Factoring the stiffness matrix only once in multiple steps ?

[thecirclingman]

Hello !
I'm running Abaqus/Standard 6.7-1 to analyze a large structure (500,000 DOFs) using linear elasticity, with many load increments involved --- there's like 200 of them, and I need them because submodeling comes next. It works fine, but the process is pretty long.

By looking at the log files I've noticed that each of those increments takes about the same time to compute, which means Abaqus probably re-factors the big stiffness matrix at each increment. However, I'm almost sure the matrix is the same from one increment to another, since I'm using linear elasticity, without NLGEOM and without changing boundary conditions...

Is there a way to "tell" Abaqus that the stiffness hasn't changed and to prevent it from re-factoring the matrix many times when once would be enough ?

 

[johnhors]

Why?

As far as I can tell you are running a purely linear analysis in multiple steps, which means that the results of each step are all linearly related. You could run this model just once and get the results for each step by simply factoring your one set of results.

Please can you enlighten us on why you need this for submodelling?

And the answer to your question, yes Abaqus does know the stiffness hasn't changed, it will only re-compute this if it does change.

 

[thecirclingman]

Thanks for your answer !
Hmm, if you're sure that Abaqus "knows" the stiffness hasn't changed when it reaches the following steps, then I have no problem at all

However, in my case, at the end of the .msg file I see that the 198 increments involved "198 passes through the linear solver", and "198 decompositions of the stiffness matrix". If I understand it right, this should mean the stiffness was re-factored at each increment instead of just doing it once. Is there a way to be sure about this ?

I'd like to factor a set of results, and I'll maybe eventually do this, but the loading is really complex here - the model is a simplified high pressure turbine blade with thermal, centrifugal and pressure loads, all varying differently along time.

And I'm concerned about efficiency because I'm doing R&D work on an experimental technique : some kind of "iterative submodeling", that consists in updating the global results from the submodel's results when the differences between the two models are important. This improves accuracy but requires some extra runs on the global model, and I'm trying to optimize everything to make sure the process isn't too time-consuming.

 

[hondaknight1]

Hi,
IU dont know anything about Abaqus --
but you say "the loading is really complex here" as a counter argument to JOHNHORS advice to factor a linear model. But this really doesn't make any sense, its a common misconception in FEA that because the loading/geometry is complicated that you have to make separate calculations for each change in load. But all you really need to do is carry out an analysis at unit load and then factor the results by your load at each load case so if you apply 100% of load in step 1, then in step 2 you reduce it by 20% then you have 80% load, it really is a simple as that.

I've come across many people who dont believe this, you can prove it by doing 2 steps in a linear analysis and comparing the result to a factored result from unit load, and you will find no difference.

This goes on to be applied to your iterative submodelling, if its linear, then its just a waste of time...

 

[thecirclingman]

Yes, of course that's right. If the loads were directly proportional to each other then I would just have to analyze the first one and scale the results ! I've also faced this misconception many times.

However, it's not that simple here, and the load set at step 2 is not just the load set at step 1 multiplied by some factor. Not even close, actually --- and no linear dependency between the successive load sets can be noticed. That's why I am concerned about having the stiffness matrix factored only once...

 

[rstupplebeen]

I have run models that have complex loadings and I modeled them each as separate unit loads in their own step. Then using linear superposition I created all the combinations of loadings. This was a 9 DOF loading but this could be expanded or contracted for you application. The real trick is to efficiently present data in N dimensional space. I hope this helps.

Rob Stupplebeen

 

[hondaknight1]

So is the load at step 2 in a different location or on a different vector?

 

[truckcab]

If everything is purely linear,then you can use the *LOADCASE facility. Check that keyword in the documentation. Works as SUBCASE in a linear Nastran analysis.



Live Long and Prosper !

 

[truckcab]

The syntax is as follows:

*STEP
*STATIC

*LOAD CASE (First load case)
(*CLOAD, *DLOAD etc.)
*END LOAD CASE
...
...
*LOAD CASE
(*CLOAD, *DLOAD etc.)
*END LOAD CASE (Last load case)

*END STEP

Check the docs for a more thorough description.



Live Long and Prosper !