A joint typically serves as a junction where bodies are joined together. Joint types are characterized as fixed or free depending on their rotational and translational degrees of freedom. If you specify a Joint as a it is classified as a remote boundary condition. Refer to the Remote Boundary Conditions section for a listing of all remote boundary conditions and their characteristics.
Joints are supported in the following structural analyses:
A joint cannot be applied to a vertex scoped to an end release.
Each multibody part made of rigid bodies is treated as a single, rigid part. Consequently, joints must not be created within a multibody part.
Similarly, functionalities such as configure, assemble, model topology, or redundancy analysis always consider each multibody part as a single part, regardless stiffness behavior. Joints must be defined between independent parts or multibody parts to use these functionalities.
The Samcef Solver interface supports all joint types except for the fixed joint, slot joint, and the imperfect joints. Only supported joint types are active in the Mechanical interface.
To maintain consistency with the characteristics of Samcef joints, you must insert a Comment object with the correct name under the joint object. The comment permits you to capture joint properties which are not available in the view in Mechanical. The comment functions similarly to a commands object: the content of the comment is appended to the description of the joint in the solver input file. The necessary name for the comment object is listed for each joint type.

For all joints that have both translational degrees of freedom and rotational degrees of freedom, the kinematics of the joint are defined such that the moving coordinate system translates in the reference coordinate system. For example, if a joint is a slot, the translation along X is expressed in the reference coordinate system.
Once the translation has been applied, the center of the rotation is the location of the moving coordinate system.
For the ANSYS Mechanical APDL solver, the relative angular positions for the spherical, general, and bushing joints are characterized by the Cardan (or Bryant) angles. This requires that the rotations about the local Y axis be restricted between -π/2 to +π/2. Thus, the local Y axis should not be used to simulate the axis of rotation if the expected rotation is large.
Joints are considered as point-to-point in the solution though the user interface shows the actual geometry. Due to this abstraction to a point-to-point joint, geometry interference and overlap between the two parts linked by the joint can be seen during an animation.
The degrees of freedom are determined depending on the selected solver. For the ANSYS Rigid Dynamics solver, the degrees of freedom are the relative motion between the parts. For the ANSYS Mechanical solver, the degrees of freedom are the location and orientation of the center of mass of the bodies.
When initial conditions are applied, there are two means for the ANSYS Rigid Dynamics solver to initialize the velocities:
A pure kinematic method, only based on the kinematic constraints. It minimizes the position and velocity increments.
A method using the inertia matrix. The position increment, scaled by the inertia matrix, is minimized; while the velocity increment is calculated in order to minimize the kinetic energy.
Unless otherwise specified using joint conditions, both the ANSYS Mechanical APDL solver and ANSYS Rigid Dynamics solver start with initial velocities equal to zero. This has different implications for each solver. For the ANSYS Mechanical APDL solver, this means that the bodies will be at rest. For the ANSYS Rigid Dynamics solver, this means that the relative velocities will be at rest.
Consider, for example, an in-plane double pendulum, with a constant velocity specified for the first grounded link. The two solvers will treat this scenario as follows:
Using the ANSYS Rigid Dynamics solver:
If the first method is used, the second link has the same rotational velocity as the first, because the relative velocity is initially equal to zero.
If the second method is used, the second link does not start with the same initial velocity as the first link.
Using the ANSYS Mechanical solver, the second link starts at rest.
Joints can be defined using one or two coordinate systems: the Reference Coordinate System and the Mobile Coordinate System.
The use of two coordinate systems can be beneficial in certain situations, such as when a CAD model is not imported in an assembled configuration. Using two coordinate systems also enables you to employ the and features (see Manual Joint Creation), and it gives you the ability to update a model following a CAD update.
For the ANSYS Rigid Dynamics solver, the zero value of the degrees of freedom corresponds to the matching reference coordinate system and moving coordinate system.
If a joint definition includes only the location of the Mobile Coordinate System (see Modifying Joint Coordinate Systems), then the DOF of this joint are initially equal to zero for the geometrical configuration where the joints have been built.
If the Reference Coordinate System is defined using the Override option, then the initial value of the degrees of freedom can be a nonzero value.
Consider the example illustrated below. If a Translational joint is defined between the two parts using two coordinate systems, then the distance along the X axis between the two origins is the joint initial DOF value. For this example, assume the joint initial DOF value is 65 mm.

Conversely, if the joint is defined using a single coordinate as shown below, then the same geometrical configuration has a joint degree of freedom that is equal to zero.

For the ANSYS Mechanical APDL solver, having one or two coordinate systems has no impact. The initial configuration corresponds to the zero value of the degrees of freedom.
Joint Condition Considerations
When applying a Joint Condition, behavior varies depending on the solver selected. The following tables demonstrate variations in solver behavior, using the right part of the translational joint illustrated above moving 100 mm towards the other part over a 1 second period. (The distance along the X axis is 65 mm.)
| Solver | Displacement Joint Condition | |
| Time | Displacement | |
| ANSYS Rigid Dynamics – Two Coordinate Systems | 0 | 65 |
| 1 | 165 | |
| ANSYS Rigid Dynamics – One Coordinate System | 0 | 0 |
| 1 | 100 | |
| ANSYS Mechanical APDL – Two Coordinate Systems | 0 | 0 |
| 1 | 100 | |
| ANSYS Mechanical APDL – One Coordinate System | 0 | 0 |
| 1 | 100 | |
You can unify the joint condition input by using a Velocity Joint Condition.
| Solver | Velocity Joint Condition | |
| Time | Displacement | |
| – Two Coordinate Systems | 0 | 100 |
| 1 | 100 | |
| – One Coordinate System | 0 | 100 |
| 1 | 100 | |
| – Two Coordinate Systems | 0 | 100 |
| 1 | 100 | |
| – One Coordinate System | 0 | 100 |
| 1 | 100 | |