peteroznewman
Subscriber
I'm guessing that the Frictionless Support is the planar face on the other end of the pipe. I'm also guessing that the Pressure is applied to the inside of the pipe. Correct me if I guessed wrong.
The Frictionless Support on one end is the same constraint as the Displacement at the other end. What these two constraints do is cause the length of the pipe to be fixed. Contrast that to a length of pipe that has no constraint on the length. As the pressure increases, the pipe will expand in diameter, but it will contract in length due to the Poisson's Ratio effect. The stress in the pipe wall will be radial (through thickness) and hoop stress (around the circumference) but the axial stress (Y axis) will be zero. If you fix the length of the pipe as you have done, you will get a non-zero axial stress. I'm assuming that is what you wanted, but maybe you will reply otherwise.
The reason for the pivot error is because the pipe is not tied to ground in all six rigid body motions. As you currently have it, the pipe is free to translate along the X and Z axes and rotate about the Y axis.
There are many ways to resolve this error, but I expect you want one that does not create any stress in the pipe. For example, a Fixed Support instead of a Frictionless Support would resolve the pivot error but would create stress at that end of the pipe, since it would not be free to expand radially.
Here is one constraint pattern to use: First delete the Frictionless Support.
Create a Cylindrical Coordinate System where the Z axis is along the pipe axis as shown below.
Create a Displacement condition on the unsupported face, set the Coordinate system to the new cylindrical coordinates. Leave the X-axis (radial) Free, set the Y-axis (tangential) to 0 and set the Z axis to 0. This completely supports the pipe.
You can keep the other displacement boundary condition at the other end if you want the pipe to have an axial stress, otherwise, delete that too.
ANSYS will still issue a warning, but this warning can be ignored because we know the model is fully constrained. The algorithm ANSYS uses to decide whether to issue this warning is not perfect.