One tiny area with high stress 1

[Barnon]

I'm no expert in FEA. But I'm trying to analyze a weldment by just uniting all the solids into one. I'm using NX design simulation. Everything looks good except for where the thin blade corner meets the tubing. Can I assume this isn't a problem? Also my Nodal stresses are much higher in that same area. Like double, but again the rest of the model looks good.
s

 

[FEA way]

This is called stress concentration in FEA. Some are physical but some are artificial. There are several approaches to solve this issue. First check stresses in other areas, see if they look correct. Also take a very close look at the area with concentration, notice how many elements have this increased stress. And what's most important try to understand why it appeared there (examine boundary conditions, loads, contacts and so on). Refine mesh in this area, perform nonlinear analysis and see if this helps. Maybe you will have to change the geometry a bit (make this corner less sharp). You could even use shape optimization (if your solver allows it) to eliminate this concentration. However it is better to do it manually.

 

[karachun]

Look like singularity. In static linear analysis, an infinite stress will be mathematically true solution, stress will increase after mesh refinement. It`s feature of FEA math, just deal with it.

https://www.youtube.com/watch?v=ZP9nh4GOkIc

https://www.comsol.com/blogs/singularities-in-finite-element-models-dealing-with-red-spots/

http://feaforall.com/what-causes-a-singularity/

 

[Barnon]

Thanks for the responses. I'm also looking at a few more design options. I'll post my results.

 

[rb1957]

this is a linear run ? so in reality you'd get a small localised yielding and everything would be fine.

maybe you can do some analysis to back out the true plastic stress based on the elastic stress (Neuber ?) ?

another day in paradise, or is paradise one day closer ?

 

[rickfischer51]

Dont include that stress in your weld calculation. The stress is occurring at a modeling feature that wont look anything like that after the parts are welded together. The weld allowables are knocked down to account for sharp corners, slag inclusions, etc.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[glass99]

My assumption with small stress concentrations is that they are fine because of the ductility of the metal, unless you are looking at fatigue. They go away completely when you do a NL material solve.

 

[jax217]

Agree with rickfischer51. I would exclude [at least] the elements immediately surrounding the artificially high stress when performing the Von Mises check of the weldment. I might tack on a weld efficiency factor for this check as well depending on the material (we use 0.85). As for checking your welds, rick is right in that your end geometry won't look anything like that (I assume it's a fillet-fillet weld), and that typical weld analysis methods and knockdowns account for this. I might even take a freebody of the cross-section where the blade meets the tubing and do a hand calc (Shigley and Roarke have good examples of this).

 

[rb1957]

"I'm trying to analyze a weldment by just uniting all the solids into one" … this is probably a "bad" way to model this feature, if you're going to pull this type of detail from it. The better way to model is as discrete pieces with the weld modelled (CBUSH?).

another day in paradise, or is paradise one day closer ?

 

[ESPcomposites]

The FEA will do what you ask of it, but you have to interpret it properly.

1. Let’s first consider a linear static analysis.

1a. If the stress concentration is finite (i.e. a plate with a hole), the FEA will be able to determine the magnitude of the stress concentration (once convergence is achieved).

1b. If the stress concentration is theoretically infinite (a sharp internal feature or crack), the stress will continue to increase upon mesh refinement (will not converge because the stress is theoretically infinite). This is what a classical solution would predict so the FEM is doing what you should expect it to.

Note: Item 1 is where some people call stress concentrations in FEA “artificial”, but that is not really the case. The FEA actually does what it should, but it’s up to the engineer to address the following items properly. So let’s have a closer look.

2. The next question is how to address the stress concentration. Let’s first consider the static ultimate load case for when the stress concentration is finite. There are two options.

2a. This can be addressed via FEM with a nonlinear analysis (material nonlinearity), but you will also need to know the stress-strain curve of the material *and* have an adequate failure criterion. Note that for composites, a failure criterion to address this scenario does not exist (with the possible exception of a not well-accepted micromechanics criteria). More times than not, we usually go to item 2b.

2b. Rather than using the FEM to solve the problem directly, we can break this into two options (materials that are notch sensitive versus materials that are notch insensitive). If the material is notch insensitive (i.e. ductile), we can ignore the stress concentration (close approximation to the real solution), provided the volume of material in high stress region is relatively small (if there is large volume of material in the region of the stress concentration, this assumption is less valid). We can also use hand calculations and the stress concentration (strain concentration) to get a more accurate result. If the material is notch sensitive (brittle metals, composites, ceramics, etc.), the stress concentration will affect the static ultimate capability and must be considered. For truly brittle materials, this is rather direct (proportionality applies). However, composites are “pseudo-plastic” or “quasi-brittle” and you can’t treat them as either brittle or ductile (at least not in an accurate manner). You will need a different approach for that.

3. Now consider the static ultimate load case for when the stress concentration is theoretically infinite. This is actually a fracture mechanics problem and not a true stress analysis. And you can’t expect a FEA stress analysis to solve a fracture mechanics problem. That said, there are some similarities as discussed in item 2 and some approximations you can make, but be aware of this distinction.

Note: For some problems/industries, there are semi-empirical factors that can be used to correlate the results from the FEA to useful data. But that requires additional testing and is often used when “pure” analytical solutions do not effectively capture the behavior (i.e. test data is used to compensate for analytical shortcomings). Some examples include welds and composite structures.

4. Finally, we should also consider fatigue analysis. If the material is a ductile metal, the stress concentration will affect the fatigue life, so we can’t ignore it this time. If it is finite, you may start with solution to determine the life to develop a crack (i.e. something like Miner’s rule). If it is infinite, you may start directly with LEFM.


Brian

http://www.structuralfea.com

 

[L_K]

In industry the most common methods to analyze the fatigue of welds are nominal, hot spot, and effective notch stress methods. These all deal
with the singularities differently.

https://caeai.com/blog/how-predict-fatigue-life-welded-structures

 

[glass99]

The bottom line for me is that linear static FEA of metal components are useless as a practical matter if I'm looking to calculate strength. Its too much judgement to say how big of an area can be overstressed. Ok if its a tiny area then fine, but then I could have just used a conservative hand calc in a fraction of the time.

The only practical solution from my perspective is to do a non-linear material, and keep factoring up the load until the deflection gets too much. You then back off whatever factor of safety you want from a force-displacement plot.

 

[ESPcomposites]

There are still some practical uses. First, we can break this down into two categories:

1. Notch sensitive metals (brittle). FEA is a great tool for determining finite stress concentrations. And these stress concentrations can be directly used for a notch sensitive material when determining the ultimate load capability.

2. Notch insensitive metals (ductile). We can break this into two categories.

2a. First, consider the case where there is a “large” volume of material in the highly stressed region. In this event, if we wanted useful information from the FEA, we would probably need to use a nonlinear analysis (material) to determine the ultimate load capability. But just knowing the stress concentration itself *may* be useful if you are combining it with hand calculations (depends on the problem).

2b. Next, if the volume of material in the highly stressed region is “low”, we can probably ignore it. The use of the FEA would be that we can address geometry, boundary conditions, loading, etc. that may not be well suited to classical solutions (i.e. hand calculations are not sufficient). We could perform optimization and assess the areas away from the stress concentrations. We may not know ahead of time where the higher stressed regions are (since this problem is not well suited to classical solutions by definition), so the FEA can provide insight about that and guide you during optimization.

Note: It may take some experience to know if the part falls into either 2a or 2b. Depending on your part/industry, this may be obvious, but sometimes it is not. Short of that, a nonlinear analysis may shed light on this. If you perform this once and turns out to fall into category 2b, then there are uses via subsequent uses with simpler linear solutions (i.e. could address various load cases, boundary conditions, etc).


Brian

http://www.espcomposites.com

 

[glass99]

Of course FEA for brittle materials makes much more sense - we do a lot of structural glass, so we really want to know about the max principle stress at the absolute peak.

Smoothing out stress concentrations in a steel component through optimization is interesting, but would possibly lead to needing 5 axis CNC milling or something.

This stuff also depends on your bureaucratic situation. Judgement about hotspots is subjective - if I make an engineering report and it gets reviewed by someone unsympathetic to my cause, like say a lawyer in the event of a failure, it can be hard to defend. Linear FEA of ductile materials in my experience leads to really conservative design for this reason.

 

[ESPcomposites]

Sorry I was not clear. I did not mean to smooth out the stress concentration (though that is possible). Rather, I meant disregarding it and optimizing the rest of the part based on the acreage stresses that exist.

Judgement is an issue, which is where the note above comes into play. It will depend on how "clear" the problem is and also the certifying authority. When it is not clear or you have a strict requirement, you might be able to run a nonlinear analysis to demonstrate the Kt does not have a global influence (or does). If there is no perceived influence, you can then perform a linear analysis for various load cases, optimization, etc. based on this assumption (to simplify and expedite the process). And at the end, if necessary, you could run a nonlinear analysis for the critical case(s). By going through this process, you may also be able to demonstrate the lack of need for a nonlinear analysis for future design variations or like parts (or least minimize the future burden).

Again, this is all assuming it is not clear. If it is clear to you and the authority, then you can bypass the nonlinear analysis. If it is clear to you, but not the authority, you might be able to run a nonlinear analysis for the critical case on the back end to appease them. So there are a few ways to work with this.

Side note: For composites, the approach can be direct if you have notched allowables. For this case, you only care about the acreage strains (remote strains away from the stress/strain concentrations) and directly compare those to the notched allowables for the given notch.

Brian

http://www.espcomposites.com

 

[glass99]

The other key skill with using NL material properties is being economical with your mesh. The mesh in the OP's question has way too many nodes, meaning that NL material would take forever to run and be really impractical. If you can keep things less than 10,000 nodes for a part like the one shown, you can iterate quickly even with NL material model. I find that I need to run models a dozen or more times before I get them right with all the boundary conditions and connections etc.