Thermal Stress Analysis

[Drej]

Guys,

I'm undertaking a sequentially coupled steady state thermal stress analysis of a simple square plate, using DS4 elements in the thermal run and S4R elements in the thermal stress. This problem has a closed form solution. I have carried out the analysis using standard SI units (kg-m-s) and the answer I get ties perfectly with closed form. Tick in the box.

However, I need to run this model in units of (mm-tonnes-s) and when I convert my model, the answer just isn't 'correct'. The mm-tonne-s model I use has been converted to mm dimensions, and I have converted the units correctly, or so I think, since I have produced the same model in ANSYS - using the same unit conversion of mm-tonne-s, which gives the correct solution. Mind-boggling.

There is significantly more displacement in the tonne-mm-s Abaqus model, which gives rises to significantly greater stresses.

Anyone ever come across this? Any thoughts?


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[TGS4]

I've run into these type of issues before too. Please list the units that you are using for ALL of your material properties and load/stress parameters. It's probably a small something.

 

[corus]

Firstly I'd check your thermal analysis to make sure you have the same answers as your original. W/mm^2 will be 10^6 different from W/m^2 obviously, and Specific heat in J/kg C will be a thousand times different in tonnes, etc.

corus

 

[Drej]

Thanks for the replies.

It turns out that there is a TEMPERATURE option on the *SHELL SECTION card that needs to be included and defined.

The documentation is a little difficult to understand, but you basically need to specify the number of section points through the shell for the thermal stress analysis. This must be used for temperature mapping.

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Drej]

Just one final comment in addition to be wary of. The *INITIAL CONDITIONS, TYPE=TEMPERATURE card for shells requires you to input the temperature for each section point of the shell. For a 'standard' five section points through-thickness this would be:

INITIAL CONDITIONS, TYPE=TEMPERATURE
N_ALL,20.,20.,20.,20.,20.

to ensure that all section points through the shell in the node set N_ALL maintain the same temperature. If you only input a single temperature:

INITIAL CONDITIONS, TYPE=TEMPERATURE
N_ALL,20.

the 20 is assigned only to the default 'top' section of the shell.

This will give you a non-uniform temperature through-thickness.

Be warned!


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com