1st order versus 2nd order tetrahedral elements 4

[feajob]

Hi,
I usually deal with 3d complex geometries and I use tet10 (2nd order solid elements) for static analysis. My models are very big (talking about 800,000 nodes). We have good hard-wares and I get my results in les than 1 hour. But, now, I have to do some contact analysis. Since, 2nd order elements are not suggested for contact analysis and my models are big. I have converted my 2nd order elements to 1st order elements. In this way, for the same number of elements, I have 6 times less DOFs in my model.
I do contact analysis in an efficient way, but, as you know, tet4 is stiffer than tet10. So, I am worry about the quality of my results. I found this paper:

http://www.mscsoftware.com/support/library/conf/auc99/p04299.pdf

It confirms my anxiety. At this point, I don’t know, what should be sacrificed? Accuracy or efficiency? I am thinking about a mix model. Only 1st order elements in contact area and 2nd order elements elsewhere, but, it won’t be efficient (solving iteratively big models!). Please let me know your suggestions.

Regards,
AAY

 

[johnhors]

AAY

Firstly, Abaqus have a specially formulated tet10 element that allows contact (C3D10M)

Secondly, experienced Abaqus users won't touch this element with a barge pole! It's stress recovery is very inaccurate (Abaqus at first denied there was a problem to me, until the very next slide on their ppt display said they were working on the problem!).

Thirdly, experienced Abaqus users (at least three seperate consultants/companies) use mixed meshing, 8 noded bricks for the contact and 10 noded bricks elsewhere. They connect 4 bricks to 2 tet10 elements, thus ensuring continuity of displacement across the join, and living with the dis-continuity in stress.

Your model using 2nd order elements does strike me as too large to be solved iteratively. Why don't you produce and solve a coarser mesh, which will still provide accurate displacements and hence loading paths, then use the results from this "coarse" model to be fed into fine meshed sub-models as boundary conditions?

 

[corus]

You would do better by spending a little more time on the model geometry and use linear brick elements. Linear tetrahedral elements are of no use what so ever and as johnhors said, quadrilateral tet elements give odd results when used in contact. Sub-modelling is fairly easy in Abaqus and would be one way of mixing quadrialteral tet elements in the global model to linear brick elements in the sub-model, although problems can arise if the driving nodes aren't chosen sufficiently far enough away from the area of interest. If you can't easily do sub-modelling in the software you have then simplify your geometry and use brick elements everywhere. This is a far better option for improving efficiency for little loss in accuracy at the area you are interested in.

corus

 

[feajob]

Johnhors, connecting 4 bricks to 2 tet10 elements is a great idea. I can do that easily.
Corus, using brick elements for a landing gear structure is not an easy task. We can do that, but, it takes too much time and my boss won't be happy.
Johnhors, Corus, I am not using Abaqus. I am using MSC products (Nastran, Marc). Well, I never did submodeling in these softwares, I can try this idea. I think that it would be equivalent of finding the interface nodal forces(on a small portion of my model, where contact happens) with Nastran in a linear analysis and applying them on the interface nodes of my small model for non-linear analysis with Marc. Please correct me, if I am wrong.

AAY

http://www.geocities.com/fea_tek/asd/

 

[johnhors]

AAY

Yes you are quite right on the necessity to use tet elements for meshing of the complex parts of a landing gear.

My procedure for sub-modelling is the reverse of what said!
I run a coarse mesh of the assembly with full contact, which I know will not produce good stress results, it will however produce good displacements which I can use in a sub-model.

When I sub-model, I first sub-divide a complex part into several or many connected volumes (sharing common boundary faces). I make planar cuts through the volume around areas of concern. I then have nice convenient flat boundaries available for sub-modelling these regions. From the analysis of the complete coarse mesh which can be a non-linear contact problem, I obtain the nodal displacements on these previously defined planar cut faces and apply these as enforced displacements on the boundaries of the sub-model.

The technique is very easy to do using any FE system. Checking is a breeze, just run the sub-model without enhancing the mesh and you should get identical results to the whole model, you can then safely refine the mesh of the sub-model to obtain a converged stress.

