×
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

Non-linear modal analysis

Non-linear modal analysis

Non-linear modal analysis

(OP)
hi do you know if it's possible to run a non-linear modal analysis? I have a structure with gap elements and i want to find the first ten eigenvectors. I think that if i used a 103 nastran would convert the gaps in springs

RE: Non-linear modal analysis

Hello!,
Yes, With FEMAP & NX NASTRAN you can perform NON LINEAR MODAL ANALYSIS. You can request prestressed normal modes at the end of each subcase in SOL 106 by adding the following items to the input file.
  • Add METHOD=SID in the subcase of interest. A prestressed normal mode analysis will then be performed at the end of this subcase. The METHOD command points to an EIGRL or EIGR Bulk Data entry which then selects an eigenvalue method.
  • For multiple normal mode analyses in SOL 106, the METHOD command may appear in more than one subcase or above all subcases. In the latter case, a normal mode analysis is performed at the end of each subcase. The stiffness used for modal analysis corresponds to the last step of the subcase. Modal analysis cannot be performed at intermediate solution step.
  • A PARAM,NMLOOP,loopid command must appear in the Case Control or Bulk Data Section to request a normal mode analysis at the end of those subcases with a METHOD command. The actual value of loopid is unimportant as long as it is a positive integer. This alleviates the cumbersome task of figuring out the exact loopid.
  • Add the appropriate EIGRL or EIGR entry in the Bulk Data Section of the NX Nastran Quick Reference Guide
You can also run a modal analysis SOL103 with contact elements, not only node-to-node CGAP elements but also surface-to-surface no penetration contact elements, take a look to this link: http://iberisa.wordpress.com/2011/11/07/analisis-d...



NX Nastran provides a contact capability for SOL 101 linear static analysis, and also in consecutive SOLs 103, 105, 111 and 112. Contact for the SOLs 601 and 701 is also available in the Advanced Nonlinear Module. Contact conditions allow the solution to search and detect when element faces come into contact. The software then creates contact elements, thus preventing the faces from penetrating and allowing finite sliding with optional friction effects.

Contact Conditions in Dynamic Solutions (SOLs 103, 111 and 112)
==================================================================

A contact condition can be included in a normal mode solution (SOL 103), and in an optional dynamic response calculation (SOLs 111 and 112). In the normal mode solution, contact stiffness result is added from the end of the converged linear statics contact solution. The contact stiffness values in the normal mode solution represents the final contact condition of the structure around the contact interface. Thus, it will appear that the resulting contact surfaces are attached during the normal mode analysis. Since the calculated normal modes include the final contact interface conditions, the response calculation (SOLs 111 and 112) which use these normal modes automatically include the same conditions.

The inputs for the normal mode solution are consistent with differential stiffness solutions which require a linear statics subcase. The difference is that the linear statics subcase should include the BCSET case control command. When defining the normal modes subcase, a STATSUB case control command must be included to reference the subcase id containing the contact definition. The contact solution in the linear statics subcase must fully converge before moving to the normal mode portion of the run.

Contact conditions can be used with the element iterative solver. However, differential stiffness conditions cannot be generated with the element iterative solver. Therefore, the default sparse solver will always be used, even when the element iterative solver is requested.

Hope it helps.
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/

RE: Non-linear modal analysis

(OP)
Thanks for your help, you've been very helpful

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