Nonlinear fea showing permanent deformation

max

Hi there,

Regarding the step settings for Calculix, Is anyone aware of specifying the steps for simulation? 

For example: If I have 1 as the total step time, I would like to only run the simulation between step 0.8 and step 0.9 with a step increment of 0.01 (e.g. simulation will run at 0.81,0.82,0.83 up to 0.9). 

Any help would be much appreciated. Thanks everyone. 

Victor

I think you need two step sections (*STEP) for this. The first to get it started and make a single step to time 0.8, and the second one to produce the results you want between 0.8 and 0.9.

max

Thanks very much for your input Victor. Do you mean something in the form below?

*Step

*Boundary

*Static,Direct

0.8

*End Step

*Step

*Boundary

*Static,Direct

0.1,0.9

*End Step

Victor

Maybe more like

*Step

*Static,Direct

0.8, 0.8

*End Step

*Step

*Static,Direct

0.01,0.1

*End Step

max

Thanks Victor, I tried to follow your structure of declaring the step conditions. However when I ran the simulation, it seemed like the first step condition was only simulating at the total step 1.0 and the second step condition was running the simulation at every 0.1 interval (0.1, 0.2, 0.3 ..... 1.0), not only between 0.8 and 0.9. The second step condition exhibited the same results as if the step condition was to be set  as ".1,1.". 

Do you perhaps have any other ideas as to how I can get this to work? 

Cheers,

Max

Victor

Here's an example. I had to use TIME DELAY to get the load to continue where it left off. Not doing that would cause the load to start again from time 0 at the beginning of the 2nd step. That might be what went wrong in your case.

The .frd file it produces contains times 0.8, 0.81, 0.82, .. 0.9

max

Thanks Victor, I have tried to modify my code so it has the step definitions similar to yours. However, I am still having problems with getting the right step value. In my attached .inp file, I tried to have a 0.9 time delay so I can obtain results at times 0.91, 0.92, ..... 0.99. I am expecting the displacement in the Z direction to change according to the step times but steps 0.91-0.99 seem to be using the total time displacement value. Can you please advise on how I can fix that? 

Victor

The TIME DELAY parameter should be on the *BOUNDARY card, not *STATIC. You also need a *AMPLITUDE that explicitly specifies the ramping to use with TIME DELAY.

The solver shows a couple of warnings which are hard to find buried between all the iteration output for each step. They include:

 *WARNING reading *STATIC: parameter not recognized:

          TIMEDELAY=-0.9