Factor of safety result causing concern.

Yash,

I don't have access to SW Simulation right now (and don't really have time to spend on it if I did have access), so I can't be much help. Plus I am not at all familiar with how it works, most of my FEA being done with ANSYS. I might be able to help a bit if you could show some of the results that you are worryied about and give some more explanation of your model, boundary conditions, and what you are expecting.

It looks like your file was first compressed with rar and then zipped. A lot of people don't have the rar software, so it would be much better if you just zipped the files or let the forum software zip them for you.

Jerry Steiger

I've checked your model and the main issue there is the presence of geometric singularities due to sharp inner corners. Regardless of material properties or fabrication processes, sharp inner corners are not common or impossible in real parts, there will be always radii as small as they would be. Thus, results near sharp corners are not correct.

Sharp edges in finite element analysis evaluate as infinite stresses due to a strain direction discontinuity just in the corners.

In order to overcome this problem, estimate a real fillet radius (no matter how small) and apply proper mesh controls in the edges and face of such radius. Use curvature mesh control to mesh more than six elements at fillets. Check Peterson's Stress Concentration Factors, pretty good literature regarding these subjects.

Regards

Yash.  Although Angelo makes a good point about stress concentrations, I have run your model to convergence and the regions that are predicted to exceed yield go well beyond this corner. 

So the only suggestions I have are to double check your load magnitude, material properties, and the manner in which you are loading the part.

Hi Yash, What are there at hole connect? Example pin, shaft,..

Several good points have been made here.  The area where over which the force was applied does appear to be inaccurate, given that the load comes from a cable running along the lower cupped portion of the part.  The load applied to the vertical face would result in more bending than the part would actually see.  Have you re-run with split lines to isolate the load to the actual area of contact?  Also, I'm assuming this was run as a linear static study.  That is fine, but be aware that any information on stress magnitude above yield is meaningless.  Also, the region of material that is predicted to exceed yield is likely exaggerated because due to the same reason... stresses are calculated from displacements and are extrapolated linearly from E, although in reality, the stress-strain curve does not follow a linear path post-yield.  This results in an artificially still part.

Two questions going forward would be:  1) Is yielding still predicted with the updated, correct loading and 2) If so, what is the actual response post-yield.  If you need to know #2, then you will have to run this as a nonlinear static study using accurate data for the nonlinear stress-strain curve and material model.  If you are also talking about the effect of repeated loading, then you will need to take into account hardening, which can be specified in the nonlinear study properties.  This is likely what cause the part failure in the physical test Mikael described above, similar to bending a paperclip back and forth until it breaks. 

I ran it again with the load face limited to what I would roughly expect to be the cable contact area.  The restult actually looks worse than before.  Approximately 72% of the part is predicted to exceed yield.  Again, post-yield data must be taken as approximate, but I would say that it is not possible to reorient the force and have the results come out below yield.  Something else is up here.  Can you confirm the load and material properties?  Do you really have ~9000lbs on a 5" x 3/8" thick aluminum bracket? 

Plot below shows volume of material above yield limit (~72%)

Out of curiosity I did a quick search for the alloy and believe LM6 is a cast alloy spec for aluminium?

http://www.hadleighcastings.com/uploads/LM6%20Alloy%20Detail.pdf

If it is cast then the material properties are most likely influenced by the cast integrity of the final part and local imperfections - there is likely to be variabllity in the nominal properties from variances in the alloying and cast process.

If you are working with high stresses and safety/risk is of high concern then the properties should be determined from samples taken from a cast part - a standard for mechanical properties for this alloy would nominate the properties and tests required. The foundry undertaking the casting should have good process control, records and traceability.

The elongation at break from the properties you've shown is 3.5%; this would seem to indicate a brittle material with potentially little ability to deform to redistribute concentrated stress areas before a brittle type failure. Impact loading would also be an issue. What safety factor are you assigning to the minimum material yield properties to arrive at a maximum allowable design stress. There should be some sort of standard for this product what do these indicate as appropriate?