Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Max/Min Stiffness ratio

4 REPLIES 4
Reply
Message 1 of 5
mike
1098 Views, 4 Replies

Max/Min Stiffness ratio

I'm wondering what is considered a high max/min stiffness ratio 1 x 10^13? , 1 x 10^12? When is a warning triggered in Simulation?

4 REPLIES 4
Message 2 of 5
John_Holtz
in reply to: mike

Hi Mike,

 

I believe that 1 x 10^10 is the limit that triggers the high max/min stiffness warning.

 

To put it in a simple example, imagine adding 1 x 10^6 and 1 X 10^-4 (a max/min ratio of 10^10). The result is 1.0000000001 x 10^6. That is getting close to the limit of precision in today's computers (15 or 16 digits normally), so some precision can be lost in the calculation. How the inaccuracy propogates through the solution is difficult to predict. So my suggestion is to be cautious when using results from analyses with such warnings. If you understand why the warning occurs in each model and "know" that it should not influence the answer, then it may be safe to use the results.

 

As with any analysis, you should check all of the results (displacement, stress, reactions, temperature, heat flows, etc) to check for potential errors.

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 3 of 5
S.LI
in reply to: mike

I'm not very clear on your question.

But a ratio like this seems too large for current double precision solver.

Usually, it causes unstable, bad accuracy results.

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 4 of 5
sunj.autodesk
in reply to: mike

Hi Mike,

 

This value is calculated by measuing the max and min diagonal terms in the system stiffness matrix. Usually it will print as a warning as you see in the log file to indicate your matrices might have some problem. However, under some cases such as when MPCs are used with Penalty method, or some initial boundary condition is used, this warnig can also be seen.

 

As long as the solver does not give you error messages, you can pretty much ignore it. But as John suggested, do be cautious you observe the results is against your intuitive. If that happens, this warning might give you some clue to check your modeling details.

Message 5 of 5
PipePakPat
in reply to: mike

I have seen only two models that produced problematic results relating to this stiffness warning.  The stress results were obviously incorrect, as they appeared in "spots" on the model... like a 12 year old's acne problem.  In these cases, the stiffness warning exceeded 1e20.  In these cases, the models contained "Gap" or "Boundary Elements" where the stiffness was defined.  Changing these gap and boundary element's stiffness to 1e10 solved the problem both times.

Pat Tessaro, P.E.
Premium Support Specialist – Simulation

Autodesk, Inc.
6425 Living Place
Suite 100
Pittsburgh, PA 15206

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report