Need help interpreting FEA stress results - Stress concentration 2

[Marko04]

Hi,

I am currently designing an assembly (clip) that will be used to fasten the architectural panels/cladding to. The clip is fastened to building wall substrate and is suppose to be able to carry both the cladding dead-loads plus resists the negative wind pressures (pull force).
The clip assembly is made out of 6063 T5 Aluminum. It consists of two aluminum parts and one thermo-plastic part (thermal-break). The two aluminum parts' crimping legs are crimping the thermal break and keeping it ib place. The crimping force is strong so shear failure where aluminum crimping legs pinch thermal break is not an issue here. What I am trying to see
whether or not these aluminum legs will fail when the clip is subjected to a dead load of 65 lbf at its very end and a windload of 215 lbf. ( The cladding dead-load would be a vertical force vector creating a bending stress on the clip while the wind load would be a horizontal force vector creating a tensile stress on the clip). When I run the FEA analysis I get high stress concentrations at the inner corners of crimping legs. I would like to know from the FEA results I obtained whether these crimping legs would deform/fracture while resisting the above mentioned loads since they have high stress concentrations at inner corners that are approx 3 times greater than the 6063 T5's yield strength. (Highest stress: approx: 63000 psi, 6063 t5 approx yield strength: 21000 psi). Will these stress concentration ( red areas shown in inside corners of crimping legs) cause a crack and ultimately failure in them? Or will the region around the stress concentration undergo plastic deformation, re-distributing loads elsewhere causing no issue/ no failure? I would greatly appreciate your input. Thanks.

Below is an animation video of the assembly and how it would behave with the loads I mentioned above:

http://www.infinitelooper.com/?v=SWolYhOyTEY

Image of high stress concentration in the inside corners of the crimping legs:

http://files.engineering.com/getfil...623-523b7747b4c1&file=2016-08-24_13-19-45.jpg

Crimping legs zoomed out:

http://files.engineering.com/getfil...ffb-ebc68820bf48&file=2016-08-24_13-15-55.jpg

Crimping legs holding thermal break in place:

http://files.engineering.com/getfil...5cf-9fae67a4a66d&file=2016-08-24_13-11-02.jpg

 

[SwinnyGG]

As a sanity check, what are the rough dimensions of the parts in question here?

One thing to consider which I'm assuming is not present in your model- what does the clip look like before it is crimped over the central extruded piece? Are you leaving residual compression forces in the root of that radius, which would reduce the stress applied through tension?

My gut instinct from your stress plot is that the stresses shown are overly localized, meaning that the model is predicting higher stresses than would exist in real life. This means that either assumptions need to change, the mesh needs refinement, or you should apply a different stress calculation scheme (centroidal/elemental stress instead of nodal).

One of the sure-fire signs that a stress plot has hiccups is a very sharp gradient in stress over a very small area, as is present in the root radius of your clip.

 

[Marko04]

Thanks for the response jg,

The total clip length is 5 inches. Good question. Below is an image showing the geometry of the extruded crimping legs before they are crimped vs crimped. To understand, are you suggesting that these residual compression forces found on the inside radius plane have been "built up" by the crimping action? (since during the crimping the inside radius surface would undergo compression). Does this mean what you are saying that this "pre-built" / pre-added compression force will help combat the tensile forces pulling on the clip and thereby reducing the overall tensile stress in that region? I am wondering when aluminum legs are crimped they essentially are being intentionally deformed, being bent about the root of the radius and compressing that radius plane, does this compressed/ deformed radius have now residual compression added to it? In other words, by same logic, when a ductile material like aluminum ( eg aluminum rod) is say for example stretched out so it yields slightly (elongates) does this mean that there is some residual/extra tensile stress contained within that rod after it has yielded? Please bear with me as I am an industrial designer with some limited engineering knowledge so I am trying to understand the concept.

I was also considering that the stresses seemed highly localized. I did a mesh refinement and applied h-adaptive looping (SolidWorks Simulation software) to get a proper mesh element size.


Pre-Crimped vs. Crimped ( Notice in the Crimped geometry that the "nose" of the legs is fully embedded in the plastic central piece whereas in the un-crimpied its not.)Do you think I should then do another analysis
on a pre-crimped extrusion and see how much compression force has been "built up" in the radius profile plane?

http://files.engineering.com/getfil...a0a-503114a1aa32&file=2016-08-25_10-33-20.jpg

 

[SwinnyGG]

To understand, are you suggesting that these residual compression forces found on the inside radius plane have been "built up" by the crimping action? (since during the crimping the inside radius surface would undergo compression).

Yes. Any time you impart plastic deformation into a part, you are left with residual stresses in and near the area that deformed. In general, the sign of the residual stress will be opposite that of the force applied to cause the deformation- in other words, if a part deforms plastically in tension, it will be left with residual compressive stresses and vice versa.

If that part is subsequently loaded, these internal stresses will affect fatigue life and single-cycle strength, either positively or negatively depending on how the force vectors compare to each other.

With that stated, it does not appear that you are creating a beneficial stress in the root radius. Since that area deforms plastically under a compressive force during the crimp cycle, it is likely to have residual tensile stress on the surface of the root radius.

This is not necessarily cause for alarm- hundreds of objects rely on crimps to hold themselves together without problems.

Now, with that said.

As I said earlier, your results appear to me to indicate an artificially high level of stress in that area. Any time you have a stress plot where there is a huge jump in stress between adjacent nodes, you have an area that at least needs investigating to determine if the stress distribution is likely to be accurate. Before I did anything else, I would re-mesh without changing anything other than the mesh size, and re-run. Knock the mesh down, in a few steps, until it gets as small as you can go before processing time becomes a problem, and compare the results between runs. Ideally you will see that hot spot of stress distribute itself over a wider area, and the peak value will drop as well.

 

[XR250]

Wouldn't it be easier to just build one and test it? Your FEA results may not be that accurate due to the difficulty in taking into account the flexibility of the connection at the studs and possibly the deformation of the densglass.

 

[Ankit_Pandey]

Plot unidirectional stresses to check if its compression or tension.

 

[cal91]

In general, the sign of the residual stress will be opposite that of the force applied to cause the deformation- in other words, if a part deforms plastically in tension, it will be left with residual compressive stresses and vice versa.

I'm trying to understand this.

Say we have a rod and we pull both ends apart until it plastically deforms, and then we let go. Will there be compressive residual stresses?

I would think from an equilibrium standpoint that there is either no residual stresses, or that tensile and compressive stresses cancel each other out.