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.