×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Determining nodal stress from elemental stress

Determining nodal stress from elemental stress

Determining nodal stress from elemental stress

(OP)
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.

RE: Determining nodal stress from elemental stress

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/

RE: Determining nodal stress from elemental stress

(OP)
Dear Blas,

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

Regards
Sarthak

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources