Gap Elements

Gap elements are two-node elements formulated in three-dimensional space. This element type is only available in a static stress analysis with linear material models.

Two end nodes specified in three-dimensional space define gap elements. Only the axial forces of the element are calculated for each element, and depending on the settings, only compressive forces or only tensile forces are generated. No element-based loading is defined for gap elements.

A compression gap is not activated until the gap is closed; a tension gap is not activated until the gap is opened. Therefore, the structural behavior of a finite element model associated with gap elements is always nonlinear because of its indeterminate condition. Whether the gaps are closed or opened is not known in advance. An iterative solution method is used to determine the status (opened or closed) of the gap elements.

Since the analysis is linear and small deflection theory is used, only motion in the direction of the original gap element orientation is considered. Sideways motion does not affect the status of the gap element.

In general, there are three applications for gap elements. Each has its own characteristics in terms of element input. They are briefly summarized as follows:

Application Type	Element Direction	Input Element Stiffness
Rigid support at the structure boundary to calculate the support reactions	Element must be aligned with global X, Y, or Z axis	Three or four orders of magnitude larger than the other normal stiffnesses in the structure
Interface element between two faces of the structure in space	Element may be defined in any direction	Same order of magnitude of the other normal stiffnesses in the structure
Elastic spring between the base of the structure and the foundation	Element may be defined in any direction	Actual spring constant calculated from the foundation soil

Avoid excessively stiff gap elements (with large spring stiffness) that are not aligned with the global coordinate system. Such elements introduce large off-diagonal values into the structural stiffness matrix and cause solution difficulties. The resulting solution may also be inaccurate. The provided spring stiffness, about three or four orders of magnitude larger than the other normal stiffnesses in the structure, is sufficient for rigid gap elements used in application type (1).

Note: This content applies to gap elements created by hand (lines drawn between two nodes of the model or between the model and the ground). Gap or contact elements created automatically (CAD models, 2D automatic meshes, or hand-built models) are slightly different. See the page Meshing Overview: Creating Contact Pairs: Types of Contact.

Use Gap Elements

To model the effects of a spring or cable where the stiffness is not always present under all loadings.
To find the contact force between two parts under a load.

Gap Element Parameters

When using gap elements, first select the type of gap element to use for the part in the Type drop-down menu in the Element Definition dialog box. The options are:

Type	Gap Element Behavior
Compression with Gap	The element transmits a compression load only when the nodes move towards each other a distance equal to the original length of the gap element. The calculated gap between the parts equals the gap drawn between the parts.
Tension with Gap	The element transmits a tension load only when the nodes move away from each other a distance equal to the original length of the gap element. (Think of this type as a wire or chain with slack. When the wire or chain gets to twice the original length, a tension load is transmitted.)
Compression without Gap	The elements transmit a compression load with any motion of the nodes towards each other. Since the line that defines the gap element cannot be 0 units long, there must be a physical gap between the parts in the model. This type of contact element compensates for the modeling gap.
Tension without Gap	The element transmits a tension load with any motion of the nodes away from each other.

The next step is to define the stiffness of the gap elements in the Stiffness field. See the table in the previous paragraph, What is a Gap Element, for guidelines on the stiffness.

When duplicating a real spring (tension or compression) or chain-like arrangement (tension only), enter the known stiffness. The stiffness (k) of a rod or simple wire can be calculated from k=A*E/L, where A is the cross-sectional area, E is the modulus of elasticity, and L is the length of the rod. When duplicating part-to-part contact, a rigid stiffness is required. A stiffness on the same order of magnitude as the modulus of the material is sufficient. Even when the two values are in different units (force/length versus force/length squared). Another method of calculating the stiffness is to use the definition of stiffness: k = F/Δ where F is the force transmitted through the element and Δ is the compression or elongation in the element. Based on the model, a reasonable Δ can be chosen. If the contact force can be estimated, the required stiffness can be calculated.

To Use Gap Elements

Be sure that a unit system is defined.
Be sure that the model is using the static stress with linear material models analysis type.
Draw the gap elements as lines. See Tips for Drawing Gap Elements below.
Right-click the Element Type heading for the part that you want to be gap elements.
Select the Gap command.
Right-click the Element Definition heading.
Select the Edit Element Definition heading.
In the Type drop-down box select the type of gap element that you want to apply.
- If the element should be active only when the new length is less than zero, select the Compression with Gap option.
- If the element should be active only when the new length is greater than twice the original length, select the Tension with Gap option.
- If the element should be active only when the new length is less than the original length, select the Compression without Gap option.
- If the element should be active only when the new length is greater than the original length, select the Tension without Gap option.
Enter the stiffness of the gap element in the Stiffness field. This is required information and the processor will not run without a value.
Press the OK button.
Add boundary elements with small stiffness as necessary to stabilize the parts. See Perform Analyses with Gap Elements for additional information.

Tips for Drawing Gap Elements

Draw lines connecting the corresponding nodes. Use the Draw Draw Line command.
Use the Draw Design Contact Elements command. This command automatically creates the lines between two sets of vertices. In the case of linear stress (where small deformation is assumed), only the shortest line perpendicular between the faces is normally required. In this situation, use the Constrain lengths option. See the paragraph How to Add Contact Elements to a Model in the section Add Geometry.
Copy the lines from one face to the corresponding face, and in the process use the option to join the copies. Then define the joined lines as gap elements. Imagine two plates in contact. Instead of drawing the lines for the gap elements one by one, do the following:
1. Select the lines (Selection Select Lines) on one of the matching faces.
2. Start the copy command with Draw Pattern Move or Copy.
3. Activate the check box Copy. Make sure the number of copies to make is set to one.
4. Activate the check box Join.
5. Set the total distance and direction vector for the copy. Use the Vector Selector button to click two vertices if you are not sure of the distance or direction.
6. Click OK. The selected lines are copied to the matching face and lines between the faces that become the gap elements.
7. Since this creates a copy of the original lines on the matching face, and since these extra lines are not needed, click Delete. (The last copy made is still selected after the command completes.)
8. Last step: change the join lines to a part number that can be defined as gap elements. This step typically consists of using a box selection (Selection Shape Rectangle) to select the joined lines, then right-click, Edit Attributes and enter an appropriate part number. If using a box selection, the entire line must be inside the selection rectangle. Consequently, the lines on the faces of the parts are also selected. Do not change the attributes of those lines. Unselect the lines on the faces by using the subtract mode (hold the Shift and Ctrl keys) while box selecting those lines.
9. See the paragraph How to Create Copies of Existing Lines in the section Modify Geometry

See Setting Up and Performing the Analysis: Performing the Analysis: Performing A Linear Analysis: Perform Analyses with Gap Elements for additional information common to gap and surface contact elements.