Min. angle for axisymmetric with bricks 1

[gfbotha]

Hallo

Using 3D tetrahedral elements, with what minimum wedge or sector (included) angle would you, generally speaking, still feel comfortable to analyse an axisymmetric problem? 15°? I realise it depends…, and might vary; but surely there must be some rule of thumb to generally deliver robust results (almost code-like).

I still very much prefer using proper axisymmetric elements (especially for non-linear) but most “designer” packages does not offer it, and at the same time computing capabilities also got better.

Thanks
Regards

 

[GBor]

Axisymmetric is 2D; Tets are 3D. I do not understand your question. Are you asking about the minimum included angle in a tetrahedral element for those software packages that do not offer 2D axisymmetric?

 

[gfbotha]

YES and NO; it is about how large a sector of the geometry you would model using 3D tets. Referring to the included angle of an element is relevant at a location on the symmetry axis (e.g. center of a dome closure), but when modelling say, a pipe, it is less relevant.

I guess when modelling a very narrow wedge there should theoretically be no real limitation but one could start running into numerical errors.

 

[johnhors]

As I understand it, you are using a FEA module embedded within a CAD system, which like most (if not all of them) will only analyse 3D models using tetrahderal elements, but your CAD part is adequately represented in analysis by axisymmetric elements.

Well, if available I would export your geometry to a full-time FEA system for analysis and use eight node quadrilateral axisymmetric elements.

Otherwise if you have only got the 3D mesh solution of the CAD system then it is imperative that you increase mesh density in areas of high stress until the problem converges (that is an increase in mesh density has little or no effect on results). You will always get some poor shaped tetrahedral elements with any mesher, but with a relatively fine mesh their effect on the average stress is minimal, so don't concern yourself too much with element quality if you have satisfied yourself that you have achieved a mesh convergence.

 

[gfbotha]

I agree, Johnhors, but am still interested in rule of thumb min. angle for an element on the axis, and then also for a geometry wedge some sitting on some radius.

Thanks for your comments.

 

[GBor]

I'm afraid I would say it depends on the boundary element availability within your CAD system. Typically, boundary conditions are limited in these CAD integrated FEA packages, so I would say you would have to revolve your axisymmetry until you reach another location where you can put reasonable boundary conditions (probably 90 degrees for a 1/4 symmetry model).

 

[gfbotha]

Sorry GBor, now I'm not with you: not talking/using boundary elements as such (classical 3D bricks). Also, not using closely integrated FE software - although it offers associativity.

I'm happy with the flexibility and properness of my available boundary conditions/restraints.

 

[johnhors]

Abaqus recommends a minimum of 10 degrees and prints a warning for elements with angles less than 45 degrees. But I think that these values are just plucked out of the air and carry no real weight on their own, since element quality is a combination of other factors (aspect ratio, skewness, curvature, jacobi ratio...). Just that elements with angles of less than 10 degrees are liable to be of poor quality. Furthermore if you go for 10 degrees then you will have relatively few elements on the axis for nodal averaging of the results, thus a 1/4 model as GBor suggests is probably better.

 

[johnhors]

What software are you using ?

GBor was referring to the boundary conditions available with a FEA module of a CAD product, which can be very limiting.

 

[GBor]

Well, I guess that's twice I misunderstood. I think johnhors points out the highlights, but the key would probably be in a detailed explanation of his "combination of factors".

 

[gfbotha]

No problem, GBor.

I was afraid this thread could easily get over-elaborated; that is why I have chosen my words carefully (from there my words like: generally, depends, robust, code, etc.). Knowing it depends on various factors I was simply hoping to get in some "good practice" estimates of the angle to be modelled. Thanks for your number, Johnhors.

We are using Cosmos DStar.

Regards

 

[corus]

The idea of 15 degrees minimum angle comes from modelling arcs where you have a variation of stress around the arc. In the case of quasi-axisymmetric in 3D, you have no variation of stress circumferentially so the only matter of concern is representing the arc on the inner and outer surfaces as an arc and not as a facetted structure. I'd keep the element size around the circumference the same relative size as the shape of the elements in the R-Z plane and use about a 10 degree segment.

corus

 

[45North]

I am probably way over my head here but will throw in my $0.02 anyways.

I would think that the basic limit would also depend on what sort of machine you are running it on. Machine Epsilon will limit how small of a number the software can deal with. If you divide Machine Epsilon by 2 the answer is ZERO. Same sort of thing with large numbers. Similarly most computational answers are approximations, but accuracy to 20 or 30 significant digits is generally close enough for most of us.

When you start generating very small numbers that are pushing the limits of Machine Epsilon most of the significant digits in your calculations are zeros. So if you get down to where only the last two digits are non-zero and you assume that the last digit is not rounded off you have a potential for about a 9% error.

As an example, using MS-Excel (32bit);
2.5E-308/2 = 0 rather than 1.25E-308
or
SIN(1/(4*10^307))= 2.5E-308
but
SIN(1/(5*10^307) = 0 rather than 2.0E-308

I'm certain that a true numerical math geek could explain it much more accurately but hopefully I didn't corrupt my explanation too badly.

It would be worth running a few test models just for giggles and see what you get. I suspect that a 32-bit machine will not do as well as a 64-bit unless the code truncates the data. I would bet you can get down to less than 1 deg before things start to get squirrley.

