×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Thermal Stress Analysis

Thermal Stress Analysis

Thermal Stress Analysis

(OP)
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: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

RE: Thermal Stress Analysis

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.

RE: Thermal Stress Analysis

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

RE: Thermal Stress Analysis

(OP)
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: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

RE: Thermal Stress Analysis

(OP)
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: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources