Diference between elemantal stress and elemental-nodal stress

[OmarMR]

Hello

I am doing some analysis in the advanced simulation module of NX6 and I get two diferent stress values, elemental and element-nodal.
I have two quetions about this.

1.- what is the diference between this two stresses?
2.- Which i have to respect to not produce yield in a plastic spring.

Thanks a lot in advanced

 

[potrero]

Without going into very much detail (and subject to better information from others), your finite element model is composed of many elements, which intersect at nodes. Elemental stresses are the stresses experienced on the elements themselves, while element-nodal stresses are the stresses experienced at the ...nodes. It is common, especially for coarse meshes, for elemental stresses to be very different from element-nodal stresses. As you refine the mesh in regions of high stress, you should watch the ratio between elemental and element-nodal stresses as an indication of "convergence". With successive mesh refinements, this ratio should trend towards unity.

 

[BlasMolero]

Dear Omar,
You should look at both values, nodal & elemental stress results. Elemental stresses are computed by NX Nastran at the center of the element, then you will have a single color per element (I like to use the option "Banded" instead "Smooth" to see plain colors).

Users may elect an option in the software that calls for averaging of stresses (simply go to Tools > Results > Post View > Display > Results > Average). This means that stresses from individual elements are averaged at nodes before plotting, so that stress contours have no discontinuities between elements. This is a poor practice because it removes information useful to the analyst. Unaveraged stresses are usually discontinuous across interelement boundaries. A contour plot that displays significant interelement discontinuities warns that a finer mesh is needed.

For instance, two parts joined by a shrink fit have different normal stresses in directions tangent to the interface. And averaged nodal stress would not represnt the actual stress on either side of the discontinuity. Also, a discontinuity of thickness or material elastic module also causes a stress discontinuity.

Best regards,
Blas.

Ah!, point 2): well, I don't understand very well the question, if you have a plastic region, then you have stresses above yielding point of the material ...

 

[OmarMR]

Hello

Thanks for your answers

And I think that my second question is no clear. i will try to explin it better.

I am designig a Spring of Acetal copolymer and I want to make that the spring can deform 10 mm and tha it do not research the yield strength of this material. And I do not kown if use the elemental or elemental nodal stress because both are diferent.

I deduce from your answers that I need a finer mesh. Is it correct??

Thank a lot in advanced for your help

 

[BlasMolero]

Dear OmarMR,
At the limit elemental & nodal stresses will converge to a closer value, then you need to create a quality mesh, use minimun 6 elements per 90 degrees. Of course, forget at all tetrahedral elements CTETRA, instead use 3D solid brick hexaedral elements CHEXA of 8-nodes, and in case of running the NX Nastran Advanced Nonlinear (SOL601) solver mesh with hihg-order CHEXA 20-nodes elements and convert to bricks mixed-interpolation "u/p" 27-nodes elements using ELCV=1. Some basic element recomendations:
• Use always elements with midside nodes when bending effects are significant, specially when element distortion is expected to be large.
• Avoid the use of 4-node tetra elements in general.
• For contact analysis, contact surfaces on 8-node brick and 27-node brick u/p elements are better.
• Use ELCV=1 to convert 20-node brick elements to 27-node brick elements, strongly recommended for contact analysis and also recommend with u/p elements, either rubber materials and other almost incompressible analysis (plasticity, creep, Poisson's ratio ~0.5).

Best regards,
Blas.

Best regards,
Blas.

 

[potrero]

@Blas,
Can you provide references to support your recommendations? Thank you.

 

[BlasMolero]

Dear Potrero,
The above Element recomendations should be followed by any user of NX Nastran Advanced Nonlinear module (SOL601/SOL701).

SOL601/701 module support different types of elements, let`s say that pure displacement based elementes are the simplest. However, in many cases they are not accurate and are replaced by other options:
• Incompatible modes (bubble functions): for 2D, 3D and shells.
• Mixed u/p formulation (involves mixed interpolation of displacement "u" and pressure "p" in order to avoid volumetric locking): for 2D and 3D elements.
• MITC elements (Mixed Interpolation of Tensorial Components): for Shells.

These element features are needed to provide a robust solution. You have plenty information in the Advanced NonLinear Manual of NX Nastran.

Best regards,
Blas.