Dear Group, I am trying to simulate the behavior of a plate with hole, also known as the 'perforated sheet problem'. The manual provides a few examples. I picked the mesh from Abaqus Benchmarks Manual 3.2.17 Stretching of a plate with a hole but made the mesh much finer throughout and especially near the hole, using *NFILL,BIAS=0.9. My simulation typically uses 800 elements CPS4 and 867 nodes. The mesh defines 50 elements from the mesh to the edge. The theoretical solution for elastic behavior is named after Kirsch and gives all stress components in analytical form: http://en.wikipedia.org/wiki/Kirsch_equations I do not arrive at the analytical solution. The vertical stress component does not seem to depend much on mesh size. Using an extremely fine mesh my simulation could tackle the radial stress component near the hole, but quickly deviates from the theory when moving outbound from the hole. Note: these comparisons are restricted to the horizontal from the hole to the outer edge. I also experimented with the infinite element CINPS4 at the edge, even with an element length of half the distance from hole to the edge. Can someone recommend an appropriate meshing and possibly element type to get close to the theoretical solution ? Thank you for sharing your expertise Frank ----------------------------------------------------------------------- Frank Richter Institute of Materials Science Ruhr-Universitaet Bochum Bochum Germany |
Frank,
> I am trying to simulate the behavior of a plate with hole, also known as the 'perforated sheet problem'. > > The manual provides a few examples. I picked the mesh from > > Abaqus Benchmarks Manual > 3.2.17 Stretching of a plate with a hole > > but made the mesh much finer throughout and especially near the hole, using *NFILL,BIAS=0.9. My simulation typically uses 800 elements CPS4 and 867 nodes. The mesh defines 50 elements from the mesh to the edge. > > The theoretical solution for elastic behavior is named after Kirsch and gives all stress components in analytical form: > http://en.wikipedia.org/wiki/Kirsch_equations > > I do not arrive at the analytical solution. The vertical stress component does not seem to depend much on mesh size. Using an extremely fine mesh my simulation could tackle the radial stress component near the hole, but quickly deviates from the theory when moving outbound from the hole. > Note: these comparisons are restricted to the horizontal from the hole to the outer edge. > > I also experimented with the infinite element CINPS4 at the edge, even with an element length of half the distance from hole to the edge. > > Can someone recommend an appropriate meshing and possibly element type to get close to the theoretical solution ? Maybe you are hitting a mesh size that makes the elements too "thick" for plane stress? If a coarser mesh gives you the right results, this may be the reason, and then using normal plate/shell elements (e.g. S4 or S4R) might be a better choice for very fine meshes. Just an idea... Hope this helps, Fernando |
In reply to this post by Frank Richter-2
The theoretical solution is for an infinite plate, so I don't believe
you'll ever get the solutions to truly match, since you're forced to model a finite domain. The solution near the hole should match up well, and I imagine that as you increase the size of your plate the comparison might improve. I've never made use of infinite elements in a structural analysis, so I'm not sure what they'd do in a case like this. Regards, Dave Lindeman Lead Research Specialist 3M Company 3M Center 235-3F-08 St. Paul, MN 55144 651-733-6383 On 6/24/2013 6:48 AM, Frank Richter wrote: > > > > Dear Group, > > I am trying to simulate the behavior of a plate with hole, also known > as the 'perforated sheet problem'. > > The manual provides a few examples. I picked the mesh from > > Abaqus Benchmarks Manual > 3.2.17 Stretching of a plate with a hole > > but made the mesh much finer throughout and especially near the hole, > using *NFILL,BIAS=0.9. My simulation typically uses 800 elements CPS4 > and 867 nodes. The mesh defines 50 elements from the mesh to the edge. > > The theoretical solution for elastic behavior is named after Kirsch > and gives all stress components in analytical form: > http://en.wikipedia.org/wiki/Kirsch_equations > > I do not arrive at the analytical solution. The vertical stress > component does not seem to depend much on mesh size. Using an > extremely fine mesh my simulation could tackle the radial stress > component near the hole, but quickly deviates from the theory when > moving outbound from the hole. > Note: these comparisons are restricted to the horizontal from the hole > to the outer edge. > > I also experimented with the infinite element CINPS4 at the edge, even > with an element length of half the distance from hole to the edge. > > Can someone recommend an appropriate meshing and possibly element type > to get close to the theoretical solution ? > > Thank you for sharing your expertise > > Frank > > ---------------------------------------------------------- > Frank Richter > Institute of Materials Science > Ruhr-Universitaet Bochum > Bochum > Germany > > [Non-text portions of this message have been removed] |
Hello Robert, Dave and Fernando, thank you for your efforts. I picked that example only as a means to tackle the meshing. The plate in my simulation is larger, the path from the hole to the edge is four times the hole radius. Well, not much different though from that example. Kirsch's publication is from 1898, so one can conjecture that Michell was not yet up to date in the following year. A few examples in the manual inspired me to try infinite elements. I had the impression that one is able to "approach" infinite dimensions with that. The ABAQUS solution is close to the theoretical results for infintite dimensions, see the examples in Abaqus Benchmarks Manual, Chapter 2.2 Infinite elements From my limited understanding infinite elements are designed for structural analyses. In my simulation I made only the ones towards the right edge to infinite elements as the force is defined on the top face. Our simulation capabilities are currently limited to the student edition of ABAQUS and hence limited to 1000 nodes and 1000 elements. Once we have the full version I will model a very large plate with more nodes and elements. This problem is generally treated as a plane stress case, so the choice of plane stress elements seems straightforward. Regards Frank ----------------------------------------------------------------------- Frank Richter Institute of Materials Science Ruhr-Universitaet Bochum Bochum Germany |
This post has NOT been accepted by the mailing list yet.
In reply to this post by Dave Lindeman
I ran this problem using the following data: (I used symmetry condition)
square domain with a radius of hole = 1.0, corner point (10.0, 10.0), Applied tensile stress = 1.0 Horizontal, vertical, and diagonal (from partition) edges meshing: biased, size from 0.05 to 0.5 Far End Edges: 0.5 size Circular Edge: 0.05 size Element: CPS4 Applied, symmetric boundary conditions on the edges connected to hole, and far edges were left free. The results are shown below. Top two figures are at angle 0, and bottom two are at 90 degrees. The solution is converging, however, because of fea, one can not match it exactly with the analytical solution (specially near the hole: stress singularity)
--
An Engineer is Never Limited by Resources |
Free forum by Nabble | Edit this page |