In a Static Structural model, you have to use the Creep Controls under Analysis Settings to turn creep On.
This shows Creep is On in Step 2, which is because if you apply a force, you don't want it ramped on over 1000 seconds you want it on at a constant value, therefore, in Step 1 the Force is ramped on in 1 second, with Creep Off, then in Step 2 the force is constant. After the solution, there is an Equivalent Creep Strain result.
I made a model of a 1 m long part, that has 100 MPa of stress, and has 1000 seconds of creep time with a Norton Material with these artificial constants:
The total deformation at 1 second before creep is 1 mm, after 1000 seconds it is 2 mm.
The creep strain calculated by ANSYS is 0.001
Norton equation is shown below and can do a hand calculation of the expected creep.
creep strain rate = 1e-8 * (100 MPa) = 1e-6
creep strain hand calculation = 1e-6*1000 sec = 0.001
length increase due to creep = 0.001*1000 mm = 1 mm.
For those looking for real creep constants, pgl has this post.
ANSYS 17.2 archive is attached.