I use Inventor Pro 2012 to do static FEA analyses. In most cases if the assembly is "simple" the convergence plot has a smooth shape(Figure 1). On contrary, when having a rather complicated assembly of parts i get a rather inconsistent plot.
Can someone please explain to me the possible reasons and meanings of the different factors. Im releatively new to FEA and would like to know more in depth the meaning of "h refinements", "stop criteria" and "h refinement threshold".
Thanks in advance!
Solved! Go to Solution.
It is difficult to provide a general answer to your question, but in my experience when the convergence plot shows as figure 2 (slope having large change between solution steps, or a subsequent step displays a decreasing value) it could mean the location of maximum stress (where we are performing the h-refinements) is changing location on the model, or we are attempting to converge at a stress singularity.
[Edit: What the plot doesn't tell you is if the 'Solution Step' was a p-refinement (degree of polynomial of the displacement field within an element) or an h-refinement (smaller 'local' mesh size). It could be that a sharp increase or decrease was due to a p-refinment and not an h-refinement]
The setting you mention are explained in the help system here (or press the help button in the Convergence Settings dialog) : http://wikihelp.autodesk.com/enu?adskContextId=RED
Please let us know if you need additional clarification of the meanings of each setting.
Thanks and Best regards, -Hugh
Thanks for such quick reply to my post. Very helpful information. Could you explain more on "attempting to converge at a stress singularity" please.
I understand the concept of changing the maximum stress location, but what does it mean to converge at a stress sungularity?
A stress singularity is where: as the mesh size is decreased, the stress increases. These happen at geometries like a sharp inside corner.
Convergence: We refine the mesh at the maximum stress location, to ensure that there is not a mesh size dependence that could affect the result value. i.e. the more dense mesh could give false indication of the 'true' stress value at that location.
In the following simple example, it shows a model with a sharp inside corner. Depending on the loading, it may or may not be a maximum stress location. However, since it is a sharp inside corner without any fillet it is likely going to be a stress singularity location (geometrically and load symmetric):
Also, keep in mind that in reality, an inside corner is most likely not a perfect sharp corner. The cutting tool must have some kind of finite radius, which would leave some sort of small fillet, and not a perfect 90 degree corner that we can model in CAD. So these singularities can easily be a result of the CAD model whose geometry doesn't even match with the real-world model:
If we simulate using the default mesh, and no convergence, the maximum stress would be equal at both inside corners in 'real life'. But, when we show the maximum stress label / indicator. It cannot point to both locations, just one. This is why I mentioned that it is possible for the convergence to change where in the model were are refining the mesh:
Now, let's use convergence and set h=3 and Stop criteria % = 3. The adaptive mesh refinement will begin to refine the mesh at the high stress location, to try to converge on a stable max stress value. However, since the max stress occurs at the sharp inside corner / singularity, the solution for the max stress value can only diverge:
In order to overcome this inherent behavior with any FEM / FEA package, we can either add a small fillet to the sharp inside corner, or exclude that sharp inside edge and neighboring faces to be included in the mesh refinements for convergence (using the Geometry Selections highlighted in the image above in the Convergence Settings dialog). Alternately, you can use the option "Include Selected Geometry" so that we will only consider the nominated geometry for mesh refinement in convergence. In this simple example, perhaps you are interested in the face on the opposite side of the column from the sharp edge to converge the max stress results.
A different example I could use is a pointed object (like a sharp wedge) pushing on a flat planar face:
In reality, since an edge has zero area, and stress = Force / Area. The stress should be infinite. However, in FEA Stress Analysis,we don't give an infinte stress value using the default mesh. Only using a very fine mesh can you see the stress will diverge to infinity.
What would happen in reality, is that if the force is great enough, it will cause the sharp point to deform a bit, and the contact "area" will no longer be a line, it will have some small area. This will distribute the load over this area, and thus decrease the stress to a reasonable value. However, the stress analysis in Inventor is what we call Linear Static Stress, which we cannot simulate large deformations, or changing the mesh to update to a new one that will mesh the deformed body. This would require a non-linear analysis that can take into account geometry changes and strains even beyond the yield point of the material. Autodesk Mechanical Simulation has nonlinear analysis capabilities.
Hope this helps! Please let us know if you have any additional questions, comments or suggestions.
Warm regards, -Hugh
Log into access your profile, ask and answer questions, share ideas and more. Haven't signed up yet? Register
Start with some of our most frequented solutions to get help installing your software.