Stress at radius of formed area of C-channel 2

[Willstegs]

I have a formed C-channel with a 20k lb. load. Doing hand calculations I find the max stress should be 12,000psi. I calculated with an offset load. I then plugged everything into Mechanica and ran the FEA with a C-channel without radius from forming (To reduce the time to run) and found that I only have a large stress around 67,000psi on the corner of the channel where it welds to the girder. To see if the radii from the forming changed the results I added the radii and now have high stress of around 80,000 psi showing up near the formed radii under the load. Why am I seeing such a difference with just the radii being added? The results do not agree with my hand calculations also which makes me believe something is not modeled properly. Both ends of the girder are held in the x-axis but are able to rotate and move in the y-axis and the z-axis is able to rotate. The material is A572 Gr50 and I do not want to see over 28,000psi max stress.

http://files.engineering.com/getfil...f3c-b430-5a457286afa8&file=RadiusCchannel.pdf

http://files.engineering.com/getfil...b-9e45-28d32fad2160&file=NoRadiusCchannel.pdf

 

[Willstegs]

Sorry here is the file of the results without a radius

 

[shaun8567]

Both the 67 ksi and 80 ksi results are due to stress singularities.

For the first model (without the radius), your peak stress is at the corner where one c-channel joints the outer c-channel (creating a T-joint). This forms a re-entrant corner, which will cause a stress singularity. The high stress results from the effected elements can pollute the results, so local mesh refinement needs to be applied, and then the elements around the re-entrant corner need to be isolated and excluded from convergence study. They will still show up during post-processing, but you can just ignore them.

For the second model (with the radius), your peak stress is at tangent point between the radius and what looks like a channel plate. If you look at the two images attached, you can see how adding in the radius adds a very sharp knife edge, were as without the radius you only have a re-entrant corner. This knife edge will also result in singularities (and thereby higher stresses). You can try adding in a local mesh refinement, and then isolating and excluding the elements along the knife edge from the analysis. Your goal is to try and confine the elements with singular results to a very small area using small elements such that you can obtain accuracy results on the radius (thin of Saint-Venant's Principle).

 

[corus]

It looks to me as if there's something wrong with your results for the no radius case as the stresses aren't continuous. You'd expect to see similar results away from the radius (or lack of it) but the stress distributions aren't the same except at the attachment to the end channel where you see the obvious stress concentration of the sharp corner. In general this may be of concern if you're looking at fatigue but no mesh refinement will converge these results at that juncture at what is effectively a zero radius. In general opt for the properly shaped C channel to obtain the nominal stresses but at the juncture with the end piece look at the stress distribution leading up to that singularity and remove the peak stress component from the geometric singularity. These 'nominal' stresses at this position will be used for either a static or fatigue assessment.

 

[shaun8567]

@corus

I agree with you that no level of mesh refinement will remove a stress singularity (in fact, all it will do is drive it towards infinity), but willstegs is using Mechanica to do the analysis (a p-method code). This is important because if an analysis contains elements that have a significantly higher stress value on them (such as s singularity), then they have the potential to cause an increase in the inaccuracy of lower stressed areas elsewhere in the model.