 

[corus]

Using nodal forces or nodal displacements from the global model to the sub-model would be equivalent. The problem is in interpolating results from the global model to the refined mesh of the sub-model. If you're doing this by hand then this will be difficult. If your software can do this for you then the interpolated results will be based on a linear interpolation between nodes. This leads to errors on the partitioned faces of the sub-model and as such it is wise to take a sufficiently remote plane away from the area of interest as the interpolation region. Any errors that will occur at interpolated values should then have little effect on the results at the area of interest.

With reference to brick meshing, I'd tell the manager that if he wants the job doing properly then he'll have to wait. If he wants a pretty picture of no real value then just use a coarse tet mesh for your analysis, and look for another place of work where they do things properly.

corus

 

[feajob]

Corus, I am agree with you regarding the interpolating problems with tet10. It is obvious to me brick elements are much better than tet elements. However, I believe that the most important thing is FEA is this "By refining a mesh no matter which element (brick or tet10) you are using, you will be closer to the real solution. Convergence will happen always by refining a mesh. But, the rate of convergence is different." For brick elements this convergence rate is higher than tet mesh. Please correct me, if I am wrong.

On the other hand, our models are very complex. Using brick elements, is a very time consuming task. I don't know how we can justify that? We can refine more our tet10 mesh , or use brick elements at some places with tet10 mesh (as johnhors suggested) and get the good solution.

 

[Drej]

feajob

I may have the wrong end of the stick here but be careful about generalising your assumptions on tet elements. First order tets are useless in anything but pure thermal analyses, however second order tets are very good for modelling complicated geometry and for use in structural problems AS LONG AS YOU UNDERSTAND THEIR LIMITATIONS. It sounds as though your geometry wil probably have to use these according to your description - this is not a problem. If you need to mesh a structure in which the stresses/response is dominated by bending consider that second order tets are quite stiff (1st order tets are useless in this respect). You will need to use about two/three tets through thickness for adequate resolution of stress results, more if your analysis includes non-linear material props. For displacement resolution only you may require less through thickness. If your problem is dominated by planar loads (membrane stresses as in in-plane bending for example) you could get away with less than three. Whatever, don't be afraid to use tet elements for contact problems. Most CAD geometries we import can only be tet meshed in most cases. We could get mapped or hex-dominant meshes, but because of the time taken to produce this offsets the benefit of a hex mesh. Once meshed wth tets, these components are used to carry out complex contact problems. The key is knowing how to mesh your component(s), knowing the limitations of your elements and knowing exactly how to tweek the contact to obtain best results.

Cheers,

-- drej --

 

[johnhors]

AAY

Again your comments are sound. With regard to brick or tet10 element usage, neither will converge to a "correct" solution, just that bricks will converge to solution that is more "correct" than tets and with far fewer elements on a "simplistic" test model. I said "simplistic" because there is no meshing software in this world that could mesh a fully detailed landing gear leg with reasonably shaped brick elements in "reasonable" numbers.

The last time I used brick elements on a landing gear leg (in days before tet meshers) was using a dumb Tektronix terminal on a VAX/VMS mainframe. I built geometry from scratch (no CAD import available, in fact no 3D solid existed). I ignored all small details (chamfers, fillets, grease holes... etcetera). The volume had to consist of thousands of simple shaped map-meshable regions i.e. bricks or wedges. A drawing refresh when a lot of lines were being displayed would give you long enough to take a coffee break (OpenGL was a distant dream). How long did I take to complete the model? Answer, a whole year!!!!

I'm sure with the improved software and hardware, the time would now be considerably less, but probably at least 2 months, BUT that is still ignoring all the small details! Such a model would only be good enough for ultimate strength analysis and completely useless for fatigue analysis.

Using tet elements (in large numbers) is the only practicable solution for meshing very complex structures.

 

[feajob]

Drej, I am agree with you on all of your statements. May may, I was not clear in my previous message. I would like just to add that I don't use tet4 (linear tet mesh) for a detailed stress analysis, I was talking only about tet10 (quadratic tet mesh).
Johnhors, thank you for your comments. It is an interesting approach. Since, the convergence rate of displacement fields are higher than those of stress fields. You assume that displacement fields obtained from a coarse mesh is good enough to be applied on a small portion of your mesh (sub-model) with a very fine mesh. I guess that the number nodes on the common boundary faces must be the same? So, you refine your sub-model without touching the boundary nodes on common faces. Now, I would like to have a rough idea about the following ratio for your sub-model:
(DOFs of your final fine mesh) / (DOFs of your initial coarse mesh) = ?

