Linear Bricks vs. Quadratic Tetrahedrals 4

[MMATguy]

Hello,

I think analysts in industry tend to shy away from using quadratic tetrahedrals and advocate meshing the whole model with bricks even if it takes 2+ weeks. As far as accuracy goes Comparing the shape functions, quadratic tetrahedral elements are just as (or more) accurate as a linear brick element. I understand that computation time is a concern, but I believe the extra time spent brick meshing the whole model would be better served doing the analysis and debugging. Some people also advocate doing a hybrid (brick and tetrahedral model, but I'm not so sure that doing this is a good idea because it could cause discontinuities in the nodal solutions (due to discontinuities in the shape functions).

What are the feelings of other people on this board concerning this subject?

Regards

MMATguy

 

[ProbaSci]

I use linear and parabolic tets almost exclusively and have had very good results. I also have a strict Validation and Verification protocol which typically consumes more time than meshing / analyzing / debugging. My models do tend to be simplistic

http://www.probasci.com

-
Implantable FEA for medical device manufacturers

 

[fkmeyers]

A tet10 mesh is typically very accurate. The problem is that tet4 elements have given the tet family a bad name. We have done lots of comparisons which clearly show tet10 elements are very accurate in stiffness and also accurate in stress when corner stress output is requested. Bricks have their place but their advantage is they are not parabolic so that means no midside nodes which means a smaller model in terms of DOF. But the newer solvers like PCGLSS seem to handle models with lots of tet10 elements as good as with lots of tet4 elements.

 

[GBor]

A Star for you, Frank!

tet4's have given a bad name to the tet family, but it is also the application of those tets. Too many analysts let their automesher put tet4 elements a single layer through the thickness of their solid model and fail to understand the impact of the results. Of course, the same analysts stick one brick through the thickness and present their "pretty picture" to management...nevermind. I feel myself climbing on my "soapbox"!

 

[fkmeyers]

See the other thread on the CTRIA3 elements. It is a similar story with regards to CTRIAR and CTRIA6 which are decent elements.

 

[Drej]

> Bricks have their place but their advantage is they are not parabolic so that means no midside nodes which means a smaller model in terms of DOF.

Not all 'bricks' are first order.

> Too many analysts let their automesher put tet4 elements a single layer through the thickness of their solid model and fail to understand the impact of the results. Of course, the same analysts stick one brick through the thickness and present their "pretty picture" to management...nevermind.

A single tet4 is not always inappropriate - modelling simple thermal loads, for example, using these elements can be perfectly reasonable. For stress modelling the use of these in regions where stress results are important these elements have limited use, as they are way too stiff. As for the single brick through the thickness, this is also perfectly acceptable in some instances, given that the element isn't subject to large stress gradients. But even when stress gradients are present, a higher order brick will often capture the response adequately.

Every element has its appropriate place in FE. It all depends on the loading and the geometry. Amen.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[GBor]

Drej,

I'll concede the thermal element single brick application and agree that not all bricks are linear, but a single, linear brick through the thickness even in areas not expected to have a high stress gradient isn't advisable. I suppose it could be justified it extremely large models where you are really struggling to keep the run time reasonable, but there would always be the "what if". You also have the questions of when and how to transition.

 

[Drej]

> ...but a single, linear brick through the thickness even in areas not expected to have a high stress gradient isn't advisable.

Don't agree. So a single linear brick in a regular plate under say simple tension (no gradient per se) wouldn't give a reasonable approximation of the stress? You need to consider the type of loading the element is under and not generalise. I've carried out studies with single bricks through thickness under bending load and found the results to be reasonable (not exact, but reasonable); of course, these are higher order bricks. As I say, though, under gradients I wouldn't advise single bricks through thickness. Two through thickness under bending gives a good correlation.




------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[GBor]

I didn't say it "couldn't" or even that it "wouldn't", just that it isn't advisable. My original statement was:

Too many analysts let their automesher put tet4 elements a single layer through the thickness of their solid model and fail to understand the impact of the results

(emphasis added)

My soapbox is now, and has always been, that many "analysts" fail to do the work that it appears that you have done with regards to testing their element types. I don't like generalizations, but that includes the implication that single bricks through a thickness is OK.

