Static with Predefined Temperature Field versus Coupled Temperature Displacement with Temperature BC

[testing]

I'm trying to get thermal stress results for cylindrical and conical shells. I'm having some issues though with results not matching each other (and theory)

I've ran two simple cases with the same cylinder. In both cases, I model 1/4 of the cylinder, restraining the edges such that it can expand freely in the axial direction, is restrained to the theta=0 andd theta=90 planes at each edge in the circumferential directions and rotation is restrained at either axial end in order to model it as an infinite cylinder.

Material Properties:
E=200e9
alpha= 1.2e-5
T_outer=100
T_inner=200

Case 1: Static (1x1 S8R element)
Predefined temperature field with reference magnitude of 100 and -100 gradient through the thickness of the shell

The resulting stress is 0.1714 MPa which is 1/1000 of the theoretical value

Case 2: Coupled Temperature Displacement (1x1 S8RT element)
Temperature Boundary Conditions of 100 at the outer surface (DOF 11) and 200 at the inner surface (DOF 15)

The resulting stress is 171.4 MPa which agrees with the theoretical value


What could be causing this discrepancy? Eventually, I want to apply a more complex temperature field from outside of ABAQUS to a cylinder, but I need to verify that the answers will be reasonably accurate first. Ideally, I would be able to do this as a Static analysis with a predefined field, but if its not going to give me the correct result, I'd like to know why.

 

[mrgoldthorpe]

Double check that you haven't used E=200E6 instead of 200E9 in case 1.

 

[testing]

I've quadruple checked that the material properties are the same.

Playing around with it some more. Changing the section thickness from .001 to 1 moves the Static results in line with the coupled temperature-displacement results. The same change does not affect the result for the coupled temperature-displacement. Why would this be? Theoretically the thickness should not affect the resulting stress due to a temperature gradient in the radially direction.

 

[mrgoldthorpe]

It must be the temperature gradient then. Make sure the gradient you use in *TEMPERATURE in Case 1 is consistent with the units you use for length (and so shell thickness); which seem to be m according to your E.

 

[testing]

Ah, so the gradient for predefined temperature fields is specified as the change in temperature per unit thickness? That would make perfect sense why the results are not matching up. I was under the impression that the gradient value was the total change through the thickness (whatever it may be).

Thanks! That clarifies things