Difference in simulation results by changing element size in LS-DYNA 1

[boar]

Hi everybody
I am trying to simulate a flying steel pipe with it's axis perpendicular to the center of a 2x2 m' steel plate (50 grad steel) 30 mm thick.
the pipe is 12 c"m diameter and about 6 mm thickness A36 steel with a velocity of 340 m/sec .
The pipe and the plate are first modeled as shell where the plate was divided into 40x40 x30 mm elements.
The plate was ruptured after 5.2 m-sec and the residual velocity was 130 m/sec.
Then I divided the elements in the zone around the plate center into 4 elements ( 20x20x30 mm each) , I got rupture after 3.1 m-sec and the residual velocity was 237 m/sec.
Then I changed the plate to solid with elements size of 40x40x15 mm and I got rupture after 3.2 m-sec and the residual velocity was 215 m/sec.
Then I divided the elements in the zone around the plate center into 8 elements ( 20x20x7.5 mm each) , I got rupture after 2.2 m-sec and the residual velocity was 290 m/sec.
Of course I did not change the other properties like material and contact (Automatic-surface to surface)
Is there any reason to such big differences in the results ?
Thanks

 

[JGard1985]

A flying steel pipe, this project sounds familiar to so many we have done at our firm. You aren't by any chance designing for a Nuclear Regulatory Commission tornado missile?

In any case you are dealing with issues of mesh convergence. The finer the mesh, the more nodes and degrees of freedom, therefore the better LSDYNA can model the response. Read this blog post on convergence and mesh independence Blog Post: FEA Convergence and Mesh Independence. Its for a simple beam in bending, but the procedures are the same for your problem.

Modeling the response includes element failure and energy absorption. A rough element mesh may just fail a couple elements quickly with little energy absorption (hence higher residual velocity). Also you need to look at LSDYNA contact definitions, eventually with very hard impacts, and a rough enough mesh, nodes can slip past eachother. You dont want this.

Keep refining the mesh and re-running. Eventually you will find that your model will converge to a steady solution (e.g. residual velocity is always XXX m/sec) and a finer mesh will have no impact on results.

When this happens you have achieved convergence and you know that the results are mesh independent.

FYI: I'd also recommend checking your results for penetration against hand calculations developed within BC-TOP-9A

Hope this helps

Jeff
Pipe Stress Analysis Engineer

http://www.xceed-eng.com

 

[boar]

Tanks JGard for your response
The problem is that I checked this simulation with CONWEP software developed by US army ,for projectile penetration, and I get around 100 m/sec residual velocity.
I thought that maybe when I divide elements around the center of the plate I disconnect some of the nodes from the undivided adjacent element
thus I weaken the section and get higher residual velocity
Am I wright ??

 

[JGard1985]

Post a picture of your mesh. You really want it to be continuous with each adjoining element sharing nodes. You don't want unconnected nodes. They'd be pretty visable in the output. You could just apply a point load at center of the panel and watch the stress distribution, any unjoined nodes would be pretty evident by stress concentrations and disjointed contour plot gradients.

That said some other things to look at

-Look at your kinetic energy. Does the pipe have the correct initial kinetic energy?
-Do you have errording surface contact on for your plate. Make sure you do or once your outside solid elements fail the pipe will sail right through
-Are your boundary conditions the same in shell vs. solid models. Fixed vs. simply supported? Check to see if you have rotation or stresses at the edege of the plates. Stresses mean your edge is fixed, rotation means edges are probably pinned
-Definitely need to have have 6-8 elements though thickness. Having a single element has only 1 integration point, so many of the results that LSDYNA provides are pretty much garbage, as they occur at the neutral axis
-Check out [URL unfurl="true"]https://www.nrc.gov/docs/ML1409/ML14093A217.pdf[/url] equation 2-11 for another empirical method for determining resultant velocity following perforation of a steel plate. You need weight, and the equation is empirical so you have to work in units it specifies

Hope this helps!

Jeff
Pipe Stress Analysis Engineer

http://www.xceed-eng.com