Hex vs Tets / different stress level 2

[Dave06fea]

thread727-152330

Hello,

I am dealing with a mechanical model in linear analysis.
The model represents a cylinder made of steel with a top and a bottom flange. The bottom flange is fixed and I apply loads on the top flange. By the way, the cylinder has a hole at mid-height.

Comparing the Hexa-20 model with the Tet10 model (same size), I have got quite the same deformation. But the Max VM Stress is in the wall of the hole for Hexa-20, while just below the top flange for the Tet10. The issue is the Hexa-20 gave me an acceptable level of stress while the tet10 gave higher than my criteria.

Which model is the most realistic?
Thanks.

 

[dwallace1971]

Possibly neither. Without seeing your model, it would be hard to tell. Can you post a couple of images so we might have a look at it?

"On the human scale, the laws of Newtonian Physics are non-negotiable"

 

[rb1957]

at least you didn't use TET4s.

why model the side of the cyclinder as solids ?
why not plate elements ??

are you looking at element centroid stresses ?
how do the nodal stresses compare ?
is the mesh size the same ??

 

[inline6]

post some images/screen grabs of the mesh so we can comment

 

[BlasMolero]

Hello!,
Of course, not doubt at all, use CHEXA 20-nodes high-order elements forever and ever, whenever you can use HEX elements instead Tetraedral, not comparison at all in the quality & accuracy of results, specially in surface-to-surface contact problems.

The problem you experience can be explained because TET meshing is automatic meshing, anarquic meshing, then this "anarquic" in the mesh cause, for instance, that symmetric stress results are not exactly symmetric, the effect is evident when using coarse mesh. But with CHEXA elements always you will have symmetric results. Please note you need to make sure to have minimum two elements in the wall thickness to capture stress gradients.

Also, another important reason is the model size: the same model meshed with TET10 elements using exactly the same element size is between 5-to-10 times bigger than the same model meshed with CHEXA 8-nodes elements, then the size does matter in fea, specially counts in nonlinear analysis!!.

In summary, HEX elements are my favourite, of course. And when dealing with contact problems I use in NX NASTRAN the 27-nodes CHEXA elements using the ELCV=1 parameter that converts automatically (at solver level) 20-nodes CHEXA elements to 27-nodes hexaedral elements:

In the following picture you can see a complex contact + material + geometric nonlinear problem, forgot at all to use here TET10 elements:

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Dave06fea]

Thank you BlasMolero for this explanation.
Could you please remind me how to calculate
the DOF of a model?

 

[BlasMolero]

Hello!,
Is easy: count the number of nodes of the model and multiply for the number of DOF of the elements: if your model is fully meshed with 3D solid elements, then the total DOF of the model is = total no. nodes x 3 (Shell & Beam elements have 6 DOF per node). The number of equations to solve is the total number of DOF less the DOF constrained nodes.

Best rgards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Walterke]

What an awesome model. How do you make the deformable part contact itself? (bottom right part)
Also: how long did it take to calculate?


NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

 

[BlasMolero]

Hello!,
This nice feature of "self contact" is a great capability of the module NX NASTRAN Advanced Nonlinear solver, you have more pictures here (tutorial still unfinished):

http://www.iberisa.com/soporte/femap/nolinealavanzado/shiftboot.htm

The key is to use the same region as source and target contact. Regarding solution time, I don't remember, but not too much, thanks to the use of CHEXA 20-nodes elements this is small model.

Best rgards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[irq]

Why do you select second-order elements for hyperelastic materials? They are susceptible to volumetric locking, therefore stiff when modelling incompressible materials. There are certain recommendations to use the lower-order elements for large strain analysis, especially for hyperelasticity and plasticity.

 

[BlasMolero]

Dear IRQ,
Please note this is a "severe" contact problem, then when dealing with contact the use of ELCV=1 to convert 20-node brick elements to 27-node brick elements is critical. It is recommended with u/p elements (either rubber materials or UPFORM=1), and strongly recommended for contact analysis.

Is well know that the use of incompatible modes improves the bending flexibility of 8-node brick and 6-node wedge elements, but when mixed interpolation (u/p) element is used, the incompatible modes option is not used.

Here I used Mixed u/p Formulation, then for you to know a few key points:
• Involves mixed interpolation of displacements (u) and pressures (p) in order to avoid volumetric locking.
• Much more reliable than reduced and selective reduced integration.
• Satisfies the Inf-Sup incompressibility condition where possible.
• Number of pressure degrees of freedom depends on element.
• Pressure degrees of freedom are internal to the elements. They do not increase the size of the global unknown vector.
• Always used for hyperelastic materials (except hyperfoam).

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/