Apply torque load in Abaqus

As you may know, elements like continuum (solid) have no rotational degree of freedom. Therefore, you cannot apply moments nor rotations directly when using them. Then, the only way to apply torque is through a coupling constraint. You have to put a moment on a reference point and connect this point with the points on your structure.

Kinematic coupling constrains the motion of the coupling nodes to the rigid body motion of the reference node. The constraint can be applied to user-specified degrees of freedom at the coupling nodes with respect to the global or a local coordinate system.

1. [In any module before Mesh] create a reference point (named as RP in Abaqus)

2. [In Interaction Module] define a coupling constraint:

Create Constraint > Type=Coupling > select RP as your constraint control point > select either Node Region or Surface (depending on your model) > Coupling Type=Kinematic

3. Apply your torque (moment) or rotational BC to defined RP

Have you started simulation in Abaqus recently? I recommend you download these free tutorials here!  FREE ABAQUS TUTORIAL  

Notes:
1. If you are using Abaqus/Explicit as solver (Steps like Dynamic, Explicit), you MUST assign Inertia to your RP avoid facing Error in job submission. In Properties module, in Menu Bar, select Special > Inertia > Create.

2. Kinematic constraints are imposed by eliminating degrees of freedom at the coupling nodes. In Abaqus/Standard once any combination of displacement degrees of freedom at a coupling node is constrained, additional displacement constraints—such as MPCs, boundary conditions, or other kinematic coupling definitions—cannot be applied to any coupling node involved in a kinematic coupling constraint. The same limitation applies for rotational degrees of freedom. This restriction does not apply in Abaqus/Explicit.