How long should this take? 2

[trainguy]

Hi all.

Here's an open ended question, but I'd like to get a feel from the industry (you) about estimated level of effort.

Starting from a 3D step file of mostly thick plates (so solid meshing is an option), how many hours of FE analyst time would you allocate to the following:

Import geometry into FEA package
Mesh the geometry with 3D (tet) elements, using automated meshing. (assume approx 50 000 elements)
Apply straightforward boundary conditions.
Appply a single set of loads (say 4 loads over 4 small rectangular areas)
Perform a linear static analysis.
Prepare a few stress / deflection plots to be able to comment on the structural performance for this single load case, without doing any redesign.

The structure would consist of the first 10 feet of a locomotive underframe, which is essentially 2 heavy I beams side by side with structure between them which receives compressive load. The load case is not fatigue related.

How different would your estimate be for a mapped (non free) mesh of mostly Hex elements?

I realize the answers could vary wildly, but it would really help to know how you perceive this.

Thanks in advance.

tg

 

[OnlineFEASolver]

Assuming the geometry is clean and everything is merged
together, it should not take a decent analyst more than an
hour to prepare your powerpoint report. Of course if
geometry is complicated it is a whole different story...

Principal -

http://www.OnlineFEASolver.com

General FEA Consulting Services

 

[crisb]

My estimate would be somewhere between 1 and 3 days effort. Importing other peoples 3D files is often problematic as the requirements for FEA are usually different to those for general CAD. Mapped mesh using someone elses 3D model ...mmmmm!

Oh, and allow an hour or so for checking reviewing the results before you submit them.

 

[johnhors]

Import geometry into FEA package - 5 minutes or less

Mesh the geometry with 3D (tet) elements - 1 hour at most to get a reasonably good mesh

Apply straightforward boundary conditions - 5 minutes

Apply a single set of loads - 5 minutes

Perform a linear static analysis - 0 minutes of user effort !

Prepare a few stress / deflection plots - 1 hour


How different would your estimate be for a mapped (non free) mesh of mostly Hex elements? - almost impossible to answer without seeing the geometry ! Could be anything from 1 to 2 days to 1 to 2 months.

 

[corus]

Importing geometry into FEA package and finding out that the geometry won't import in that obscure format, there's an error in the dimensions, the geometry needs fixing - 2 days.

Meshing the geometry and finding out that there's a sliver in the geometry that won't heal, the parts don't match up and need to be tied or the geometry has to be redrawn - 2 days.

Applying loads and boundary conditions and finding out that nobody knows the loads and were hoping the computer would tell them, and where to put them, and then finding out you need to repartition the model for that area to be loaded - 2 days

Perform an analysis and finding out that you have too many elements and not enough disc space, and the system has just gone down - 1 day.

Preparing nice pictures and assessing the structure against design codes and finding out you need another 6 cases - 3 days.

I wouldn't have done it using tets in the first place, and it doesn't take more than an hour to partition it up for simple geometry.

Total realistic time 10 days, but call it 15 just to be safe.

corus

 

[GregLocock]

I'm with corus

Import geometry into FEA package

5 minutes to 8 hours, depending on the solid model.

Mesh the geometry with 3D (tet) elements, using automated meshing. (assume approx 50 000 elements)

1 hour to 8 hours, on my slow laptop. I often try it different ways, and basically hate meshing. Luckily I'm only interested in stiffness so if push comes to shove I can live with disgusting mesh quality.


Apply straightforward boundary conditions.

20 minutes, mostly just checking that it is doing what I expected. But I don't normally have straightforward meaningful boundary conditions


Appply a single set of loads (say 4 loads over 4 small rectangular areas)

20 minutes


Perform a linear static analysis.

5 minutes

Prepare a few stress / deflection plots to be able to comment on the structural performance for this single load case, without doing any redesign

4 hours to a week.

Seriously I'd expect to take a week on this to do it properly, but if it was something bodgy as a quick look for my own amusement, using a solid model that I have built, 4 hours. I think the Hypermesh tutorial that covers this would come in at less than 2 hours.

Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[cbrn]

Hi,
you speak about a locomotive underframe. As far as I know, most frequently these chassis are "ladder-type" frames, so mathematically it has "multiple auto-connectivity". This kind of situation can make most meshers (even extremely powerful meshers) bomb out. So be EXTREMELY careful in considering the time needed for this operation.
I would never consider less than 2 or 3 days for an analysis like this, executed with care and considering that presumibly you do it for the first time (my guess, but otherwise you would already have a precise idea about how long it can take).

Regards

 

[johnhors]

Cbrn - "multiple auto-connectivity" ? I cannot see any issue when auto-meshing with tetrahedral elements on any valid volume definition, no matter how complex the volume is.

 

[GregLocock]

Hmm, how about rivetted tubular cross members joining C channel main frames. Joint efficiency might be 50-60%, in torsion. No simple tet mesh will work for that.

Nice catch cbrn.



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[johnhors]

That's not a meshing issue. It may be an issue of how you decide to assemble the meshed components together.

 

[Kwan]

Don't forget to add time to validate the results. Deflection plots and such are fine, but this information is not enough to validate the model.

 

[rb1957]

so, how long is a piece of string ?

i work with riveted joints all the time. i just work with a standard model mesh (ie welded joints) then apply the forces and moments to the physical connection to shears and tension loads on the fasteners. sure its not exact (the joint isn't that rigid, so the load distribution is different, conservative and unconservative on different elements of the structure, but i thnk its near enough ...

 

[GregLocock]

Oh, for me it's just that joint efficiencies in ladder frames are a huge source of disappointment. In production even welded joints typically throw 30% of their potential stiffness away. (That's confirmed by physical tests)

Anyway, I think a rivetted joint is probably outside of trainguy's original scope.



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[SWComposites]

Time to finish an FE analysis is somewhat inversely proportional to how long you tell your manager it will take: if you are a realist (i.e., experienced) you might say it will take 2 weeks, but everything will come together easily (for once) and it will only take a day to finish. At which point you either find something else to do for 9 days without telling your manager, or you look silly for estimating 2 weeks. The next time you have a FE task your manager will expect it to be done in one day, but this time everything will go wrong (see posts above) and it will take three weeks of long overtime hours to straigten out the mess and get a result. In which case your manager will think you are incompetent or something.

Glad to see I'm not the only one who has experienced nightmares trying to mesh CAD geometry. One button meshing of solid geometry: ha!

So, trainguy, why did you ask the original question?



Steve

 

[gurmeet2003]

Just to increase the number of votes. I will say if structure is only plates, three days.

Gurmeet

 

[cbrn]

Johnhors,
I'm sorry to contradict you, but I already ran into this problem both with CosmosWorks v.2004 (back in 2004) and with ANSYS v.10 / v.11 (year 2007, and ANSYS is recognized to have good meshing controls...).
If you have a single volume with a very large number of voids (i.e. it has "islands", "multiple loops", "multiple auto-connectivities" or however you prefer calling it), and the solid space between the voids is at least one order of magnitude less than the magnitude of the voids themselves (it's what happens in a ladder-type frame when it is ALL-IN-ONE considered as a single solid, and NOT when the various beams are left independent and then joined together), then very likely the mesher will start at some location following its internal heuristics, then will propagate the mesh around the first void (pay attention to the fact it has two different paths to do that...), then around the second void coming from the first path and the second void coming from the second path, then it will have to fill the conjunction between the two voids... etc... etc.. and in the end, what do you think will happen? The mesher will not be able to resolve the contradiction coming from the fact that, in the same location, the elements coming from one path are not compatible with the ones coming from the others.

OK, the explanation is confused, I recognize, but believe me (or better try it) it happens!

Regards

 

[trainguy]

Everyone,

Thanks for the responses. I asked because my business partner nearly fell over when I suggested 2 - 3 wks.

I believe our quote went out at 1 week, but it's not a fixed price.

We'll see. Truth of the matter is, whenever I assume a single case, we end up doing at least 5-6 runs with modified load / boundary conditions in order to validate the hand calcs or toss them...

More often than not, the issue is the perceived stability of thin plates in the FEA versus actual buckling in real life & hand calcs. This may not be applicable to the thick plates in the loco.

Thanks again.

tg

 

[johnhors]

cbrn,

Thank you for your reply. Needless to say that I haven't used any of the softwares that you mention !

