Quality of Tet meshing

[OptiEng]

Hi,

For a particular problem, I am resulting to using quadratic tet meshing due to the geometry of my model becoming is likely to become more complex through optimisation, and partioning may become inefficient. However, I am quite concerned about the accuracy of the results (see attached) file. I am using C3D10M elements, and advice would be much appreciated. I have read to avoid using linear tet meshes, but also have seen exmaples where quadratic tets are comparable to hex in terms of accuracy.

Note. I repeated problem using hex elements with similar mesh density a obtained a much smoother stress distribution. This is a structural problem with small deformation of an assumed linear material.

Many Thanks

 

[johnhors]

You are looking at stresses on a sharp corner, this is a singularity. You cannot seriously expect good results here with either hex or tet elements. The fact that hex elements appear to present a smoother contour plot does not make the results any better. You can put a fillet radius in the geometry or at least a chamfer to improve confidence in the results.

Additionally, the modified tet element C3D10M is known to be inaccurate at stress peaks, producing higher stresses than the standard tet element.

http://www.Roshaz.com

 

[OptiEng]

Hi Johnhors,

Thanks for you very much for your feedback, the thing is... it is a circular hole, not a sharp corner sorry if this is not clear from the image attached.

P.S. I agree with you on the C3D10M, it shows, higher stresses at the edge of the hole than is shown by the hex elememt model.

Regards

 

[corus]

As johnhors hinted at, the problem is having confidence in the results, and you don't have that with tet elements and the irregular contours produced.
With difficult geometry it's sometimes useful to mix the element types. Where you just require some continuity of the structure to carry the loads, and the geometry is difficult, then partition the area off and use tets in the difficult areas. In more regular areas (such as around the hole), and where you're more interested in the stresses, them use hex elements. You can refine the mesh in that area for greater accuracy, and still maintain smooth contours that are more 'believable'.
The disadvanatage is Abaqus will tie two neighbouring regions of different element types, so the stresses at that juncture will appear irregular there. The advantage though is that you'll reduce the number of nodes considerably.

Hoping to say Tata

 

[gwolf2]

As jh says - you have modelled a singularity, the stresses are random numbers - if you refine the mesh the stress will just increase to infinity. You must put whatever true geometry is there into your model to get the correct concentrated stress.

 

[johnhors]

OptiEng, you have a 90 degree corner in a high stress region, I would believe that the real component has a chamfer, you should include this in your modelling.

http://www.Roshaz.com

 

[OptiEng]

Thanks everyone, I looked up singularity and it seems to mostly be a problem with crack problems. In reality it would like to have 45deg chamfered edge on it to aid shaft insertion.

I have remodelled with a chamfer but still seem to get irregular stress distribution at the hole edge. I will try some other element types.