I can’t tell from the image if those are shell elements with thickness turned on or are solid elements. If they are solid elements, you can’t simulate plasticity effects without putting many elements through the thickness, at least 4 quadratic or 8 linear elements through the thickness if you used solid elements. A shell element has internal layers to keep track of plasticity. Look up in the ANSYS Help to see how many layers are in the shell by default. The number of layers may be increased by command so look for that also.
The curved part has no stress at the start of the simulation. I assume the bottom edge is a Fixed Support.
You must have the Shape Memory Alloy material properties in the material assigned to that part.
Try using a moment on the top edge of the part. That is more likely to reverse the curvature and is a simple boundary condtion to apply. You will need to take many substeps to smoothly apply this moment.
You need a multi-step analysis. Step 1 applies a moment, and step 2 sets the moment to 0. As the moment is ramped down to 0, the part will “spring-back” some amount. It is not sufficient that the part is practically flat at the end of step 1, you will have to go past flat and have some curvature in the opposite direction so that as the moment is ramped down, you have a practically flat part at the end of step 2.