Nonsensical Stress Values - Internal Pressure and Temperature on Cylinder 7

[mtz_engr]

Hoping to find someone that knows a bit more than I do on this matter.

I currently have a cylindrical geometry modeled and meshed with 2D Quad elements. This has been assigned Titanium material properties and a specified thickness. I have several load cases of combinations of internal pressure values (100 to 6900 psi) applied to the internal faces of the elements and temperatures values (-400 to 1000 deg F) applied to the nodes of the mesh. Both ends are fixed in translation and rotation. (intial temperature set as 70 deg F)

I started by performing a Linear Static solution to see what kind of results I got. I am interested in the tangential stress around the cylinder, because this is the principal stress and what should be the highest for this geometry. Interestingly enough, towards either end of the pipe, the stress values are highly negative (I am talking 100,000+ ... Saw -430,000 psi on one case) and the largest value seen towards the center is around 35,000 psi for the extreme case of pressure and temperature.

Doing hand calculations of the tangential stress causes by pressure and temperature, I arrive at around 93,000 psi for the combination of the hoop stress and thermal stress. I designed the geometry in the model to be able to handle this with a modest factor of safety.

Can anyone give me any indication of why the values I am getting in FEA are so strange? (Nonsensically negative towards the ends and positive but low towards the center)

Thanks in advance.

Using Patran/Nastran 2020

 

[Elphick]

I don't understand your argument of comparing thick-shell theoretical numbers to thin-shell results.

But considering your new dimensions and the material & pressure/temp loading specs which your have posted above I don't understand those theoretical numbers either.

I've hand-calc'ed (thick & thin) and there is no way you build up those stress numbers either at the middle or ends of the pipe.

What theoretical references do you use??

 

[mtz_engr]

Sorry if that was not clear.

The total is including contributions for the temperature caused by the temperature gradient as well as the pressure load.

For example, the thermal contributions are around 75 ksi, while the pressure contributions are around 18 ksi. (total of around 93 ksi)

The reason I was using both thick and thin forms of the hoop stress equation was to see how the FEA was interpreting the problem. I believe it is interpreting it as a thin wall problem, when it is actually a thick walled problem.
Not exactly sure how to account for this within the software.

The equation for maximum thermal stress in the tangential direction comes from the Timoshenko reference given by nlgyro

 

[Elphick]

You'll have to model your problem as a 3d solid FEM.


The peak thermal stress equation is based on a thin-shell assumption. You cannot use is as-is for a thick-shell calc.

 

[mtz_engr]

Well, I have since modeled it as a 3D Solid.

Pressure only cases match up with expected results from Lame equations for stresses in thick cylinders.

Temperature only cases match up with expected results as well from the equations found in the journal paper below.
Stresses were determined analytically using the Lame equation for pressure and integrating an equation for the thermal stress.
(

https://doi.org/10.1016/0020-7403(96)00001-X)

Just an update, to let you guys know I got everything working correctly and to thank you all for the suggestions.

I am now checking how much the results change wrt to mesh density.