Thank you,
AAY

 

[corus]

The days of taking a year to produce a model are long gone, thankfully, and I would think that using tet meshing to model every single little pimple in the overall model would be a waste of computing power, if you were to use recommended mesh sizes. Finite element modelling is a compromise between cost and accuracy. You can throw your automatic meshes at some imported geometry and find that you have either quickly ran out of space on your compute or the analysis is taking days to complete. Alternatively you can decide early which features need accurate modelling and which features can be ignored as having only a minor localised effect and not worth considering. This will reduce the cost of developing the model and reduce the cost of analysing it for little effect on the accuracy.

On a second point, quadrialteral elements have a problem with the mid-side nodes in contact which can cause problems in convergence and produce odd results at the mid-point positions. As tet elements can only be used in their quadrilateral form I find it is better to use linear elements where ever possible in contact problems. Even though it means spending a little time on reviewing the details needed to be modelled, on the mesh quality, and a little time on deciding on what is to be obtained from the model.

corus

 

[johnhors]

AAY

Yes you are right again, the mesh density on the common boundary faces remains the same (I mesh these with a density greater than that used in the rest of the coarse model - a kind of half way house between coarse and fine meshing).

As for DOF's, this is determined by hardware resources, on the machines I use, any model below 400,000 nodes will run with ease, the largest I have run is 440,000 nodes using either Lusas or Abaqus. So the coarse mesh of the whole component is usually about at the max capability i.e. 1.2 to 1.5 million DOF's. Sub-models after refinement approach the same size. So the ratio that you want is the ratio of the volume of the whole model to the sub-model, this can be anything between 10 to 500.

 

[johnhors]

Corus

I'm afraid that omitting any geometric features is politically unacceptable! If I do remove a grease hole I would have to justify my action. How do you do that? Answer - run the complete geometry model intact! Sub-modelling is the only feasible way to produce models good enough for fatigue analysis that include all possible stress raisers.

 

[corus]

For a hole within a structure that can be judged to have no effect on the overall stiffness then if you model the structure without the hole then look at the nominal stresses at the hole position. Use a stress concentration factor on the nominal stress from Roark's formulae to make an assessment of the peak stress at the hole position. In my view that method would be more accurate than modelling a hole with only a few elements around the circumference, as I've often seen. You can make an initial assessment of the stress there by either doing a simple assessment with hand calculations or intuitively arguing that the stress at a certain hole position must be less than another hole position and can therefore be excluded from the overall model and fatigue assessment.

corus

 

[johnhors]

Corus

Where I work the Catia model is sacrosanct. The model that I use for analysis is the same one used by manufacturing. There is only one current model allowed per component for auditing purposes. I fought and lost the battle to make allowances for engineering judgement some years back. This is now the common (enforced) practice in aerospace as a whole. Using engineering judgement to omit geometric features for an analysis would be viewed upon in a very dim light by litigation lawyers, if the occasion arose (and it does!). You simply have no choice but to mesh Catia solid models as-is.

 

[corus]

Fair point johnhors, but the engineering judgement I was implying is based upon logic in that if you have a bending stress in a beam, for example, then it can be reasoned that a hole at the outer surface will have a higher stress than a hole in the middle, based upon nominal stresses. As such there's not much point in modelling the centre hole if you're looking at fatigue damage at a hole. In addition, my experience is that CAD imported geometry is more trouble than it's worth (due to drawing errors) and that the purpose of a CAD drawing is different from that of a finite element model.

It's probably fairer to assume that lawyers are unable to reason and ensure that you have plenty of space on your machine for the massive models that must occur. It makes you wonder how the Wright brothers managed without computers.

corus

 

[feajob]

I would like to thank everyone for their responses. It was a very helpful discussion for me.

AAY

http://www.geocities.com/fea_tek/asd/

 

[izax1]

AAY

I know this might be a little late, but in MSC/PATRAN Fields you can easily convert (interpolate) displacement fileds from a global to a local model


See:

http://support.mscsoftware.com/kb/results_kb.cfm?S_ID=1298&requestTimeout=2000

Good luck

 

[feajob]

izax1, thank you for your response. I am going to read this document.

AAY