About the stability criterion in Dynamic / Explicit analysis

[mandriam]

Dear all,

Here is a question(s) about the stability criterion in a dynamic explicit analysis.

In ABAQUS user's manual I red that the stability of an explicit procedure can be ensured if the time-increment is small enough. Then, as a limit criterion of stability, the given time-increment should be less than 2 / Omega. Omega is defined as the frequency of the entire system ... so my questions are :

1) I can't really see what Omega stands for ... does anyone see better than me about that said frequency ?
2) I also estimated the stable time-increment to be about 1,0E-07 s given my material's constants and given the smallest element size of my model (delta_t = L / c). Still, how can I ensure myself that the solution given by such a time-increment is sufficiently reliable indeed ?

Any response from you will be meaningfull I think I realise a tensile simulation using a viscoelastic law.

Thank you in advace,

Mandriam

 

[burningDiesel]

You can think of it as the time it takes a shockwave to pass through an element, which is directly related to the element eigenvalues (eigenfrequency). So you can imagine that your time increment has to be lower than this time, else you will never be able to 'see' these shockwaves!
(So this is a conceptual explanation, for the actual theory, look up the the CFL (Courant-Friedrichs-Levy) condition)

In practice, ABQ calculates it for you, using an element by element algorithm, which conservative. As you can imagine, boundary conditions etc. compress the eigenfrequency spectrum. There's also a factor 0.9 in there somewhere I think (you can probably find it in the theory manual).
There's also an option to let abaqus calculate the time increment for the entire model, but I never use it because the time you win with the higher increment size is lost again by abaqus calculating this value.

So long story short, just use the abaqus default, and it's by definition conditionally stable (and conservative).
Also if you use damping the increment size is reduced, but again abaqus will do this automatically.

 

[mandriam]

Thank you much for your quick reply !

Okay, so if I understand, the time increment has to be small enough in the sense that a shockwave shouldn't have time to cross that element more than once during an incrementation.

It's indeed clearer. Though, about the effect of boundary conditions on the eigenfrequency, which is one of my first interests, I haven't found yet how ABQ determined that (i.e. how it redefined the increment-size in function of the boundary conditions). The problem that I had is that I saw signs of instabilities when I increase the rate of deformation I apply to the model. Then I corrected my boundary cond. but I think it's better if I could justify the new boundary conditions are safe enough and prevent form new instabilities phenomenon.

I may spend more time to figure that out, but right now I got to admit the increment size given by ABQ is conservative enough.

Anyway thanks again !

 

[missil3]

There usually is a factor of safety used when determining the timestep by the software. @sdebock says its 0.9 by default for abaqus ? This factor is important if you are loading occurs very quickly you should use a lower value for the factor of safety (0.65 - 0.7). This results in an increase in computational time obviously but might be required to get good results.

I don't know about ABAQUS but in LS Dyna there is a number of ways the software can calculate the characteristic length required for timestep calcuation. Usually it is the shortest diagonal, or based on area or someother formulation).Then the time taken by sound/shockwave to travel the characteristic length is your timestep.

I am not sure how your boundary conditions can be related to the stability of your solution in an explicit analysis ?

 

[mandriam]

Hi all,

Here is what SIMULIA customers help says.

Q :

In an Abaqus/Explicit analysis, is the loading taken into account in the calculation of the stable time increment?

A :

(The following applies to any version.)
No, loading and/or load type is not directly considered in the calculation of the stable time increment. The numerical stability of the system is solely governed by the condition of the mesh.
This does not mean that the numerical stability of the system is not influenced by the loading, but only that the influence is indirect.
The effect that external loading may have on the stable time increment or the stability of the system comes through the affect of the loading on the deformation of the model. For example, if the loading causes the model to deform in such a way that the highest natural frequency increases, then the stable time increment may decrease.
Additionally, if the load (force-based or displacement-based) is too large or is applied too rapidly, then the deformation speed can become too great. In this case, Abaqus/Explicit will issue warnings and if necessary stop the calculation with the message
***ERROR: The ratio of deformation speed to wave speed exceeds 1.0000 in at
least one element. This usually indicates an error with the model
definition. Additional diagnostic information may be found in the
message file.
In this case, applying the load with a smooth step amplitude definition, scaling the stable time increment, or using a finer mesh may alleviate the error.

 

[mandriam]

My personal guess is that one studying the stability of dynamic explicit simulation has to distinguish two things :

1. The calculated stable time increment, that depends on mesh condition, materials constants such as density, elastic constants, and then the characteristic speed wave.

2. The other one is the limit of stability that depend on boundary condition (meanly the rate you deform your material). In the way that B.C. can affect the entire system frequency. Understand, the system proper frequency is the one obtained by using M (mass matrix) and ü (acceleration). Though I cannot tell more about that system frequency since it’s not clear even for me.

Then I think, ideally the best compromise between your boundary conditions in one hand, and your meshing conditions in another hand, would be that 1 << 2. Understand, the conservative time increment calculated by 1 (whatever its value is, 10E-3,-4, -7 etc.) should be far less than the limit time increment calculated by 2. But both are called stability criterion.

 

[IceBreakerSours]

There is a section in the ABAQUS Theory Manual that talks about characteristic element length. Search the following keywords in the documentation: Convection diffusion characteristic element length Yu Heinrich.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083