Determining level of geometric detail to be included in FEM 1

[krt222]

Hello,

First, let me state that I attempted to search for answers to this question throughout this website but did not find exactly what I was looking for. If I have missed this exact question and answers to it somewhere, please make me aware and direct me via a link.

So, my question is this: in the contecxt of large forged and cast steel and iron structures subject to highly variable, multi-directional loadings over a 20 plus year design life, what are some known procedures / guidelines for determining what, if any, geometric features (primarily micro geometry)of a native 3D model may be neglected (i.e. suppressed prior to FEM meshing) within finite element analyses for extreme (safety factor on local yielding) and high cycle fatigue (safety factor for SN based damage accumulation fraction) strength calculations? Specifically, I'm looking at bolt holes (not intending on modeling internal threads, bolts, stresses from bolt preload, etc. however) and clearance holes for studs, etc.

My intuition is to start with a model defeatured of all micro geometry and run some unit load cases (using known governing loads) to determine magnitude of macro peak stresses, then divide the max macro stresses by an assumed stress concentration factor plus an added buffer of safety (let's say combined 4x for a threaded bolt hole) and plot a gradient at that cut-off value and only include micro geometry which is greater than the cut-off.

I'd also like to expand the discussion to whether it's common practice in this type of analysis to include or somehow account for internal threads, bolts, stresses from bolt preload, etc.

Thanks in advance for your input,

- Kevin

 

[krt222]

Sorry I should make a clarification:

"...and plot a gradient at that cut-off value and only include micro geometry which are located in areas greater than the cut-off."

Also, I should have noted that it is my intention that the components in question be meshed with solid tetrahedral 10 noded elements and that I am using Femap/Nastran for my FEA software.

Thanks,

- Kevin

 

[flash3780]

I think that you have mostly answered your own question. The general approach would be to defeature your model enough such that you have a reasonable problem size, then sub-model or apply stress concentration factors to more highly stressed areas.

Ideally, you'd want to have a very fine mesh over your entire part, however we're limited by the capability of our computers, so defeaturing your model and submodeling is the next best thing. The problem is, it takes engineering judgment to identify areas that may have higher stresses in a defeatured model. Nobody's yet invented a black box that tells you a perfectly accurate stress distribution over a complex geometry. On the bright side, many software packages have made defeaturing and submodeling much easier.

On a side note, you mentioned that you're using 10-noded tetrahedral elements. If you're planning on submodeling, you may consider using a finer mesh of 8-node brick elements to increase the fidelity of the displacements on your cut planes. First order elements don't need quite as much uumph from the computer, so you should be able to pack more nodes into your model.

In regard to modeling threads, I don't know that it would be very worthwhile. There has been quite a lot of work done on analytical analysis of bolted joints. Take a look at "An Introduction to the Design and Behavior of Bolted Joints" by John Bickford. However, the bolt load distribution or analysis of flange "waffling" are a few things that are perhaps best studied with a finite element model (just be sure to preload your joint).

One more thing: you mentioned high cycle fatigue. If you're looking at multiaxial cyclic loading in a Goodman diagram things start to get a bit squirrely. Many people assign a sign to the von Mises stress based on the sign of the largest absolute principal stress. From there, you'll need to calculate the stress amplitude with the von Mises method (don't just pluck von Mises stresses from your solver).

 

[krt222]

flash,

Thanks for the input. I'll have to read up on submodeling as I've admitedly not done any to date. With as many relatively small fastener holes and small machining features as exist on the components I'm analyzing, the complexity of the macrogeometry and the fact that loading is very multi-directional (and many states of stress in the components are multiaxial through time) I struggle with applying stress concentration factors to anything other than a microgeometry defeatured, first cut model to draw areas on the component which directs my subsequent second, higher fidelity FEM pass which includes micro geometry in those areas that the first pass conservatively deems necessary. I.e., I do not want to apply an estimated, if even very conservative stress concentration factor to be taken as the end result in the critical areas for either my extreme loading safety on yielding calculation nor my fatigue life calculations as I believe doing so, in order to be conservative would probably end up being vastly over conservative in many instances.

What I'm working on now is actually brute forcing a test on my theorized process / logic whereby I go through the painful effort of meshing a completely featured, microgeometry and all untouched 3D model with sufficient mesh density at the microgeometry locations to see how my logic stands up for a given component.

