First, I am impressed with all the strategies taken for meshing, most importantly using curvature based mesh.
My best suggestion always for the mesh either in FEA or CFD is to assure that your simulation is "grid independent". To clarify, your simulation results should not change 'considerably' from one mesh resolution to another one. Having said that, it is generally recommended to have couple of different mesh resolution and refine the mesh up to the point that the deviation in results becomes minor and negligible based on your design intent. The only consideration in FEA is 'Singularity' which can be verified throughout applying finer meshes closed to hot spot regions for the stress at sharp reenterants, wherein stress escalates notably and goes to infinity. There are some techniques such as applying a small fillet to get rid of singularity, however, if those don't work, then you should ignore those artificial high stresses.
Hope it helps.
Hi Siavash, my apologies I didnt see that you had replied to my question, what your saying makes perfect sense.
way to select the mesh size is, there must be minimum 3 elements across the thickness of the part.
based on this select the mesh size range followed by convergence test.
- ananda ganesh
The 3 elements thru the thickness is a guide line and is often over kill depending on what you are modeling. For bending the sim tet10 element is quite good at bending behavior - in my experience it is better than tet10's in many other codes. Best to do a test and explore how many elements it takes to get what you are after. I have done many jobs (with validation experiments to verify bending response as a function of thru the thickness number of elements) were 1 element through the thickness models bending nearly identically to 5 elements through the thickness. Where it deviates is near the restraints, not at the maximum bending stress region for a simple beam. The investigation of regions of high stress gradient would be a whole other subject and all bets are off on how many elements are required - a convergence study would be required.
Good morning Ryan,
First let me address your main question (Does it just boil down to the smaller the element size, the more accurate you get.). In a very general sense yes (if you mean precision), but it is important to realize that the solver becomes more precise in regards it its own internal convergence. The accuracy of the sim is totally dependent upon the application of fixtures, contacts, external loads, and material properties, in regards to the phenomena you are modeling. Two large deciders for this are 1: Are you happy with the degree of precision you see out of your iterations? 2: Do I have enough resources to spend to get my .001% convergence and is it worth it? So, you can just go ham with your mesh, but a much more effective way of meshing is to first map out your load paths, where ever loads transfer, a refined mesh is highly recommended. As far as to what degree and type, this depends on your convergence preference (your comfort) and the type of contact condition/boundary condition you have (I have a white paper somewhere that goes into detail about different meshing and contact practices if I find it I will edit this post). Side note, make sure you also look at your a/b ratios when refining meshes and adjust them accordingly depending upon your application it doesn't do you much good to go from a .1" element size to a 1" element size because it creates an extreme, a transition is needed (the degree of transition is controlled by your ratio). To that note, there is much more to mesh refinement than just simply the element size there are many different element types as well (I'll dig for that white paper...).
Your second, unasked question, is (Is the mesh the actual problem?) How you look at/what data you look at with respect to the mesh is important as well. For example, if you are getting strange singularities or hot spots, viewing your plots as discrete elements instead of continuous will help you determine if it is a mesh problem. If your stresses go from a minimum to a maximum in a single element or the transition to a maximum from a minimum is very abrupt you should refine your mesh in that area, inversely if you find a nice transition and you don't like the numbers you are getting I would review the simulation set up (contact conditions, fixtures, load applications, material properties, maybe even the type of simulation) and ensure everything is in order with what you are modeling.
Feel free to upload your model I'm sure all of us will help where we can!
(PS- apologies for the windy post)
Take a look at the attached image. Deciding which mesh is sufficient for what depends on what you are after.
From the information presented it is easy to see what the impact is and the decision is easy. Do this type of thing with whatever you are working on and it will become obvious for you as well. The key point is that you should not focus solely on the maximum value that a given mesh produces but on its global or local behavior and what you are trying to sort out. Its an estimate, just like a hand calc or any other calculation.
tet 10 in bending.png 486.1 KB