turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Simcenter 3D Forum
- Eigenvalues with load

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-02-2016 04:03 AM

Hello everyone,

I have to determinate eigenvalues of a system under different conditions. The system has a fixed constraint and it is under load (mass load).

Howewer, the 103 solver doesn't allow to apply a load condition, and my question is very simple, how can I apply a load on my system ? Or maybe I don't use the right solver, and if it is that, which solver do I have to use (101,103 ...) ?

Thank you !

Arthus

Solved! Go to Solution.

Labels:

6 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-02-2016 04:31 AM

Dear Arthur,

If loading (mass load, in this case) do not stiffen or soft the structure, then non sense to think in consider any preload effect in the NX NASTRAN eigenvalue analysis (SOL103), think in the strings of a guitar, here the pre-load in the string can change its frequency, of course!!.

When you perform a SOL103 analysis you get the natural frequencies and mode shapes of the structure, **that are functions of the structural properties and boundary conditions**. A cantilever beam has a set of natural frequencies and associated mode shapes. If the structural properties change, the natural frequencies change, but the mode shapes may not necessarily change. For example, if the elastic modulus of the cantilever beam is changed, the natural frequencies change but the mode shapes remain the same. If the boundary conditions change, then the natural frequencies and mode shapes both change.

For example, if the cantilever beam is changed so that it is pinned at both ends, the natural frequencies and mode shapes change, OK?. In you case, if you change the mass value the natural frequency changes, but the mode shape is the same, unless you change the location of mass.

**SOL103** analysis is usualy the first step in performing a dynamic analysis to determine the natural frequencies and mode shapes of the structure **with damping neglected**. These results characterize the basic dynamic behavior of the structure and are an indication of how the structure will respond to dynamic loading. The next step is to excite the structure and perform the dynamic response either in the time domain (modal time history or dynamic transient SOL112 analysis) or in the frequency domain using a modal frequency response (SOL111), as well as other DIRECT methods.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-02-2016 04:48 AM

Dear Arthur!,

A common mistake about mode shapes from a SOL103 analysis is that they define the structural response, wrong!!. Mode shapes are relative quantities, they cannot be used alone to evaluate dynamic behavior, it is the relation between the structural loading and the natural frequencies that determines the absolute magnitude of dynamic response.

The relation of a specific loading to a set of natural frequencies provides explicit scale factors that are used to determine the extent to which each particular mode is excited by the loading. Modal frequency response analysis and modal transient response analysis are modal methods (or modal superposition methods) that use the modal results to determine forced response, OK?.

For instance, **Modal Frequency Response Analysis (SOL 111) **is a method to compute frequency response. This method uses the mode shapes of the structure to uncouple the equations of motion (when no damping or only modal damping is used) and, depending on the number of modes computed and retained, reduce the problem size. Because modal frequency response analysis **uses the mode shapes of a structure**, modal frequency response analysis is a natural extension of normal modes analysis.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-03-2016 08:54 AM

It sounds like you want to compute prestressed normal modes. This requires two subcases. The first subcase is a static subcase that contains your structural loads. The second subcase is the normal modes subcase. You add a STATSUB=x (where x is the subcase ID of the previous static subcase) to the normal modes subcase. This tells Nastran to add the differential stiffness computed in the static subcase when computing the normal modes.

See STATUSB in the QRG for more information.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-06-2016 02:14 PM

I concur, Dr. B :-)

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-06-2016 03:59 PM

@Jim B ,This is also called stress stiffening

Amit Nandi

Application Engineer, DesignTech Systems Ltd.

Application Engineer, DesignTech Systems Ltd.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

05-06-2016 04:23 PM

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc