Element size in explicit dynamic analysis with plasticity

[henki]

Hi,

are there any guidelines for element size/mesh density when performing impact/crash analysis?

With plastic material behavior, the stresses do not grow infinitely as the mesh density is increased. However, sometimes very fine mesh is needed to obtain converged solution, which results in slow and expensive computation. When the point of interest is for example the maximum plastic strain in the structure, should the element size be decreased over and over again until converged solution is achieved? Or does there exist some standard which says for example that "if the plate thickness is 5mm, then the element size should not be decreased below 2.5x2.5mm"?

-henki

 

[henki]

Let's take an example. I modelled a 500 x 500 x 500mm steel box (only 1/8 of the box to save time) with a plate thickness of 5mm. An explosion occurs inside the box and the used material model is Johnson-Cook. I performed an explicit dynamic analysis using CalculiX, therefore the only acceptable element available was underintegrated 8-node solid element. I put 4 elements through the thickness direction to capture the bending behavior. I performed the analysis using 4 different mesh densities and examined the plastic strain in the inner edge of the box where the stresses are the highest.

Now the obtained equivalent plastic strain in the integration point of the critical element with different mesh densities was:
- Critical element size 12.5 x 12.5 x 1.25mm, PEEQ = 0.076
- 6 x 6 x 1.25mm, PEEQ = 0.110
- 3 x 3 x 1.25mm, PEEQ = 0.136
- 1.25 x 1.25 x 1.25mm, PEEQ = 0.173
Of course the PEEQ grows when the element size is decreased, as the integration point approaches the sharp corner. But how would I know what is an appropriate size for the element?

I know this is a problem that should have been solved using shell elements, but there are no appropriate shell elements in CalculiX for this kind of problem. The smallest element size I used is way too small in my opinion for this kind of time-consuming analysis, but I don't know what size would be optimal.

I did a search on the subject in this forum, but found little answers. Most topics were concentrated on mesh density of static problems. Could using stress concentration factors to determine the critical stresses in this kind of problem be a valid approach to avoid overly refining the mesh? Or anything else?

-henki

 

[salmon2]

for explicit method, element size doesnot matter as solution will always converge. But depends on how detailed you want your results to be you may want to use finer mesh. Usually, I wouldn't mind using very fine mesh and let computer to run several minutes because "explicit" is always much faster than "implicit". I always prefer solid elements over shell element if I can afford the time.

I personally feel your results will more rely on your material model at your loading rate. Metal material at high loading rate will be brittle, not ductile any more. These data are often difficult to get.

 

[corus]

Why don't you look at the nodal values, which should converge as opposed to the elemental values for the reasons you've stated.

 

[henki]

corus, good point. Why didn't I think of that. I have to re-run some analyses.

By the way, which one do analysts more use as a design guideline: stresses and strains in critical element nodal point or integration point (as the stresses are more accurate in the integration point)? For example when plotting PEEQ against time, should I plot the PEEQ from nodal or integration point?

These things are not fully clear to me, as I don't have anyone to discuss these matters with in my workplace. I'm the only structural engineer in our company and I've just gotten off the school bench .

-henki

 

[corus]

Use the nodal values as these are on the surface, which is generally where highest stresses/strains are. Some people 'skin' the model with shell elements so as to improve the accuracy of the nodal values but I can't see the benefit of that if you're happy with the mesh you've achieved, ie. Nodal values have converged to a reasonable degree of accuracy.