Determining nodal stress from elemental stress

[smsarthak]

Hello everybody,

I am trying to determine nodal stress from element stress already calculated during analysis.

Attached is model I was trying to verify.
This model is a flat plate and a pressure is applied on the plate. The maximum bending stress shall be 75 MPa and the minimum stress shall be 0 MPa. The output vector seems 7021 seems to calculate values at gaussian points, which is 74.6 MPa, less than 75 MPa.

I have already tried Model > Output > Process > Convert Tab. The output vector 9000000: Converted Vec 7021 is created. But it also shows the same results as Vec 7021.

Kindly tell if I am making any mistake in creating this new vector.

Thanks in advance.

 

[BlasMolero]

Hello!,

For CQUAD4, CTRIAR, and CQUADR plate elements, element forces, stresses, and strains are only calculated by NX NASTRAN at the centroid. You have the option to compute and output these quantities at the corner grid points setting the "Element Corner Results" customization at the NASTRAN Output Request in FEMAP. Then, to obtain the corner stresses in addition to the centroidal stress, you should request:

Please note for the CTRIA3 element the corner option is ignored for this element.

To activate the output at element corner results you need to activate it in the "nastran output request":

If you re-run the analyss and plot elemental vonMises stress you will see the following value: please note the options selected in the CONTOUR OPTIONS window: contour type = elemental, NOT use of corner data, and not to perform smart averaging (well, in this case is the same because not element discontinuities for material, thickness or element orientation exist). Also, in the previous window SELECT POSTPROCESSING DATA activate the option DOUBLE-SIDED PLANAR CONTOURS, this way you can see in ONE plot (simply rotating the FE model) both stress results in TOP & BOTTOM faces for Shell CQUAD4 elements:

To plot NODAL STRESS results simply activate CONTOUR TYPE = NODAL and also activate the option USE CORNER DATA:

The above demostrates how to see in FEMAP both nodal & elemental vonMises stress results in plate CQUAD4 elements, OK?.
Best regards,
Blas.

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

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[smsarthak]

Dear Blas,

Thanks a lot for your detailed reply. Was of great help.

Regards
Sarthak