A spring element has two basic forms. The first is the classic spring. This spring connects two nodes on the model. This spring can be axial or rotational. For an axial spring, a spring stiffness, k, is applied to the spring element. The spring will deflect a distance x. This distance will depend on the axial force in the spring element, F, and the spring stiffness. The distance the spring deflects can be calculated by the equation x=F/k. For a rotational spring, a torsional stiffness, k t , is applied to the spring element. The spring will rotate through an angle ϑ. This angle will depend on the moment applied to the spring, M, and the torsional stiffness. The angle through which the spring rotates can be calculated by the equation M/k t .
The second form of the spring element is a DOF spring. This spring will connect a single DOF from each node to which it is connected. This spring will have a stiffness value as described for the classic spring.
Spring Element Parameters
When using spring elements, first select the type of spring for the part in the Spring Type section in the General tab of the Element Definition dialog. For most applications, the Spring type is appropriate. To transfer the loads from different degrees-of-freedom at each node, select the DOF Spring type. Next, specify the spring stiffness in the Spring Stiffness field.
If you selected the Spring radio button, specify if you want the spring to resist translation or rotation in the Element Type section. If you selected the DOF Spring radio button, specify the degree-of-freedom to which you want to stiffness applied at the I-node and J-node in the I Node and J Node sections.
When the units of the spring stiffness are shown, the input will be converted based on the Display Units. When a DOF Spring uses different degrees-of-freedom at each node, the physical meaning of connecting a translation to a rotation are difficult to envision. Therefore, no units are shown for the spring stiffness, and no conversion is performed.
Use the Analysis Type drop-down to set the type of displacement that is expected. Small Displacement is appropriate for parts that experience no motion and only small strains and will ignore nonlinear geometric effects that result from large deformation. (It also sets the Analysis Formulation on the Advanced tab to Material Nonlinear Only.) Large Displacement is appropriate for parts that experience motion and/or large strains.
- The orientation of the spring elements can be displayed using View
Visibility Object Visibility Element Axis 1 command. Axis 1 points in the direction from the I Node to the J Node. If axis 1 needs to be reversed for some elements, this can be done by selecting the elements (Selection Select Lines), right-clicking, and choosing Invert I and J Nodes. - Use
Options Analysis tab and set the Use large displacement as default for nonlinear analyses option to control whether the Analysis Type defaults to small or large displacement.
Advanced Spring Element Parameters
Select the formulation method that you want to use for the spring elements in the Analysis Formulation drop-down box in the Advanced tab. If the Material Nonlinear Only option is selected, nonlinear material model effects will be accounted for but all calculations will be performed based on the undeformed geometry. The Total Lagrangian option will refer to the initial undeformed configuration of the model for all static and kinematic variables. The Updated Lagrangian will refer to the last calculated configuration of the model for all static and kinematic variables.
Visualize Spring Elements in the Results Environment
Spring elements can appear in the Results environment either as a line or as an actual spring. For the spring to be rendered, you must activate the Visualize as spring check box in the Visualization tab of the Element Definition dialog. You can then specify the dimensions of the spring. If the sum of the values in the Beginning Length field, the End Length field and the product of the Number of Coils and the Wire Diameter fields is greater than the length of the spring element, the spring will not be drawn in the Results environment. The value in the Coil diameter field refers to the diameter of the spring along the centerline of the wire. The Beginning Length field and the Begin attachment type drop-down box refer to the I-Node end of the spring element. The End Length field and the End attachment type drop-down box refer to the J-Node end of the spring element.
If you specify attachments at either end of the spring, you must define an orientation point. The coordinate entered in the X, Y and Z fields will be used to assign the plane in which the attachment is located. A vector will be created perpendicular to the spring element passing through this point. The attachment will lie in the plane that is perpendicular to this vector. If this coordinate is along the line of the element, the spring will not be drawn in the Results environment.
Basic Steps for Use of Spring Elements
- Be sure that a unit system is defined.
- Be sure that the model is using a nonlinear analysis type.
- Right-click the Element Type heading for the part that you want to be spring elements.
- Select the Spring command.
- Right-click the Element Definition heading
- Select the Edit Element Definition command.
- Select the type of spring in the Spring Type section.
- If the Spring radio button is selected in the Spring Type section, specify if this spring will be axial or rotational in the Element Type section.
- If the DOF Spring radio button is selected in the Spring Type section, select the DOF for the i node and j node in the I Node and J Node sections.
- Specify the stiffness of the spring in the Spring stiffness field.
- Go to the Visualization tab.
- Activate the Visualize as spring check box.
- Define the dimensions of the spring.
- Press the OK button.