First of all, what you observed is the expected behavior and physically meaningful.

Stress BC in Autodyn is basically Pressure BC. Pressure is applied to the selected surfaces of a solid structure. Please be aware that the stress inside the solid structure is not necessarily equal to the pressure on the surfaces. This is because every material in Autodyn has Equation of State (EOS). In other words, every material in Autodyn, except the materials have Rigid EOS, is compressible. The stress in the structure is calculated from the strain generated from the pressure load through the material constitutive relations.

Autodyn program is based upon Explicit method and is primarily used to model highly dynamic events in a very short time of period. In such events, the major deformation mode is stress wave progression.

When a pressure is applied to the end of a cylinder in your model, a stress wave is created at the end and is propagating inside the cylinder towards the other end. From the pictures in your post, you can see that stress wave travels farthur and farthur away from the pressure BC with time. A stable stress state could be reached after the stress wave has traveled back and forth along the cylinder many times.

If the stress from the pressure BC is the pre-stress in static equilibrium, you need to extend the End Time of your simulation to make sure the stress wave has traveled back and forth for several times along the cylinder length. At the same time, you need to apply Static Damping under Controls to damp out the dynamic oscillations of stress (or kinetic energy). Once the kinetic energy has approached zero, the material is in the state of static equilibirum and thus the stress state is static. Then you can conduct the subsequent dynamic analysis in the next load step.

You can find the instructions on how to determine the value of static damping from ANSYS Online Help at