I will consider alternate elements once I hone in on the critical areas and potentially embark upon any submodeling. My experience to date is primarily with the solid tet 10's so I'll have some learning to do there as well. I do understand the benefits from other element types I just lack the experience of working with them.

Regarding the even smaller microgeometries of thread profiles, etc. I really don't want to go to the extent of including them in my models but I was curious if there are any studies or general knowledge on how a threaded hole with a preloaded fastener installed compares on a stress concentration factor basis to just a hole (so effect of the internal thread geometry, fastener geometry and preload stresses). I've got Bickford sitting next to me but I'm only in Chapter 5.

With regards to fatigue I will be interfacing with a software program called DesignLife by nCode / HBM that will use the absolute max principle stress method or the critical plane method, depending on the extent of multi-axiaility it calculates (i.e. will not be using von mises 'stresses') as the basis for creating stress time histories by combining the stresses resulting from each of the load signals (that are aligned with each of the unit load cases stress) to be rain flow counted and then compared against a family of SN curves depending on the effective R value for each given cycle and summing the damage accumulation on a nodal basis per Miner's rule.

Thanks again,

- Kevin

 

[GregLocock]

You seem to be doing a wonderfully complex job on the FEM side while ignoring the vast gaping problems with fatigue analysis and load measurement. On cars we run fatigue analysis using measured loads with about a 1mm element size, including some fancy pants stuff on spotwelds which are obviously of great interest to us.

BUT the loads used are measured, yet vary by 30% from run to run, which is what, a factor of 8 on life?



Cheers

Greg Locock

I rarely exceed 1.79 x 10^12 furlongs per fortnight

 

[krt222]

Greg,

My question was not geared towards accuracy of the loads or the fatigue calculation methodology but rather what level of geometric detail need be included in my finite element model. I'm given the loads for my analyses and I do accomplish various sanity checks on them to ensure processing errors or otherwise are not glaringly apparent - but it's not my primary responsibility to ensure their accuracy (different persons on our team handle that). Furthermore, the fatigue calculation methodology is a requirement for a 3rd party certification and I've not found a more appropriate method for our application to date so I stick with it for now.

Regardless, the analysis I'm embarking on, with regard to fatigue, will be utilizing time series fatigue load signals as estimated by another team using some very sophisticated multi-body dynamics software tools by MSC. These estimated loads are certified by a 3rd party through parallel calculations using a different software tool from another company as well as through empirical field testing. While the loads are certianly not 100% accurate, I have a pretty large degree in confidence in their being conservative as we place a 1.265 load scale factor on top of every time series.

Also, the basis for the damage accumulation fatigue calculations per German FKM methodology combined with another German methodology (which I will not attempt to spell) will be a family of R value synthetic SN curves which are generated conservatively based on standard EN material specifications using 95% survival probability knockdowns and material defect / quality inspection knockdowns, etc. Again, the material SN curves are certainly not 100% ccurate but I have high confidence that they are conservative.

Thanks,

- Kevin

 

[ColonelSanders83]

In my humble opinion, you will need a different model for fatigue analysis. The details removed for the global stresses are all important for proper fatigue analysis in highly stress local components with complex detailed local geometry.

In my past life, local and global stresses were analyzed with separate models. I should state I worked on submarines at the time.

A global model was built using plate and shell elements to accurately calculate global stresses and displacements. These models would generally contain features no smaller than 5% of the size of the structural components in question for global values. Fatigue assessment of the overall structure (sometimes of plates 4 inches thick) and forgings (up to 20 tones in weight) was evaluated in areas of structural importance.

Detailed break out models were built for all areas of local discontinuities using the imposed displacements (strain) from the global model. Detailed fatigue assessments would then be performed on individual components based on accurate local models with very good mesh refinement and accurately imposed boundary conditions.

Just my two cents worth.


A question properly stated is a problem half solved.

Always remember, free advice is worth exactly what you pay for it!

 

[flash3780]

^Agreed. I reread my original post and I didn't realize that I wasn't very clear. I would recommend defeaturing and submodeling all stress concentrations unless it is obvious that they are not in any sort of load path. You can find an example of this sort of approach at this link.