 

[johnhors]

One degree ! That's one helluva distorted element ! Most respectable companies have some form of FEA quality checking policy on top of any error and quality checking provided by the software vendor. I can't imagine that an element with a one degree angle would be acceptable. Since the OP wants to put tetrahedral elements right up to the axis, any results from such a distorted element would be unacceptable even if the solver and computer could handle what would be a severely ill-conditioned problem, caused by the fact that the surface normal restraints on either side of the one degree slice are almost parallel.

 

[gfbotha]

Yes, 45North, that is the kind of numerical processing errors I also thought about (including the accuracy of the CAD model), apart from the element quality issues.

For elements near the center line I tend to agree with Johnhors - 1° sounds a bit small - except if it involves a region of low stress & stress gradients where one might actually get away with it. Not sure about a 1° segment for elements sitting far away at/on some radius...(i.e. modelling a pipe or casing)

Don't have the time right now, but might try it out some day - would be interesting.

 

[johnhors]

Depending on the type of solver used the ill-conditioning induced by using a 1° element angle can "poison" the overall solution ! A solver like Abaqus would most likely abort the solution anyway.

 

[jte]

It seems to me that everyone focusing on a 1° arc is assuming that the axisymmetric component touches at the centerline.

We deal with this situation often in the world of pressure vessel evaluation for the process industries. Picture a vertical cylinder 20' (~7m) diameter x 3" thick shell say 30' tall. I have a conical transition (similar to a piping reducer) which has a 30° off vertical profile and transitions me to a 10' diameter shell. Let's say teh Inspection group has discovered a thin spot (due to corrosion) near the large diameter to cone transition and for simplicity I want to model it as though it is a full band extending 6" on the 20' diameter shell and 6" onto the cone. It has corroded down to 2" thick. As a first pass, I'm only going to include internal pressure. Its full of pressurized hydrocarbons and bad things would happen if it fails to contain the pressure. On the other hand, an immediate unplanned shutdown of the plant is not only costly but carries with it the not-insignificant hazards of taking the process through a shutdown and startup sequence. Keep in mind, BP Texas city

http://www.csb.gov/index.cfm?folder=completed_investigations&page=info&INV_ID=52

killed fifteen people during a startup in 2005. So, you, the analyst, get a call: Is is safe to keep operating until we can get to the next planned shutdown (or at least limp along for a month while we plan a quick one) or do we need to shut 'er down NOW? This type of scenario happens a lot more often than most folks realize.

We now enter the world of Fitness For Service, since we are well past the "new design" code limits.

http://www.memagazine.org/contents/current/features/healthcare/healthcare.html

I could go to my trusty old full blown FEA package and use true axisymmetric elements, or I could use my solid modeling package with the same FEA solver, but restricted to solid elements. If I choose (for whatever reasons) to go with the solid modeling package, I will build a profile of the geometry, which looks just like the axisymmetric model, and sweep it one degree for an inside arc length of about one inch. If I use more than one element through the 2" thickness, I can easily have well-conditioned tetrahedral elements. I apply internal pressure, fix the bottom section cut in the vertical direction, and apply the calculated longitudinal stress as a pressure along the top boundary on my small diameter section. I apply symmetrical boundary conditions on the edges of the slice. Within a few hours of the initial phone call I can have some feel for how dire the situation is, and at that point can either recommend an immediate shutdown or move on to a more detailed model incorporating a more realistic degraded area and additional loads.

Using 3D tetrahedral elements, with what minimum wedge or sector (included) angle would you, generally speaking, still feel comfortable to analyse an axisymmetric problem? 15°? I realise it depends..., and might vary; but surely there must be some rule of thumb to generally deliver robust results (almost code-like).

My perspective is that it depends. Perhaps one way to look at it would be to put at least enough of a swept arc to have several elements through the swept section. If the profile goes all the way to the centerline, then the concerns expressed in prior posts regarding sharp angles become applicable.

jt

 

[johnhors]

Putting aside the question of elements touching the centreline and just considering a 1° slice for the moment. The symmetry boundary conditions on the slice edges are almost parallel (as I stated in an earlier post). Then in the absence of any radial restraints (which shouldn't be necessary for an axisymmetric model whether 2D or 3D as here), this setup produces an almost singular stiffness matrix. Consequently the results are garbage (and that happens even before considering element quality or machine precision) !

15° is a sensible choice for the slice, which would yield both quality elements and a well conditioned stiffness model.

 

[cbrn]

Hi,
perhaps I got lost somewhere, but there is a foundamental thing I don't understand.
The OP's model comes from CAD, right? OK, but why not make a section (section, slice, however your CAD may call the intersection of the solid with a datum plane) of the revolution solid, in order to get a 2D axisymmetric surface? I sincerely can't see a CAD unable of doing that, and I don't see many FEA unable to deal with 2D-geometry...

OK, if you have non-axisymmetric loads / restraints then it may become a little harder since you need harmonic formulation, and only in that case I'd agree not going less than 10 - 15° span with a solid 3D sector in order not to have too close BCs on the sector's delimitation faces.

Regards

 

[gfbotha]

Cbrn, surely the CAD software will easily give one a segment (which we agree should generally be 10-15°). And, you are right; in that way one could also easily get the 2D profile to use if 2D axisymmetric elements are available. But, as I said in my OP, unfortunately the "designer version" of the FEA does not offer the 2D.

A previous version (4.5) of Cosmos DStar had it (2D)..., but they took it away (bad! - already requested to bring it back - guess it is about priorities). It is still available in the conventional but more cumbersome CosmosM.