Yes, I can appreciate that this type of structure can be difficult when the target element size is too big. Setting a target element size which is too small can be equally problematic in that the model size in terms of nodes and elements can quickly become too big to handle.

But with appropriate local mesh size control there should not be a problem.

I'm afraid I find your description of the meshing process rather puzzling. As far as I am aware, there are three basic meshing schemes :-

1). Advancing Front.
2). Delauney.
3). Octree.

Of these the Octree is the most robust (it is very rare for it to fail to produce a mesh), but it's mesh quality is the poorest of the three. The advancing front is the least robust, but can produce the best quality mesh.

Of these three only the advancing front has any form of mesh propagation, but then it doesn't have to follow any kind of path through the structure, and almost certainly will not. Since it starts from a skin of shell elements it can choose any face of the skin (or front) for the base of the next tet element it is going to create. It is safer for the advancing front mesher to sort the front of faces by area and elect to start with the smallest one first. Of course the first and second in the list could be at opposite ends of the volume. Thus element numbering will appear to be randomly scattered through out the model. The mesher will do it's best to smoothly transition from small element sizes to some local or global target mesh size. I know of three commercially available tetrahedral meshers that use this face area sorting method. With correctly selected and applied global and local mesh sizes, these meshers will not find any problem with geometry features that vary by an order of magnitude. However, introduce features that differ in size by 100 to 1 or more, like a wafer thin panel connecting to a large solid block, then that geometry does get rather challenging (for any mesher!).


The Delauney mesher can fall over with this type of structure, but that is nearly always solved by reducing the target element size in local areas, just as you would with the advancing front method.


The Octree mesher by its very nature should in theory never fail ! Though I have seen it fail as used in Catia V4 and V5, but that was due more to poorly defined volumes.


As I said at the beginning I haven't used the softwares you mention, so I can't comment on them, but I've been using tet meshers since they first appeared on the scene and have never yet failed to mesh any geometry and I work on very complex 3D shapes, I'll admit they haven't all gone smoothly in the past (with poor Catia V4 models), and I've thrown some models back at the CAD jockey as not being worthy of an FE analysis, but that's all in the past. I would not expect any correctly constructed CAD model to present an insurmountable problem. Slivers as mentioned by other posters can be either removed by collapsing, sewing, healing etcetera or simply ignored by surface meshers which "jump" over them.

 

[cbrn]

Hi,
Johnhors, thank you for your detailed reply. I appreciate it.
I'm with you in saying that, with proper control, no mesh fails. But that's one point of concern for the O.P. Because if he manages to have an acceptable mesh with the automatic built-in routines of his program (and only a little bit of tuning on the element size), it's one thing; if he has to spend time to see where the mesher is encountering difficulties, it's another thing...

When I used CosmosWorks in 2004, it had extremely poor mesh controls (only local refinements of various types, but no possibility to control the algorythm logic). On the other side, Ansys has all the controls you mention (its default mesher is an Advancing Front, but an "alternate" can be used and as far as I know it's an Octree). Nevertheless, once I had to try a fast calculation on a portal for high-voltage electric line, I had been provided with the 3D model of it, all condensed in a solid (!) - in fact, it would have been far better to model it as a beam structure, having more than 200 beams interconnected!!! - and of course the meshers failed miserably. I didn't even try and spend the time needed to control the mesh properly over more than 200 locations: I re-built the structure using interconnected beams, directly in Ansys...

Regards

 

[meshparts]

Hello,

I found the last two posts of johnhors and cbrn very interesting.

I think both have right, but from different points of view.

From a mathematically point of view, it should be always possible to mesh any kind of geometry using one of the meshers commented by johnhors. If the geometry is clean...

From the user point of view there are some cases, like cbrn said, how are not clean or how can only be meshed with a very large number of elements. Which makes it practically impossible to mesh.

In my opinion, the CAD people should take training courses about how to design for FEM. I mean, it's really not too much asked, to avoid lines in the middle of an area... Where the line begins and end in the middle of the area and has no meaning, other then to make the meshing impossible.

Having a clean geometry from the start, can drastically improve the time for meshing that geometry.

Regards,
Alex