What is a Spring Element?
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, kt, is applied to the spring element. The spring will rotate through an angle q. 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/kt.
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.
When to Use Spring Elements:
The basic guidelines for when to use a spring element are:
Two parts are connected by a spring with a known spring stiffness value.
Two parts are connected by a part that will only transmit an axial force. The spring stiffness for this part can be calculated as AE/L where A is the cross-sectional area, E is the modulus of elasticity and L is the length.
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. If you want 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. (Mathematically, mixing degrees-of-freedom on each end of the spring gives Resulti = Resultj = stiffness*(Ui - Uj), where Ui and Uj are the translation and rotation at the respective end of the spring, and Result is the force and moment at the respective end of the spring.
The orientation of the spring elements can be displayed using the "View: Options: Element Orientations: Axis 1" menu. 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".
Visualizing Spring Elements in the Results Environment:
Spring elements can appear in the Results environment either as a line or as an actual spring. If you want the spring to be rendered, you must activate the "Visualize as spring" checkbox 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 Using Spring Elements:
Be sure that a unit system is defined.
Be sure that the model is using a structural analysis type.
Right click on the "Element Type" heading for the part that you want to be spring elements.
Select the "Spring" command.
Right click on the "Element Definition" heading..
Select the "Modify 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" checkbox.
Define the dimensions of the spring.
Press the "OK" button.