Joint components

In many models, it is necessary to simulate joints and pinned connections for rotational purposes. Modeling the actual joint components with surface to surface contact will create very long run times. In most cases, the effects on the actual joint components are not important. The easiest way to simulate a joint or pin without a long runtime is to create a Truss element along the axis of the joint and connect it on the ends to the part that will rotate about the axis. Since truss elements cannot resist rotation, this creates an effective pin joint. Adding these lines to an existing meshed model can become quite tedious. The Create Joint command provides a quick alternative to this process when working with a CAD model. Using the Create Joint you can select the surfaces that you want to use to create the joint. When you create the surface mesh, truss elements will be constructed between these surfaces.

Figure 1: Schematic of a Pin Joint

Instead of modeling a true pin, a clevis and eye are connected with a pin-style joint. Truss elements from two points (A and B) are connected to each node on the selected surfaces. (To simplify this figure, only one line is shown from each point to each surface. Also, points A and B are moved outside of the parts for clarity.)

A pin joint can be visualized as sets of space trusses. The truss elements (blue lines) that extend from the surfaces of the clevis (green body) to point A form one space truss. If the truss elements are sufficiently stiff, point A cannot move relative to the surface of the clevis. Likewise, a second space truss is formed from the clevis to point B. Likewise, space trusses are created from the eye (light blue body) to points A and B. Because truss elements have pinned connections, the space trusses and bodies they connect to can rotate about the line A-B, but they cannot translate independent of each other. Thus, a pin is simulated.

To create a joint, follow the steps below.

1. Optionally select all of the surfaces that you want to be involved in the joint. You can either click the surfaces on the model (be sure to hold down the <Ctrl> key to select multiple surfaces) or select the heading for those surfaces in the tree view (again be sure to hold down the <Ctrl> key to select multiple surfaces). You must have the Selection Shape Point or Rectangle and Selection Select Surfaces commands active to select surfaces by clicking them in the model.
2. Select Mesh CAD Additions Joint.
3. The Create Joint dialog will appear to allow you to enter the specifications for this joint. The surfaces that you selected before entering the Create Joint screen will be listed in the Participating surfaces section. If surfaces were not selected before, or if additional surfaces need to be added for the joint, select the surface or surfaces and click the Add button.
4. Select the type of joint that you want to create in the Joint drop-down box.
   • Pin joint (lines to axis endpoints): This option will create a classic pin joint where the nodes at each end of the surfaces included in the joint are connected to the opposite end of the joint axis. This type of joint will allow the model to rotate around the axis. See Figure 1.
   • Universal joint (lines to axis midpoint): This option will create a classic universal joint. The nodes at either end of the model will be connected to the midpoint of the axis. This type of joint will allow the model to rotate about the axis as well as swivel about the center point of the axis. See Figure 2.

     

     Figure 2: Schematic of a Universal Joint

     Compare the universal joint to the pin joint. Instead of the space trusses being connected to two points (A and B in Figure 1), the space trusses of a universal joint are connected to one point O. Because truss elements have pinned connections, the space trusses and bodies they connect to can rotate about point O, but they cannot translate independent of each other. Thus, a universal or ball-and-socket joint is simulated.

5. If you want the joint creator to decide where the axis of rotation will be, based on the geometry of the surfaces involved in the joint, select the Automatic detection of axis/center-point radio button. To specify the axis of rotation, select the Manual axis/center-point specification radio button and enter the X, Y, and Z coordinates in the appropriate field. If your joint is a pin joint, you will have to enter the coordinates for the two end points of the axis. If your joint is a universal joint, you will have to enter the coordinate for the center point.
6. Press the OK button. If the mesh already exists, the lines for the joint will be created.
   • To create another joint, repeat the process.
   • To edit the specifications of a joint, select it in the Meshes branch of the tree view, right-click, and choose Edit.
   • To delete a previously created joint, select it in the Meshes branch of the tree view, right-click, and choose Delete.

If the mesh does not exist when the joint is defined, then when you execute the Mesh Mesh Generate 3D Mesh command the surface mesh will be created as usual, and then the joint application program will create the lines for the joint (either truss or beam elements). These lines will be placed in the next part available in numerical order. If you defined multiple joints, each joint will be placed in a unique part.

Potential pin joint issue

When two parts are in contact (no gap between them) and the contact type is free or surface contact, the elements of the pin joint are connected to the nodes on one of the parts, not both parts, at the contact face. This connection methodology prevents the parts from becoming locked to each other, which would occur if coincident nodes from two parts were connected to the same truss element. The joint must be free to articulate. Considering the approximation being used for pin joints, this situation is usually not a problem. However, if a joint behaves as if it is locked, then change one or both CAD parts to include a gap between the joint surfaces of the parts. Alternatively, use differing hole diameters or add a chamfer around the contact edge (as shown in the below-right figure) to ensure that the joint is free to articulate.

Parts 1 (light blue body) and 2 (green body) are in surface contact. Two sets of nodes exist along the line C-D. However, the elements of the pin joint (lines in blue) are generally connected to only one set of nodes along C-D, not to both set of nodes. So, the joint is normally free to articulate. If, for some reason, the joint behaves as if it is locked, use the modified geometry shown on the right to correct the problem.

When you place a chamfer on one or both parts, the two cylindrical surfaces, to which the pin joint is applied, have no coincident edges. One set of truss elements is connected to the nodes along C-D, and another set of truss elements is connected to nodes along C'-D'. The possibility of any truss being connected to coincident nodes of the two parts is eliminated, ensuring that the joint is free to articulate.