C3D10M integration points

[jisb]

Hello,

Could someone explain to me how I should report values (e.g., maxPrincipal nominal strain values) for a particular element? I noticed that for C3D10M element, there are 4 integration points, and each has a certain value. How do people normally report? Average across these 4 values? Sometimes I see that these 4 values could be very different. The geometry in our model is imported from IGES, and can't be meshed into hex elements (in Patran), and I had to mesh in Tet10. THanks a lot!

Sean

 

[johnhors]

Sean

Your question, begs the question "Why ?"

Only a four noded tet the C3D4 will have a uniform stress due to it's linear shape and displacement functions, but as you probably know, don't touch these elements with a barge pole. Whilst the 10 noded tet has parabolic functions and thus a linear variation of stress within the element, how meaningful is an "average element value" and for what purpose bearing in mind that tet meshes contain a jumble of elements with highly variable volumes and shape qualities.

Lastly avoid using the modified version of the Abaqus tet, i.e. use the C3D10 element unless you have contact and then only use the modified tet for those elements in contact. The modified tet is prone to report inaccurate stress values, Abaqus are well aware of this and have been working to improve stress recovery from this element for some time.

 

[jisb]

Hi johnhors,

Yes, I am aware of why tet10 has more than one integration point, and I am aware that these elements are not good for stress precidtions. However, (fortunately, and luckily) we need to predict the strains and displacements instead of stress values. Also, my problem is a dynamic contact problem -- rigid container contains a bowl of soft tissue, things like that, and the only available elements in abaqus is C3D10M -- the modified version of C3D10. :-(

Could you have further comments on the "strain" and "deformation" (displacement) predictions using this element? Thanks very much,

Sean

 

[johnhors]

Sean

Displacement predictions should be good as with all parabolic elements, strain with these elements is just as dodgy as the stress since they are linearly related.

Is your geometry that complex? I mean how difficult would it be to split it into hex meshable regions. Failing that I know of several Abaqus "experts" who all independently of each other tackle these problems using 8 node bricks for contact and ordinary ten node tet elements to model the rest of their models. They interface 4 linear brick element faces in a square with two faces of tet elements for their mesh element transitions. Not perfect, but they all believe that this gives them much better contact, and is preferable to using tied slidelines for the mesh transitions.

 

[jisb]

Thanks.

Actually, our material is non linear: we used hyper elastic materials. So strain and stress are not linearly related.

Yes, our geometry is complex: It's a human head (brain/skull). But I would very much like to learn more about how to partition it to hex meshable regions. Done in Abaqus/CAE? I even couldn't successfully import my geometry (IGES from Rhino): abaqus complains it's a corrupted file (but it worked fine in Patran). Even if I can import my geometry, abaqus/cae says it's not a valid geometry, etc. If you could point me to some related material to handle the element /partition problem, that'll be really great! Thanks again.

 

[johnhors]

Sean

I see your problem more clearly now!!!

The contact methodology in my last post only really works well on mechanical assemblies, like for pins in lugs, gear teeth and cam followers, where it is a relatively simple task to cut the volumes near the contact area into hex meshable regions. One bunch of guys that I know of does use Patran with Abaqus, another bunch uses Femap and yet another uses Cadfix, they all create mixed hex and tet meshes with these softwares. I don't know of anyone using Abaqus/CAE for work like this.

To be brutely frank my experiences with IGES files produced by Rhino are not good, they appear to require a great deal of geometry healing after import, whilst IGES files produced by higher end CAD systems like Catia, ProE, Solid Works etcetera require little if any healing.

Also Abaqus/CAE although improved enormously over the last few releases, it is still poor at importing CAD geometry. The messages that Abaqus/CAE produce about corrupted files, imprecise geometry etcetera are merely a reflection on it's own lack of ability to handle these models and should not be taken as meaning that there is a problem with the CAD model itself.

Finally if you contact the guys at

http://www.damt.co.uk

, they are very experienced in using Abaqus for contact and mixed hex/tet meshing.