Other than this, we'll have to agree to disagree, I suppose. I'll leave it to you to close the thread as you see fit.

 

[gio1]

Brick elements yield better stress results in contact analyses

 

[MMATguy]

"Brick elements yield better stress results in contact analyses"

Why is that? I would think that two coincident and lined up (node for node) tet10 meshes would model contact well.

 

[Drej]

> Brick elements yield better stress results in contact analyses

This falls into the category of sweeping generalisations methinks. Would be interested to know why you think this is so.

> I would think that two coincident and lined up (node for node) tet10 meshes would model contact well.

Contact in spatial 3D elements (such as bricks, tets and planar elements) is actually modelled using the gauss points of the element(s) - not the nodes. But yes, a well 'matched' mesh (of any element type) usually provides good modelling contact conditions in general, although there are many, many other factors that come into play here, most of which are off topic for this thread.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[gio1]

I have never come across a program that uses gauss points to model contact. If you know of one please let me know.

As far as I know there are 3 kinds of contact algorithm:

1- node to node contact
2- node to surface contact
3- surface to surface contact

In the first case the boundaries of both contacting surfaces are defined by their respective nodes. This is not completely accurate as some relative penetration is likely to occur.

The second case is often referred to as the “master-slave” approach, as the assumption is that the “slave” surface, defined by nodes, cannot penetrate the “master” surface, defined by element faces (or segments in 2D case). However, edges of the master surface may still penetrate gaps between nodes of the slave side.

The third algorithm is the most accurate. Here master and slave surfaces are iteratively swapped and effectively prevent any relative penetration. It is also the most computational intensive.

The formulation of second order tetrahedrons (the only tetrahedrons relevant for stress analyses) as well as second order wedges and membrane shells suffer from a problem that makes them not entirely suitable for contact analyses:

The direction of nodal forces developing as a reaction to a uniform face pressure is not consistent for all nodes: mid-side nodes will develop a force whose direction is opposite to that of corner nodes.

Not only this will make convergence more difficult, but assuming that it is reached, the resulting prediction of contact pressure will be wrong.

ABAQUS have developed a special modified tetrahedron to overcome this problem, but in my experience it still does not yield results as good as in the case of hexahedral elements.

 

[johnhors]

Gio1 is quite correct. I know several very experienced Abaqus users who all shun the C3D10M element for contact problems, and use 8 node bricks instead (for the contact) and would rather suffer the incompatibility induced when merging a ten node tet mesh (using normal C3D10 elements) directly onto the 8 node brick elements. In my experience the modified tet element can over cook peak stress values by 10 to 15 percent. Abaqus are aware of this problem and have been working to improve the performance of this element.

 

[Drej]

> I have never come across a program that uses gauss points to model contact. If you know of one please let me know.

ANSYS. Perhaps you've heard of it?

For surface to surface contact -- by far the most commmon type of contact used -- we populate the contact surface with gauss points, which are then used to transmit pressures. Hence: (1) the gauss points are used to model contact and (2) the reason for my statement on the types of element that are used for this contact (see above). All of the other types transmit forces at the nodes.

> The formulation of second order tetrahedrons (the only tetrahedrons relevant for stress analyses) as well as second order wedges and membrane shells suffer from a problem that makes them not entirely suitable for contact analyses

This appears to be a problem unique to ABAQUS (in fact, I've heard ABAQUS users talk of this problem before), as ANSYS does not suffer from such problems, so be careful not to generalise (see above). Tets or bricks in ANSYS are both excellent and can be used as and when necessary in contact analyses -- if anything, the tets are better.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[gio1]

I have done some research.

1- You are right in saying that Ansys (which I have heard of, but never used) provides a surface to surface contact algorithm based on gauss points. This overcomes the problem I mentioned regarding high order tetrahedrons

2- I have used several FE softwares and none had this feature. All of these softwares (and not just Abaqus) suffer from the limitation I mentioned regarding high order tets. In Ansys'own words (from one of their brochures) this feature is unique to their software, therefore it is you who are generalising, not me, as Ansys is the exception in this case.

3- I think the bottom line is "For contact analyses always use bricks if you can, unless you have Ansys". This thread was being general and not referring to any particular software, hence my statement on tet elements.

Regards