact, a rigid stiffness is required. Generally, the cross-sectional area and contact modulus can be on the same order of magnitude as the area of the element(s) surrounding each node and the modulus of the material. So with a 0.5-inch by 0.5-inch mesh, the area surrounding each node would be approximately 0.25 inches squared. Another method of calculating the stiffness is to use an alternate definition of stiffness: k = F/D where F is the force transmitted through the element and D is the compression in the element. Based on the contact distance, a reasonable D can be chosen (such as 10% or 1% of the contact length). If the contact force can be estimated, the required stiffness can be calculated from which the area and modulus can be entered for the contact element.

## Basic Steps for Use of Contact 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 contact elements.
4. Select the Contact command.
5. Right-click the Element Definition heading.
6. Select the Edit Element Definition command.
7. Enter the length of the contact element at which you want contact to be simulated in the Contact Distance 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 Contact 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.