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
- CAE Simulation - Simcenter 3D Forum
- Real Eigenvalues Analysis / Eigenfrequency analysi...

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

01-08-2014 04:34 AM

Hello,

I'm doing a real Eigenvalues Analysis with solution 103. All works fine.

But some things are a bit unclear to me, perhaps someone can help with his experience:

- When refining the mesh, is there a convergence of the eigenfrequency? Does this converged frequency is the one which corresponds closest to reality?

- Are Hex or Tet elements more accurate?

best regards,

Silvan

Solved! Go to Solution.

7 REPLIES

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

01-08-2014 06:56 AM

Hello!

An adequate element mesh is required to create an accurate model. For static analysis the mesh density is primarily controlled by the load paths; the element mesh must be fine enough so that there is a smooth transition of stress from one element to another in the region of interest.

Load paths are also important for dynamic analysis, but there is an additional consideration: **the mesh must be fine enough to accurately represent the deformed shape of the modes of interest**. If many modes are to be considered in the analysis, then the model must be fine enough to accurately represent the mode shapes of the highest modes of interest.**A general rule is to use at least five to ten grid points per half-cycle of response amplitude.**

Another way to verify the accuracy of the mesh density is to apply static loads that give a deformed shape the same as the mode of interest and perform stress discontinuity calculations. This process can be laborious and is not recommended as a general checkout procedure.

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

01-10-2014 08:02 AM

This is an interesting topic for me as Siemens PLM is reviewing its support of adaptive meshing analyses. On the web you will find a good bit of information on adaptive meshing with respect to linear statics. Most methods take an element strain energy error approach to refine the mesh in areas of high stress/strain gradients, thus minimizing the gradients and resulting in a converged mesh for the particular linear statics loading condition.

It is much harder to find information regarding adaptive meshing based upon normal modes results. Each mode produces a stress result, though the magnitudes are arbitrary. For a given mode one can take the same approach as a linear statics stress result, but how do you weigh the importance of one mode over another? The stress results of each mode have to be scaled relative to one another. Then a mesh refinement "map" needs to be created to drive the refinement of the mesh. The map defines where mesh refinement is or is not needed. Individual modal mesh refinement maps takes into account how each mode would want the mesh refined, and those maps must be enveloped to produce a single (i.e. worst case) mesh refinement map. The enveloped map takes into account how all modes are wanting the refinement to proceed. With a single mesh refinement map, a mesher can update the mesh accordingly.

NX doesn't yet support adaptive meshing with respect to normal modes solutions, but it is something we have thought about implementing in a future release. I would be interested in hearing opinions on the value of such capabilities from our users.

Regards,

Mark

Mark Lamping

Simulation Product Management

Product Engineering Software

Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

2000 Eastman Drive

Milford, OH 45150

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

01-22-2014 05:55 AM

Thank you two for your responses, it's a lot of information, but some things are still not very clear to me:

@blas:

You say that also in dynamic analysis one has to make sure that " there is a smooth transition of stress from one element to another".

And that the mesh must be fine enough to accurately represent the deformed shape. I interprete from this that the elements should not be too distorted.

BUT: In my logic the stress transition and the element distortion depend on the amplitude of the vibrational movement. But as the amplitude is an arbitrary result, stress transition and distortion are then also arbitrary...?

Best regards,

Silvan

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

01-24-2014 01:55 PM

Dear Silvan,

The following picture will show you what is important in modal eigenvalue analysis: the element size will be fine enough to capture correctly both the mode shape and obtain accurate resonant frequency results. All depends upon what is required from the results.

If only the resonant frequencies and mode shapes or the displacement modal response are required, then a "relative" coarse model will suffice. However, if the acceleration or stresses are required then a much finer mesh will have to be used. If stresses are being found then the same mesh that would be used for a linear static analysis is needed, OK?.

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/

- Tags:
- element size

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

01-28-2014 02:29 AM

OK, thanks a lot.

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

05-03-2014 10:24 AM

Yes. There is convergence to the "physical" frequencies. Refining the mesh should improve the quality of your results, as your mass and stiffness would be better represented by a finer mesh.

You can make the convergence test yourself: select 4 or 5 different meshes ( say 10k, 20k, 30k, and 50k elements), and then plot frequencies vs number of elements. You would see that your curve is getting to some asymptotic, and the frequency difference decreases as the number of elements increases.

Good Luck

Marc

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

05-14-2014 10:21 PM - edited 05-14-2014 10:22 PM

Marc, this seems like a very complicated proposition, not even necessarly practical... For a couple parts I can see it maybe, but for complete systems, that could be very costly.

We can't quite use detailed stress models for dynamics response, there's always a trade-off, the modeling is what separates the boys from the men :-)

I guess you could put priority between modes by mass participation factor, but then you'd end up with a "good mesh for X excitations", and a "good mesh for Y excitations", ...

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc