The problem with the Fixed Support, is it doesn't let the face contract with the Poisson's Ratio of the material and so creates lateral stress in the face that is not considered in a hand calculation.
The way to get an ANSYS tensile model to have the stress you can calculate from Force/area is to use three displacements on three faces, one for X=0 on the face normal to X, a second for Y=0 on the face normal to Y and a third for Z=0 on the face normal to Z. This represents a 1/8 model of the center of a rectangular bar in tension.
Then the stress is uniform in the bar. Here is the Normal Stress in the Z direction.
The force was 200 lbs, the area is 0.62 sq. in so the stress by hand calculation should be 200/0.62 = 322.58 psi, which is what ANSYS calculated.
Your material model is multilinear. The first stress in the table is the yield stress of 896. This means the result above is in the elastic range.
In the linear range, the strain depends only on the Young's Modulus of the material. You used E = 2667 psi, so by hand calculation, we expect a strain of Stress/Modulus = 0.12095
If you increase the force, you can get this material into the plastic range.
I hope this helped your understanding.
Attached is an ANSYS 19.1 archive. (I can't easily tell if you use a different version, but you can say what version when you next attach).